# 30cc Inline Twin 4-stroke Engine based on Westbury's Wallaby



## Eccentric (May 21, 2021)

My next engine build will be a derivative of Edgar Westbury's Wallaby, first designed for a model train, then updated for use in a model hydroplane.  The engine is an overhead valve, water cooled, 30cc, inline twin cylinder  4-stroke. My version will use no castings.

I am a huge fan of Edgar Westbury's work as a model engine designer. He was very prolific producing designs optimized for construction by the home machinist with minimal tools, typically a small lathe and a drilling machine.  His first engine design was published in the 1920's, a single cylinder 2-stroke for a 13 foot wing span model airplane.   He joined Model Engineer magazine in the early 1930's and went on to publish many wonderful engine construction articles as well as several books on machining.

This is a video of a classic Wallaby: 

Construction articles for the Wallaby are available from the "Model Engineer" magazine and have been in the public domain for decades. Anyone needing help locating them, feel free to PM me.

The engine has a bore of 1 inch and a stroke of 1-1/8 inches.  It has a built in oil pump to provide pressure fed lubrication to the tappets, crank shaft center bush and the connecting rod big ends. I have redesigned the Wallaby to be machined from raw stock, using no castings, and I will be using ball bearings on the crankshaft, camshaft and timing gears.

I use SolidWorks  for my computer aided design work and Fusion360 for tool path generation.  I first fabricated 3D printed models before committing myself to cutting metal.

The original Wallaby had 5 main castings: the Body Casting, Sump, Cylinder Head, Cylinder Head Plate and Timing Cover.

I have split the Body Casting into three machined parts, the crankcase, rear timing plate and the block. I learned the technique of separating the crankcase and the block from Terry Mayhugh's build of Ron Colona's Offy.  When designing a casting, a good engineer will strive to incorporate as many features as possible. This will reduce total part count and reduce cost of a mass production, but results in a very complex part, making it difficult to machine a one off.  The Cylinder head has many internal passages that make it a good candidate for a casting, but difficult to machine, so it will likewise be made as two parts to be bonded later with high temperature structural adhesive.

Other design changes include the use of bearing housings for the crankshaft end bearings and the camshaft bearings.  This will allow me to fabricate these precision components on the lathe independently from the machining of the crankcase.

-------------------------------------------------------------------------

My first Goal - Machining the Large components:


Sump
Crankcase
Block
Timing Back Plate
Crankshaft Main Bearing Housings
Dummy Crankshaft
Camshaft Bearing Housings
Dummy Camshaft





*                                Assembly model of only the large components*






*                             Another View






3D Printed Mockup of the engine















*

Sump

I have decided to machine the sump first.  It is the second largest part and has many of the same shapes that will need to be machined into the crankcase, so will provide good practice developing the tool paths, tool selection as well as the speeds and feeds.  The sump is less critical dimensionally than the crankcase.  The crankshaft center bearing is held exclusively in the crankcase and the sump only holds the two bearing housings for the crank case, but will rely on the crankcase for alignment.  There will be two locating pins where the sump and the crankcase mate to provide positive, repeatable alignment between the two and the crankshaft bearing housing mating surfaces will be machined from the same setup to provide the best alignment.

Datums for the sump, Top, Right side and Front

Machining Steps


Flatten top and Right side of the work piece and insure they are perpendicular
Mount the work piece in the vise with Top against the vise face and the Right side down against parallels - machine left side at least .05" over dimension.
Mount work piece in vise with the Top against the vise face and the Front down and machine the back side at least .05" over dimension.
Mount in the vise with the right side against the vise face and the top down.  Machine the bottom square at least .05" over dimension.
Take to drill press and drill a 1/2" hole from top, center of sump measured from Right side +.02", from Front +.02", and 1.5" deep (which is more than 1/8" from inside bottom of sump).  this hole is the starting point for the end mill to machine the inside.
Mount in the vise with the Right side against the vise face and the top up.
Machine the inside of the sump.  See detail below.
Center drill all holes
Drill all holes to depth including the two alignment holes. The alignment holes reamed to 1/8" interference fit.
Flip part over with Top against parallels, and the Right side against the vise face.
Machine minimum clearance for crankcase bolts, leaving the majority of the material to be removed later.
Lightly sand the top surface of the sump on a flat surface with 180 grit, then 320 grit and finally 600 grit to create a flat clean surface-don't get carried away, enough to just remove tooling marks.
After these steps, the sump is compete for now and is ready to be attached to the crankcase for the machining of the front and back. 3D  modeling programs allow "configurations" of models to be created that are derivative or different than the base part.  I use this feature to create modified versions of the model to optimize the machining, creating both models specifically modeled for a specific machining operations as well as special configurations of the stock material.  This is nice because as design changes are made to the base part, they are carried forward into the derived parts.

Detail of sump machining operations - A special 3D model is created for the machining of the top of the sump, it has the following modifications:


All features are removed from the Front and Back.
.020" of material has been added to Front and Right side.
Corner fillets removed.
Oil drain hole in bottom removed.
A special model is created for the raw stock, it has the following characteristics:


square block, .020" over sized on the Front, Back, Left and Right sides.
Has a 1/2" hole 1.5" deep in the middle of the sump for the 1/4" end mill that will be used to remove the majority of the material to start in.  End mills are great at cutting on their side, but not so good at machining down.  By machining from the side of the part, or from a predrilled hole on an interior feature, the pocket machining operation can remove more material, quicker, with less stress on the cutter.
*




Work piece locked in the vise ready to machine the inside of the sump.  The 1/2" hole is used for an entry point for the end mill.*​*




Modified model for machining the inside of the Sump.  Compare to sump model above.





Finished inside machining of the sump






Finished bottom machining of the Sump. The sump can now be bolted to the crankcase for further machining.*



Lessons learned:


I added .020" of stock to the top of the model that was machined off during the first horizontal milling operation.  I then switched tools and touched off on the top of the model and my tool path was then .020" too deep.  I noticed quickly, but there is an area on the back where the main bearing mount is .020" too deep.
When machining the bottom I had problems with the work piece remaining securely clamped in the vise.  It was moving during machining.  I need to experiment, it may of been due to the fact that the work piece was hollow between the vise jaws, it might have been I just didn't have the vise tight enough, it might have been I did not have a three point clamping points, or I did not have enough of the work piece in the vise.
Should have used a smaller step over when using the 1/4" ball end mill on the main bearing housing surfaces.
Things that worked well:


I used a two flute 1/4" flat end mill at 8,000 RPM spindle speed, coolant, 15 ipm and .050" depth of cut.  I was happy with the rate of material removal and the finish.
I did not use a ball end mill on the inside of the sump.  My thinking was no one would see the inside, so smooth surfaces were not worth the machining time.  However, the surface turned out acceptably well with just with the 1/4" flat end mill.
When cutting deeper than the cutter flute length (.75" in my case), I step the material out .010" in the model to prevent the sides of the tool rubbing.  This effect can be seen in the deep channels cut in the sump bottom.


----------



## Mechanicboy (May 22, 2021)

Hi, you can cast the engine block and other engine parts when you are use the 3D printed pattern in the cast sand and pour direct into, then the pla will burn away. It save a much time.


----------



## Jasonb (May 22, 2021)

Also look at what notch you had the vice cross bar in as you can end up with more force going downwards rather than sideways if it is too close to the fixed jaw. I tend to only use my one of these vices where I need the height or jaw opening as I've had stuff move the rest of the time I use a Kurt Copy on the CNC as I find it gives a better grip.

An Adaptive type tool path will give more even wear along the side of the cutter when clearing out the waste in parts like the sump, spiral down say 0.2" each stepdown and then cut using 10-15% of the cutter diameter, set a fine stepdown of of say 0.05" to get the final stepping of the contour.

For something like the bearing housings I would leave metal on them and line bor the two halves when bolted together.


----------



## Eccentric (May 23, 2021)

Jason,

Ahh, I see.  that makes sense what you say about the vice cross bar and the direction of force depending what notch it is in.  I had not thought of that before.  I have limited Z and a Kurt style vise is too tall for my machine.  

I will try your suggestion regarding the use of more of the side of the cutter (.2" vs .05") with smaller % of the cutter used each pass.  thanks.

I agree with you and will line bore the crankshaft bearing surfaces, I have not done this before so it will be yet another adventure.  Mounting the engine perfectly in line with the spindle on the cross slide seems daunting.

Mechanicboy,

I like you casting technique.  Casting is something I would like to learn how to do at some point.  Right now I still have alot to learn about machining.  thanks for the post.


----------



## Eccentric (May 28, 2021)

Working on the top crankcase.  Here is my plan:

Square the stock up on all sides in the lathe.
Drill the camshaft hole through the work piece, working from both the front and back, .05" undersized.  Use the bottom and right side as the datum.
Mount in the mill and using the bottom and the right side as datum, drill and ream the camshaft bearing holder holes from each end.
Drill a 1/2" hole approximately in the center of the cylinder as a clearance for the flat end mill to enter.
Mount in the vise with the bottom up and the right side against the vise face
Machine the bottom using a 1/4" flat end mill. Touch up the crankshaft bearing holder surfaces with a 1/4" ball end mill.  Used a .200" step down ( .050" fine step down) with a .050" side cut. 1 hour, 16 minutes total machining time.
Machine three flats on the center bearing holder surface, one for a center oil hole and the other two for the middle camshaft bearing mounting screws.
Mount in the vise with the top up and the right side against the vise face and machine the top with a 1/4" flat end mill. 28 minutes machining time.
Center drill, drill and tap the 6 block mounting holes.




Squaring up the stock in the lathe.  I left it over sized, but did not need to "re-square" up the work piece after the camshaft hole was drill and reamed.





Finished bottom machining.  You can see small steps .0745" down.  the wall sides are .010" thicker so the 1/4" end mill can mill deeper than its .750" flute length.  this keeps the mill shaft from rubbing.





Machining the crankcase top surface






I also worked on the block, I brought it to exact dimension on the lathe before machining out the inside.











The engine so far.


----------



## Eccentric (Jun 1, 2021)

The cylinder head is one of the more complex parts due to the fact that there are 7 different surfaces that need machining, five on the outside and two internal, and they must all align as well as possible.  The tools that are used include a 1/4" end mill, 1/8" end mill, 1/4" ball end mill, 3/32" ball end mill, spot drill and drills. I did some significant redesign of the head making the following changes:


Used larger, yet more cost effective, CM-6 sparkplugs.  I had to juggle their position to clear the head mounting screws.
I like to use complete bronze valve cages which incorporate the valve guide and the valve seat.  the original design has the valves seat directly into the aluminum of the cylinder head.
Moved the water jacket holes to give as much clearance to the cylinder head holes, that is maximize the amount of head gasket material between the holes, the edge and the combustion chamber.
Rotated the exhaust flanges so the mounting holes do not hit the seam of the top and bottom halves.  I don't want the flange mounting screws putting a separating force on the two halves.
Adjusted the sparkplug depth and angle to give good access to the combustion chamber, but not interfere with the valve guides.
Maximize the water jacket volume without compromising wall thickness.
In order to machine the internal passageways for the air/fuel mixture and the exhaust gases, I decided to fabricate the head from two pieces bonded together.





*3D Model of the one half of the cylinder head showing internal passageways*

 My plan evolved as follows:


square up two blocks of aluminum, .25" oversize from front to back and from left to right.  Exact dimension top to bottom.  Total height of the head is .875, bottom half is .475" thick and the top is .400" thick.
Machine internal passages. roughing will be done with a 1/8" end mill entering from the outside of the work piece leaving .010" material. All radii are .1875", so a 1/4" ball end mill will be used for the final finishing passes.  Total machining time is 34 minutes per half.
install locating pins located in the excess material
bead blast the internal passages and the mating surfaces, this increases the surface area for the adhesive.
Bond the top and bottom halves of the head using structural adhesive and a sprinkling of 80 grit glass beads.  this insures there is a micro space between the halves and the adhesive does not get squeezed out during clamping. Loctite EA9340 is used as the structural adhesive.  It has excellent resistance to chemicals including fuels and coolant and is rated to a very high temperature.  The alignment pins are used to insure proper alignment, but the three .375" internal passageways can also be used to align the two parts by installing matching dowels. Note:  Using the glass beads did not work as they were too big and the two parts just slid around on them like ball bearings and the adhesive would have to be much thicker than I wanted.  I ended up just bonding clean parts, but was careful to moderate the clamping force so as to not squeeze out the adhesive.
After the adhesive is cured, square the parts up to proper dimension all around.




*The two starting work pieces next to a 3D Printed model of the head*





*Roughing out the internal passageways with 1/8" end mill*






*Internal passage ways after finish machining with 1/4" ball end mill.






Cured cylinder head work piece, machined to proper size all around.





Machining of the internal water jacket from the top. *

The cooling and mounting holes are machined from the bottom as this is the critical mounting surface with the block.  I used a 1/4" and 1/8" flat end mills to machine the top.  I did not worry about the aesthetics as it will be enclosed and the roughness will not have a material effect of the coolant flow.  This is in contrast to the fine finish machining of the air/fuel and exhaust passages that need smooth air flow and thus justified the additional machining time.





*Machining the underside - combustion chamber, valve guide holes and water jacket holes.  I used a 1/4" roughing end mill, a 1/8" finishing flat end mill and a 3/32 ball end mill for the sparkplug hole.





Finished machining the bottom with the head mounting holes complete.  *

The mounting holes were spot drilled and drilled through using peck drilling.  this is where the drill bit enters about a diameter of the drill bit then retracts and clears the chips, working its way "peaking" through.





*I was very happy with the alignment of the internal passages and the valve guides.





Simple jig to provide the proper angle for the machining of the spark plug holes.  *

A 3D model was created for the machining of these holes using the top edge, closest edge as datums.  I am not sure about the proper use of the word "datums" in this context, data is plural for datum, any way I used these edges as my zero points for machining.


----------



## Eccentric (Jun 1, 2021)

Machining is complete.  I was happy how the external and internal sparkplug holes met.  I did not want to machine the spark plug hole all the way through from the outside as it gets very close to the valve guide, so I machined the internal spark plug hole with the same set up as the valve guides.






Finished Head after bead blasting.  I masked the bottom surface, not sure why, probably doesn't matter one way or the other.






Complete head, all holes drilled and tapped.


----------



## Jones (Jun 1, 2021)

Great idea bonding the cylinder head together from 2 parts!

Roy Amsbury's V8 used a built up cylinder head as well, though it's silver soldered brass, so it has been done before successfully


----------



## kuhncw (Jun 1, 2021)

Very nice work and a good detailed explanation of your process.  Will the plate that seals the top of the head be removable or permanently attached.

Chuck


----------



## Eccentric (Jun 8, 2021)

Chuck,

The Cylinder head cover plate will not be permanently attached, but held down by the same studs that secure the the cylinder head to the block.  I am working on the head cover plate now.


----------



## Eccentric (Jun 8, 2021)

I am trying a new clamping technique I have seen Terry Mayhugh use to machine flat backed parts that require machining all around the outside boarder- temporarily bonding the work piece to a chunk of MDF. My usual way of machining a part like this is to clamp the work piece to the table with some sacrificial material behind it and clamp beyond the machining   boundary.  I leave tabs connecting the final piece to the work piece so that the part is held during all machining operations. The problem with this is that these tabs require post machining operations to remove them. I usually cut  them off with the band saw, then hand file the last remnants of the rough sawn tab.  I am not very good at this and usually file some of the surrounding area or do not get a good blend where the tab was.  I figured the Cylinder head cover plate would be a good part to experiment with-it is about a 1/4" thick and 1.75" X 3.25".



I first used the fly cutter to get a nice flat surface on the back side of the part, then used 5 minute epoxy to bond the flat side to a block of MDF.  I made the MDF block narrower than the work piece so I could use some shims to space the work piece up from the vise jaws and use them to establish my Z axis zero point. I did not clamp the work piece to the MDF, but instead laid a thin film of epoxy on both the MDF and the work piece, them lightly pressed them together to remove all air.  Clamping has a tendency to squeeze out the epoxy and I am not interested in maintaining a dimensionally accurate bond as I will be spacing the work piece off the vise, not the MDF.





*Using a fly cutter to prepare a flat rear surface





5 minute epoxy to secure MDF to work piece*

I am concerned about the use of coolant while machining as MDF acts like a sponge, soaking up water, swelling and losing all dimensional stability.  I fear that using even a light misting may cause problems as the machining operations will be about 45 minutes. On the other hand I don't like running roughing operations where I am removing a far amount of material quickly without coolant; the cutter will load up as the temp of the work piece rises.  In the end I rubbed the MDF down with light machine oil and used a small mist of coolant.  Let us see what happens. 





*Work piece clamped in the vise with parallels used to provide proper spacing from the vise*

OK, lessons learned.  Using both sides of the vise to level a work piece does not work.  In my case the clamping jaw is taller than the stationary jaw and the part was machining uneven.  I noticed this early so I switched to using parallels under the MDF as is traditionally done.  However, due to my caviler bonding process, that is using no clamps, the bottom of the MDF is not representative of the plane of the back of the work piece.  Also when I switched to parallels, the work piece was lowered and I did not reset my Z axis zero, so the through holes did not go quite through the part.  this can be seen in the last picture below.

 Oiling the MDF was not sufficient to prevent water damage,  As seen below the outside of the MDF swelled .055".





*MDF absorbed moisture and swelled even though only a light mist was used for cooling*



Evidence of the swelling of the MDF can been seen in the final part.  The final machining operation used a 1/16" flat end mill and the part rose with respect to the cutter by a total of .023" between the commencement of the machining and the end.





*.023" trough due to the MDF swelling and the work piece rising during the machining process.*

So where do I go from here?  I do like the idea of using MDF as a machining substrate as it is much cheaper than using a piece of sacrificial aluminum, for example.  The part I attempted the technique with was relatively small and a little moisture on the MDF and the resultant swelling had an outsized impact on the final result.  Do I attempt to seal the MDF somehow?  Paint?  Is it becoming more trouble than the effort saved?  I have further experimentation to do.


----------



## kuhncw (Jun 8, 2021)

Quote: "The Cylinder head cover plate will not be permanently attached, but held down by the same studs that secure the the cylinder head to the block. I am working on the head cover plate now. "

Thanks.  

Chuck


----------



## Eccentric (Jun 23, 2021)

This installment will discuss my process for finishing the outside surfaces of the crankcase and the sump.  I have found that it is advantages in my workflow to first create a perfectly square work piece to all of the max outside dimensions.  In the past I have left extra material on to be machined off at later stages only to mess up because I misremembered what side I left material on, or what the new datum was supposed to be. In hindsight I would have made an exception with the top of the block and left some extra material so I could fly cut the deck after the cylinder sleeves are installed.






Here is the squared up stock roughed out using a fly cutter on the mill.

I have recently been using a new technique, importing a model of the stock into the CAM program creating the tool paths for machining on the CNC router.  The program considers the stock to have been machined by a previous machining operations.  I am using the free version of Fusion 360 CAM and am pleased with its capabilities (albeit limited).






I create a simple drawing with the necessary dimensions that I machine to using the DRO on the mill.






Once I rough out most of the material on the mill I clamp it to the CNC router bed and machine.  I use a 1/2" drill bit and a 1/4" HSS roughing mill at about 1000 RPM on the mill, a 1/4" carbide end mill running at 8000 RPM on the CNC router, then a 1/4" carbide ball end mill to finish the final profile.






I spot drill using the CNC router in the same setup as the main bearing surfaces to insure proper placement.  I then take the work piece back to the mill to drill the holes as the CNC router has a very limited Z and does not have room for a tool holder, chuck and drill bit.






Here I am roughing out the bottom of the sump on the mill.











When touching off the part, I do not use just the edges, I will touch off both ends of the part, move the axis to the middle of the two touch off points and then set the DRO to the center dimension of the final part.  This way if there is any discrepancy between the drawing and the true dimension of the work piece, the difference is split between the ends and is far less noticeable.






The parts just off the CNC machining the outside profiles.  Here I use a .010" step over with the 1/4" ball end mill.  It takes about 45 minutes a side.  If I reduce the step over, the machining time increases linearly, and if I increase the step over the machined surface is not as nice.  I find that .010" step over is a nice compromise.  We will see how well the sides clean up and look after bead blasting.






On the sump I machine the two sides  and the bottom, each in a different setup


----------



## Eccentric (Jun 27, 2021)

The cylinder  block starts with a trued up work piece of 6061-T6.  This was done on the lathe, but could have been done with a fly cutter on the mill.  After using both, I get more accurate results in the mill, but not quite as nice a finish---probably could if I were more patient.






The first machining operation is from the side to create the internal cavity. I spot drilled the location of the block cover screw holes.  In hindsight I would not have done this as I ended up match drilling these holes using the cover plate.  My fear was that if I used the spot drilled holes and the cover was slightly out of position, it would interfere with the block to crankcase mounting.



If you look closely at the cavity in the block, you can see a .010" step where the depth of cut exceeded the .75" flute length on my cutter.  This technique allows me to cut deeper than the flute length without hitting the shoulder of the cutter.






Next, all of the machining from the top was done in one setup.  The large holes for the mounting of the cylinder sleeves were machined at the same time with the same tool to insure concentricity of the hole at the top and bottom of the block. The hole at the bottom is .004"  smaller to ease the installation of the sleeve and allow for a cutter to machine only one of the surfaces, top and bottom, at a time.  In hindsight I would have left a bit of excess material on the top of the block and used a fly cutter to deck the top after installation of the cylinder sleeves.





A dime for scale, the block is really quite small.



The block cover only required machining from one side so was a relatively easy part to fabricate.  I used a roughing pass with a 1/4" flat end mill, a horizontal finishing pass with the same end mill and finally a roughing and finishing pass with a 1/16" flat end mill.  this last operation milled the fins and all of the holes.






As mentioned earlier I decided to match drill the holes for the 2-56 cap head screws mounting the block cover to the block.  This was done to make sure the cover plate does not interfere with the mate to the crankcase or the cylinder head.  I used two .006" shims against a second set of parallels.   Since I had previously spot drilled the block and did not want the drill to find these and follow them, I first ran a clearance drill through the hole to create a new spot for the drill to center on the hole before drilling for the tap.






 As a rule I don't like match drilling, I believe in building to print.  But there are cases where the required precision is too tight to call out on a print and not realistic to call out for fab in my home shop.  Other parts where I will match drill include the main bearing housings to the crankcase and sump.






Here I am using the mill to tap the 2-56 holes in the block.  A spring loaded tap guide is loaded in the mill chuck.  I had to replace the spring in this guide with one much softer as the original provided too great a force for a tiny 2-56 tap.  I used the DRO to locate the holes for drilling and tapping.






The block cover in place.  I think the block looks really cool, I got the idea for this design from Terry Mayhugh's build of Ron Colona's Offy.






The engine so far.


----------



## kuhncw (Jun 27, 2021)

Very nice work.  Looks great.

Chuck


----------



## Eccentric (Jun 29, 2021)

Time for some Lathe work (or should I say fun   )





The bearing holders are fairly straight forward jobs on the lathe.  I need to fabricate two main crankshaft bearing holders and two camshaft bearing holders.  Here I have the start on one of the Crankshaft main bearing holders and I am test fitting the crankshaft bearing.  I used sealed bearing, as opposed to open or shielded bearings.  I have used open ball bearings in the past, but used a rifled  bronze bushing out board the bearing for an oil seal.    At the speeds and temps that this engine will run, the sealed bearings should give good performance and provide a good oil seal.  The bearing holder has an oil seal O-ring to seal it to the crankcase as shown below.






The photo above shows the main features of the main bearing holder: a groove for an oil seal O-ring, a .010" relief to clear the ring of the inner race.  I first faced the blank, turned the outside diameter, drilled and reamed the through hole to clear the crankshaft.  I then used a boring bar to create the features on the inside of the bearing holder.  A round tool with the same profile as the O-ring was brought to bear to create the groove.






The holes for the mounting screws in the main bearing holders were drilled on the mill.  The inside diameter of the main bearings is .5" and so I used the 1/2 inch dummy crankshaft clamped in the chuck on the mill to align the bearing holder in the mill vise.  I then centered the mill DRO at this point and used the bolt circle feature to layout the six mounting holes on each bearing holder.  I am using 6-32 socket head cap screws to secure the bearing holders to the crankcase.  I first use a .113" drill, the size for the tap, not the clearance hole for a 6-32 screw.  I then remove the bearing holder from the mill vise, install it on the crankcase and match drill the holes for the 6-32 threads in the crankcase.  Finally, I return the bearing holder to the mill and drill the .113" holes out to .140" in the bearing holder; the clearance hole size for the 6-32 screws.






Now to turn my attention to the camshaft bearing holders.






The camshaft bearing holders were fabricated using the same work flow as the main bearing holders.  The primary difference was in the fabrication of the rear camshaft bearing holder.  It has an additional feature that routes oil from an oil gallery to the center of the camshaft where oil will travel to the cam lobes.






There is an additional step in the fabrication of the rear camshaft bearing holder, the CNC router was used to create the profile of the flange.






The rear camshaft bearing holder was then mounted in the mill vise and the oil hole was drilled.  This hole routes oil to the center of the cam shaft.  A hole is drilled down the length of the camshaft to deliver oil to the cam lobes.






The timing cover was machined by the CNC router.  Here it is mounted to a block of MDF with 5 minute epoxy.  I have had trouble with this technique in the past as the MDF will absorb coolant and swell.  Here the technique worked fine as the timing plate is just a 2 dimensional profile and a slight variance in the Z axis will not materially affect the resultant part.






The timing plate is responsible for aligning the bearings for the timing gears as shown in the photo above.  There will be a timing cover that holds the mating bearings and encloses the timing gears


I am working on a base for the engine that will also hold the other components required to run: radiator and fan, fuel tank, timing electronics, etc.  I also fabricated some engine mounts along with the display pillars and decorative washers.





The engine so far.


----------



## Jasonb (Jun 30, 2021)

Regarding your swelling MDF, you look to be using just standard grade which will be the most likely to swell, Oil will make it swell just like water will. You can also get Moisture resistant which does swell in extreme conditions but should hold up OK for this use and then there is exterior grade which will be even less likely to move. If you only have standard to hand then varnish the exposed faces, epoxy will seal the top so you will only have exposed MDF when the cutter machines any away

I've been using 4 flute ball nose cutters for 3D finishing as you can feed them twice as fast for the same given spindle speed & chip load which halves machining time. You could also probably up the spindle speed too as the effective cutter dia is mostly less than the actual dia of the cutter.


----------



## Eccentric (Jun 30, 2021)

JasonB,

Thanks for the input, I was unaware that there are different grades of MDF, but it makes perfect sense.  I just used a piece that was laying around and I am not even sure of its origin.  This is good news as I like the technique, I'll google it.  

You are correct in that I do use a two flute ball nose cutter and it is a great idea to move to a 4 flute for final finishing.  I would be able to make finer passes in less time.  I usually leave about .020" of material from the roughing pass, and at really small step overs the cutter hardly removes any material and could run faster.  Good idea.  Thanks.


----------



## Eccentric (Jun 30, 2021)

When I kicked off the machining of my Wallaby project a month or so ago, I decided to divide the project into four stages.  My first was machining the large components and this is now complete with the exception of some cleanup work.

 Here is the original CAD design:





And the final result:





Timing Gear side






Flywheel side






The engine looks bigger than it really is, it is only 3 1/8" long!

Next I am going to tackle the power train, not sure if this is proper nomenclature, but I have grouped the project into the 1. major components, 2. the power train, 3.  the valve train and 4. the timing train.  The power train consists of the crankshaft, middle crankshaft bearing, con rods, pistons, rings and cylinder sleeves. So I will be looking at the crankshaft next.  But before I start making chips I need to spend some time working on the 3D CAD model and making a set of prints that reflect the actual dimensions of the parts fabricated.  For example, I will measure the distance between the two main crankshaft bearings and match the crankshaft length to this.  Another example is the actual center to center distance of the crankshaft and camshaft. 



OK, back to the computer.........


----------



## Eccentric (Jul 5, 2021)

Time to start working on the crankshaft.  I cut a length of 1 1/4" by 5/8" bar to length and laid out the crankshaft from a 1:1 printout.














Then using a combination of drilling, a compressed air driven cut off wheel and the mill, removed most of the material for turning the first crank pin.

I marked off and drilled the holes on the ends of the work piece with a center drill for turning on centers. Then turned the first crank pin.










I only remove material with the drill and mill as I machine each feature to leave as much strength in the work piece as I can for each operation.

I had a bit of a brain fart and accidently used a dead center in the tail stock when I started turning the first crank pin. I caught my mistake before too long, but may have ruined the dead center. I installed a live center and continued machining.

Then I turned down the second crank pin as I did the first. This was all pretty standard lathe work turning between centers. Since the force of clamping the work piece between centers was straight through the crank pins being turned there was not distortion introduced by this clamping action.

I turned the crankpins to .500" finishing the last thou with emery paper. I am not completely happy with the finish, but they got better as I progressed with the fabrication of the crank. I ground a cutter from a piece of HSS as shown below. The intent, though not necessity executed well, was a broad faced tool at exactly 90 degrees to its length, with a radius on each side and a notch in the middle to reduce the amount of the tool cutting the work piece. I have generous reliefs on the face and sides.








When the crank pins were finished to proper dimension measured with a micrometer, I made some precision spacers to fit between the crank webs. They may not look precision, but I was very careful to make these a good fit, not too tight and not too loose, milling first then running them on emery paper on my surface plate (my band saw table). I made a crank once where these were an interference fit and they actually flexed the crank so that when they were removed the crank sprang back. I bonded them in place with JB weld. Not sure if this was the best choice, the JB weld got soft when the work piece got hot from machining, but it seemed to work out OK.












Here is the setup in the lathe preparing to turn the center main bearing journal.










Here is the center journal for now. I left it .010" over sized because I will finish it to final dimension in a setup where I turn all main journals at the same time to insure concentricity.










To determine the actual dimension between the two main crank bearing inner races, I fully assembled the crankcase, sump and main bearing holders with a dummy shaft with two bearings able to float as shown below.

Then reaching through the cylinder holes in the crankcase I spread the bearing and hot glued them in place. This gave me the actual dimension I needed to turn on the crankshaft shoulders that will rest against each of the main bearings. The design dimension was 2.3125" and the actual measurement was 2.331". I split the difference to maintain a centered crankshaft.



This worked exceedingly well as I ended up with a smooth crank with no end play.












The final operation on the lathe brought the three main journals into concentricity. They were all initially turned to between .005" and .010" over final dimension. I painted them with Dykem and used a thin strip of aluminum in the shape of a tool to rub on the journals to give me an indication of how far out I was. I was surprised that the journals were not perfectly concentric as I had been really careful. So I took very light .001" cuts off each journal walking the carriage back and forth in multiple spring passes. Fortunately I had enough material on them to allow me to produce nice concentric journals. I brought the two outside main journals down to about .0005" over, then removing and replacing the part in the lathe on centers test fitting them to the main bearings. I only used emery paper after I removed the part from the lathe to maintain my concentricity.








I am very pleased as to how smooth the crank turns in the engine now. There is no play in any axis and the crank turns under its own weight.

I have a few operations to finish the crankshaft, I need to drill oil holes that will deliver oil from the center main crank bearing to the big end rod bearings, I need to drill holes through the center of the crank pins (the ends will be sealed with plugs as there will be oil in there) to reduce rotating mass, and I need to add the counter balances.








Crank model with counter balances



I have started researching how to calculate the size and mass of the crankshaft counter weights. This is not a performance engine, won't rev very high, and it is impossible to balance an inline twin with both pistons moving in unison anyway. But I want to get as close as I reasonable can. I am not going to wait to weigh the actual pistons and con rods, but can estimate their weight and center of gravity with the CAD program.

Since the pistons do move in unison the engine can be modeled as a single cylinder engine with twice the mass of one of the con rods, pistons, rings and wrist pins. The formula I found is as follows: Weigh the top half of the connecting rod and add it to the weight of the piston, wrist pin and rings. Then take a percentage, say 55%, and add it to the weight of the bottom half of the rod. Place this weight in the CAD model at the center of both connecting rod journals on the crankshaft. Then adjust the weights of the counter weights to balance the entire rotating assembly.



I will let you know how it works out.


----------



## Eccentric (Jul 17, 2021)

This will be a quick update on the status of the crankshaft -- The only operations I have left are threading each end.  I have not cut threads on my new lathe and don't want to learn on my crank with its many hours invested.  I will practice on scrap and then finish off the crank later.



We left off on the design and placement of the counterweights







Since the pistons do move in unison the engine can be modeled as a single cylinder engine with twice the mass of one of the con rods, pistons, rings and wrist pins. This the two yellow rings in the assembly above.  The formula I found is as follows: Weigh the top half of the connecting rod and add it to the weight of the piston, wrist pin and rings. Then take a percentage, say 55%, and add it to the weight of the bottom half of the rod. Place this weight in the CAD model at the center of both connecting rod journals on the crankshaft. Then adjust the weights of the counter weights to balance the entire rotating assembly.



The counterweights needed to be slightly wider than the crank webs, they could not extend toward the ends of the crank because they would interfere with the sides of the crankcase, but there is room inside the crank webs toward the conrod.  I use two 4-40 cap head socket screws to secure each counter weight.

Before I set to work on the counterweights I did some cleanup and material removal on the crankshaft.  I fabricated two plates that I clamped to the sides of the crankshaft to insure I did not knock the crank journals off center with further machining.  I reduced the radius of the crank webs and trimmed the sides of the crank webs, all to reduce the mass at the conrod end of the crank.  In hindsight I should have done this machining before I finished the main and center journals, but I was impatient and wanted to see how well the crank ran installed in the crankcase.








Then on to the counterweights.

First I rough cut some 1/4" mild steel plate.










I used the mill to drill three holes to align with three threaded holes in an arbor mounted in the lathe.  I then turned the outside radius of the counter weights.










I used a cutoff wheel to slice the round disks in half to give me two counter weight blanks.  I then mounted them in the mill, zeroed the Z-axis against the parallel under the blank and machined the top side as shown below.












Below is the first counterweight test fit on the crank.








I then used the following process to accurately locate the mounting screws for the counter weight where I wanted.


I marked each counter weight and its associated crank web so they would not get mixed up later
All of the following work was performed on the mill, I drilled two holes in each counterweight so they would be centered on the crank web, so the holes ended up slightly off center on the counter weight.   The holes I drilled were the diameter of the drill bit used for the 4-40 tap.
Then I mounted the crank in the mill vise and match drilled one of the holes. through the counterweigh,  into the crank web.
 I then tapped this hole in the crank web.
I drilled out the one matching hole in the counterweight to a tight clearance fit and mounted the counter weight to the crankshaft with a 4-40 screw.
I then mounted the assembly in the mill vise again and match drilled the second hole in the crank web.
I tapped the second hole in the crank web
I mounted the counterweight in the mill vise and drilled out the second hole to 4-40 clearance size.
I used a 3/16" end mill to create my counter sinks for the heads of the socket head cap screws.
I then repeated this process for the remaining three counter weights.


Below is a close up of the mounted counterweights








The final operation I performed was drilling the two oil holes that will deliver lubrication to the large conrod end bearings from the crank center bearing.








This is the current state of the crankshaft.  So far I have not screwed it up and it still turns true in the crankcase.


----------



## Eccentric (Jul 21, 2021)

I am going to present my design and fabrication process for the Wallaby conrod in three posts: one focused on the Computer Aided Design (CAD), one focused on the Computer Aided Machining (CAM), and one on the actual machining. 






Above is the drawing for the Conrod with most of the critical dimensions, there are some minor dimensions such as fillets and radii that are not called out.  These could be shown on another sheet and are defined by the choice of the end mill used.








Here are a couple views of the 3D model for the connecting rod.







The next series of pictures detail the steps I went through to create the 3D model.  The dimensions for each were pulled from an initial sketch.  The final drawing is a result of the final CAD model.




I first used a "revolve" feature to create the two barrels for the piston pin and the crankshaft main journal. 






I added the web between the barrel sections, this will eventually be shaped as an "I" beam for max strength and min weight.  The lightning cutout will be added later.  This is a simple "extrusion" feature.





The "extrusion" feature on the end cap for the end cap screws to bear down on.






Above is another "extrusion" feature for the threaded end cap screws.  Fillets have been added around the big end barrel.  I used a "fillet" feature, but due to the complexity of the multiple surfaces that intersect, a blended surface would look better.  I may go back and improve this area.

Below a "cut" cut feature gives us the side profile we need.








Below are three "cut" features: the counter sink for the head of the cap screw, the clearance hole for the cap screw and the threaded portion in the conrod.








Then finally the lighting cutout "cut" feature in the web.




Next I am thinking that I will show the steps to machine and insert the associated CAM process where it is needed.

Let me know if this is interesting, too much detail or not enough.  thanks.


----------



## gadabout (Jul 21, 2021)

Eccentric said:


> I am going to present my design and fabrication process for the Wallaby conrod in three posts: one focused on the Computer Aided Design (CAD), one focused on the Computer Aided Machining (CAM), and one on the actual machining.
> 
> View attachment 127757
> 
> ...


Hi, 
am liking the detail very much , please keep it up!!
regards
Mark


----------



## kuhncw (Jul 21, 2021)

Nice work.  I'm enjoying the details.

Chuck


----------



## CFLBob (Jul 21, 2021)

Eccentric said:


> Let me know if this is interesting, too much detail or not enough. thanks.



You know we could keep you busy writing and not building the Wallaby, right?  

I have one question: what CAD program is this? Solidworks (based on the file extension)?


----------



## gadabout (Jul 21, 2021)

Oh and the OCD in me thinks the typo in the heading needs correcting .
regards
Mark


----------



## Eccentric (Jul 21, 2021)

Bob,

I use SolidWorks for CAD and Fusion360 for CAM.

For Gadabout it,  

That is funny, I probably never would have noticed that "Westbury" is misspelled in the title of this thread.  I will look into how to edit it, now it is bugging me.

Greg


----------



## gadabout (Jul 21, 2021)




----------



## Jasonb (Jul 22, 2021)

Yes keep it coming. Having done a few similar conrods it's interesting to see how others go about it. Judging by the colour of the 3D image you are going to be using bronze which can make a difference to the machining methods over an aluminium one which is mostly what I have made mine from.


----------



## GreenTwin (Jul 22, 2021)

I use SW 2011.
It is quite nice when it works correctly, which is most of the time.
I use it for work and modeling, and so I can justify the expense.
.


----------



## xpylonracer (Jul 22, 2021)

Jason

6061T6 is stated on the drawing.


----------



## Weldsol (Jul 22, 2021)

Hi Eccentric not being a CAM or CNC user I'm interested how you will machine the conrod as I can't see how you will be able to do the big end bore as this will have to be done after splitting the cap otherwise you will end up with an oval bore.
I know when I did my conrod set I had start with split blocks drilled counter bored and tapped do both big & small end bores then  make a jig so that I could do the profiling (material Dural)

Paul


----------



## Jasonb (Jul 22, 2021)

xpylonracer said:


> Jason
> 
> 6061T6 is stated on the drawing.



I missed that and was going by the colour of the part as the original used Gunmetal (bronze) castings. I thought the same was going to be used which makes it easy to soft solder the bearing cap on and machine as one.

If it is going to be aluminium then I tend to screw the two parts together, bore and then hold by the two holes to do the CNC external shaping, sacrificial brass screws can help as it does not matter if they are partly machined away. The alternative is to split the rod in two in the CAD package and machine each part separately then screw together and finally bore, I've done it that way once where shape of rod lent itself to that approach.

Also raises the question that 6061 is not a good bearing material so will really need bearing shells but drawing shows 1/2" big end hole and crankshaft is 1/2" too. If not using bearing shells I tend to use 2014  (2011 in US) as that can run straight on the shaft and is also less likely to stretch.


----------



## Weldsol (Jul 22, 2021)

Just been reading ETW's notes from ME 1962  on the Wallaby and he specified con rods in Bronze or Dural
Paul


----------



## Jasonb (Jul 22, 2021)

2014 which is the old HE15 spec is about as close as you can get to Dural. It's heavier than 6061 so could muck up the counter balance weight calcs but not as heavy as GM


----------



## Eccentric (Jul 22, 2021)

You all are correct, the conrods were intended to be made from cast bronze.  I am building this engine without castings and I can't afford a chunk that big.  Using aluminum with leaded bronze bushes would be ideal, but I am not ready for that level of complexity.

Solid bronze is heavy and not ideal for conrods. I have wondered about the suitability of aluminum without bronze bushes for the conrods, but Westbury seems OK with it. He states"..lighter rods machined from Duralumin (an obsolete term, originally a trade name for one of the earliest types of age hardened aluminum) may be preferable to some.   In the Sealion build article he states that "duralumin or similar light alloy is a more suitable material for the job".   Of course, he is a 50+ year old source. 

It will be interestig to dissasemble the engine after a couple of hours running to see how the aluminum holds up. That of course depends upon: one that the engine actually runs and two that it ever makes it to two hours


----------



## Jasonb (Jul 22, 2021)

The 6061 won't hold up too well, there is a risk of it stretching around the holes and as I said earlier it is not that good a bearing material. 

Although Dural is no longer made 2024 or 2014 both in T6 temper are a much better option and often specified on model engine drawings.They won't stretch as their about 50% stronger and as they have about 5%copper in will be OK as a bearing surface. Really any of the 2000 series alloys will be OK as they are similar to Dural, the 6000 series are not really similar. I've used 2014 as that's readily available in the UK for Glow, Diesel, 2-stroke petrol and 4-stroke petrol model engines all without issue


----------



## Eccentric (Jul 22, 2021)

I can readily get 2024 T3/T4 (not T6) at my local metal distributor, but I thought 2024 was really soft and malleable.  I use some thin sheets of it on the lathe to protect a work piece from the chuck jaws, but I don't know what temper it is.  I would have to order T6 online--totally doable.


----------



## Eccentric (Jul 22, 2021)

Conrod order of operations


square up the blank 1" X 3.5" X .438"
machine cap bottom shape on CNC
machine 3/16" counter bore on bottom of cap
Center drill two holes
drill 2 each .089 holes on bottom .5" deep
follow up with and drill both .113", but only .125" deep
tap the 4-40 holes using a spring tap guide in the mill
machine  off the end cap
drill out holes in cap to .113 and install end cap
drill and ream the .501" main bearing hole
drill and ream the .251" piston pin hole
Mount to CNC machining fixture
Go to the CNC for contour machining both sides





Squared up blanks.  The thickness is the only critical dimension.



Now I need to machine the cap bottom.  Solidworks allows for "alternate configurations" which is a variant of a part with differences.  I use it to crate simplified models to ease the generation of the CNC tool paths.  Below I create a shadow solid that isolates the bottom of the rod so I can machine the curved bottom feature.  I overlay the desired shape over the part and create an alternative configuration for the rod.




Sketch creating model for machining the conrod end

Below is the finished model, notice the small cut between the main body of the conrod and the end section.  this allows me to isolate just this end part to target the machining and stay clear of the vise.

The CAD tool tells me the smallest radius I need to machine is .133", so I can use a 1/4" end mill to create this feature








Time to export the model for the CAM work.  I use fusion360 and highly recommend it.  It is free for us home hobbyists and does everything I need it to.  It has a nice user interface, but getting all of the settings needed to create a tool path can be frustrating.  It has taken me some trial and error to get the CAM to do what I want it to.  Fortunately it has a "template" feature that allows you to save a setup for use in later parts.  So once you get it dialed in, you are good to go.

I export an IGES file and import it into Fusion 360.  I select "Manufacture".






This green highlighted geometry selection tells the cutter to only cut the area of interest and not interfere with the clamping on the rear portion of the work piece.








Contour Parameters


1/4" flat end mill
8000 RPM at 13 IPM
Step Down of .1"
Climb milling for smooth finished surface
2 Passes, the first will leave .020" of radial material, the second will be a finishing pass. 
The tool path is simulated to verify it is doing what we want, then exported to a Gcode file.  This I put on a USB drive and carry out to the workshop and load onto my CNC router.  I use LinuxCNC and am quite happy with it.  So much of this software stuff it is finding something that works, learn its idiosyncrasies and making it work for you.





Machining






Finished end cap feature. One down, One to go.






Over to the mill, establish the center of the holes with an edge finder.








Counter bore 3/16" and center drill






Drill the two hole sizes.  I like to drill the clearance hole in the same setup as the tapped hole to insure they are truly concentric.



Next I will mount the conrod in the mill horizontally and mill off the end cap.


----------



## Weldsol (Jul 23, 2021)

I like to tap the bar prior to slitting as it is easier to hold plus doing the tapping at the same setting as the drilling (using a centre in the drill chuck to support the tap holder ) ensures the threads are true to the cap

Paul


----------



## Eccentric (Jul 25, 2021)

A quick update on the completion of the manual machining for the connecting rods.






Here I am machining off the conrod end cap.  As Paul suggests, it is better to tap the holes before cutting off the end cap.  A slitting saw could also be used.  I am using an 1/8" end mill and I am offsetting each pass .005" so that each face, both the conrod and the end cap, are climb milled for a nicer finish.





The final manual machining is pretty straight forward: using the edge finder to locate the two holes, center drill, drill and ream.






Here are the two conrod blanks ready for the CNC router.  Behind them is the beginning of a fixture to locate the conrods during the CNC routing operations.  The conrods will need to be flipped so we can machine both sides and we need to maintain proper orientation with as much precision as we can.


Next installment I will detail some more CNC tool path generation in Fusion360.


----------



## Eccentric (Jul 27, 2021)

The first step to CNC machining the conrods is to make the fixture to hold them in a manner that allows them to be machined on both sides.  I like to machine the fixture and the conrods all in one setup so the conrods and the fixture have the axis touched off at the same time.  It is OK to make the fixture and use it later, but there will probably be a couple of thou zeroing error when the fixture is setup in the vise a second time.  So I machine the fixture and tap the 6-32 threaded holes in the vise, install the alignment pins, then machine the conrods without re-zeroing the work piece.




Here is the conrod blank mounted on the fixture.  Note that the hold down screws only provided a downward locking force and do not locate the blank, this is done by precision machinied pins.  There are matching machined pockets machined into the fixture to locate the pins.



The conrods will have the following machining operations:


Removing the majority of the material then finishing the flat surfaces - 1/4" end mill
Machining the flat sides - only needs to be done once - 1/4" end mill.
Machining the curved surfaces - 3/16 ball end mill
Machining the cut out in the middle of the conrod web- 3/32" flat end mill.
Flip and repeat
I made three different 3D models to ease the generation of the tool paths.  Below is the first one, note that the side cutouts and the middle web cutout are missing from the model.



Below is the simulation of the first machining operation.  the blue represents the material left by the roughing pass and the green is the finishing pass for the flat surfaces. Note that the very top flat surfaces are not machined as this is where the tooling hold downs are.  The machining parameters are: 1/4" flat end mill, 8000 RPM, 15 IPM, 050" step down, .020" material left on roughing pass.












After the 1/4" flat end roughing, but the sides have not been finish machined.

Next, with the 1/4" flat end mill still mounted, the sides are machined:








Below is a simulation of the finishing pass with the ball end mill.  The parameters are as follows: 8000 RPN, 10 inches per minute, .005" step down and only the curved surfaces were selected for machining.  While the other machining operations took about 10 minutes, this one takes 25.






The fine blue lines show the tool's path, the yellow lines are moves where the tool is not in contact with the work piece.






After the side milling, contour milling and the web cutout milling. Read to flip it over and do the other side.







The above simulation shows the expected result after machining the curved surfaces using the 3/16" ball end mill.  I have circled two areas that were not properly machined during the horizontal finishing pass, I did not notice these artifacts until after machining the conrods.   I will have to finish these areas by hand.

Finally the conrod web cutout is machined with a 3/32" end mill, this will give nice radii in the corners.










While I was machining the second conrod my compressor gave up the ghost.  My spindle is water cooled and requires compressed air to seal the bearings. The compressor's electric motor made a horrendous screech and then blew a fuse.  I ordered a replacement 5 hp motor from Amazon and it will be here tomorrow.  So I will have to re-establish the CNC axis zero points and restart the milling operation.  I will touch off the precision pins in the fixture.



Below is the first conrod mounted on the crankshaft, I am very pleased with the fit.






Notice the reliefs I had to add to the sump to clear the conrod cap attachment screws.  I did not include these screws in the CAD model, so did not notice the interference.  The CAD model should include ALL the parts including hardware, live and learn.


----------



## Eccentric (Jul 29, 2021)

I received a new electric motor for my compressor and was able to continue machining this morning.  I finished up the second conrod.





I will bead blast these before I install them.




I also worked on the main crankshaft center bearing.  Fairly straight forward lathe work.  I started with a couple of bronze bushes and machined a bit more than 1/2 off of each, then soldered them together.






I chucked them up in the lathe and drilled and reamed the inside diameter to .501", then turned down the outside diameter to .625".  I made a little sideways notch tool and machined a small groove in the middle of the bronze bearing for oil. Then cut it off.

For the bearing caps, I grabbed a couple of pieces of scrap aluminum, fly cut a smooth surface on each. Then clamped them together in the vise.  One was a tiny smaller so I used a few pieces of paper between it and the vise jaws to lock them both down.  then I machined a couple of countersinks, drilled and tapped, then screwed them together.






 then back to the lathe:






I turned the outside to 1.250" and drilled and bored the inside diameter to .625 using the bronze bushing (still soldered together) as a check.  Faced the outside, cleaned up the edges and parted it off.

I then heated up the bronze bushing and separated the two halves.



Below is the bearing cap and the bronze bush installed in the upper crankcase.






I oiled up the bushing and tightened everything down.  there is an area of about 10 degrees where the crank is a bit tight.  I'll inspect it and see if anything stands out, otherwise I think this will wear in.  I still need to drill the oil hole in the cap and bronze bushing and I will also drill a small hole and inset a brass taper pin to insure the bronze bushing does not spin.


----------



## CFLBob (Jul 29, 2021)

Beautiful, as always.


----------



## Eccentric (Aug 1, 2021)

*Cylinder Sleeves*


I have made both of my cylinder sleeves, and of course the second one came out better than the first.  I was targeting an ID of 1.000" and I had to take the first one out to 1.005" to get the ID consistent all the way through and to remove a scratch by honing.  The technique I used to get the second near perfect included the following strategies:


Used a four jaw chuck to give max clamping support on the blank cast iron work piece.
Cut the ID before the OD to provide more material to stabilize the blank while cutting the ID. 
I used an oiled paint stick and applied constant, but slight, pressure on the outside of the sleeve, sort of a poor man's following rest to counter act the pressure of the boring tool.  without this I was getting about .002" spring in the part from the start of the boring pass to the finish.
When close to my final dimension, I used a bunch of spring passes where I did not advance the cross slide, just ran again and again
I ran the lathe really slow so there was no chatter, I had to go down to 280 RPM, but got really clean cuts.
I used the finest power feed setting.  A single pass took about 6 minutes
All of this required extreme patience, but I got two sleeves that I am happy with. But more important I think I have a solid technique for future builds.






Wow did I learn a few things preparing my cylinder sleeve blanks.  I attempted to cut the cast iron rod into two using a standard cut off wheel like I use to cut mild steel.  That did not work.  I cut and cut and cut and cut and all I ended up with was a chunk of really hot cast iron.  Finally I stopped and did some research.  I then switched to a diamond masonry blade and that made all the difference.  It cut right through the cast iron.  On the first blank I drilled the internal ID out to .5" using the largest drill bit I own, then bored it out to close to the final 1".  That took forever.  So I bought a set of drills sized 9/16 to 1" and drilled the blank close to final dimension before I started boring.  Much quicker.





Set up on the table saw for cutting cast iron blanks.   Out of the frame is another large C clamp (G clamp) holding the wood to the miter slide.








Test fitting the first blank in the cylinder block.  I turned the OD first on this one.








My drill bit set from Amazon, saved a bunch of time boring.












Second cylinder sleeve - nice finish on the ID, right on the numbers, no chatter at 280 RPM.

Honing went pretty quick on the second sleeve and I took off just under .001" of material.  the first sleeve took longer as I had a step of .002" at the top end that I could feel with my finger.  After taking this out and removing a scratch toward the bottom I ended up .005" over my target internal diameter.  This will complicate the manufacture of the rings as I will have to make two batches of differing sizes.  The pistons will be different too, but in the big scheme of things pistons are nothing compared to making rings.








Sleeves test fit in the block.  One cylinder I gave a cross hatch hone, the other I did not.  I do not know if this matters.  The sleeves are sitting slightly proud of the top of the block, these will be fly cut flat after the sleeves are secured in the block with loctite.


----------



## Thommo (Aug 2, 2021)

Hey Eccentric, just wondering why you didn’t x hatch both bores? Engines looking great!


----------



## Eccentric (Aug 2, 2021)

I have never cross hatch honed a model engine cylinder before and I don't recall seeing it done.  I did my first cyliner as I usually do, no cross hatch.  But all of the full sized engines I've ever rebuilt, I always put a cross hatch pattern in the hone, so I did it on the second cylinder.  I think that the finish on the model engines should be so fine that you don't really see the hone pattern, but I don't think you want the finish so fine it is "polished".


----------



## Thommo (Aug 2, 2021)

In full sized engines, the idea of cross hatching is to “hold lubricant”on the bore as well as assisting in “bedding in” the rings! However, as you say model engines don’t usually have it at all. It makes me wonder why. Thank you for your response.


----------



## Eccentric (Aug 3, 2021)

*Piston rings*

First off I want to say that I have seen that the fabrication of rings can be a charged subject on this forum and I am no expert so take what I do with a large grain of salt.  I was amazed that Brian's recent discussion of making rings garnered over 30 thousand views over a period of a few months.  Wow!

I try to machine to print, but there are so many hours in the fabrication of the sleeves and rings that I want to be able to use a part that might not be perfect.  So I make my cylinder sleeves first, then make my rings to match them, then I make my pistons to match the rings.

A recent revelation was Terry's light inspection technique.  I machined an aluminum plug (don't have any Delrin), painted it black and use a super bright flash light to backlight the rings in the sleeve. 

I use George Trimble's formulas for the dimensions of my rings and the stress relief fixture. Given a 1" bore, the thickness of the ring should be between .040" and .045". I go a little bigger, say .050" This is rather critical! Too thin and there is not enough wall pressure, too thick and you have too much installation stress (broken ring). The relaxed gap should be .15" ( I use 4mm - .154"), compressed gap should be .004". The height of the ring is not too important.  Smaller is less friction, say .03125"

I use my CAD program to do my math for me. Below is my calculation for the fixture:






First I take the internal diameter of the split and gapped ring in the cylinder sleeve.  That is represented by the circle on the right, the internal diameter of the ring in my case is .900"  Using a half circle allows me to measure the arc length.  I determine that the arc length of the internal of the split ring is 2.8234".  This is twice the displayed ring half arc length of 1.4137 minus the gap of .004.  These dimensions are placed on the left diagram which represents the heat treat fixture.  This gives me a diameter for the fixture of .9455", a spacing pin diameter of .154" (I use a 4mm threaded rod)  and the position of the gap spacing pin from the center of the fixture of .5038" (I round to .50")

Summary of my piston ring fabrication process:

I put the cast iron slug in a 4 jaw chuck for the max gripping power and rigidity.
I turn the ring blank down, leaving 300% material, so instead of .050" thick, I turn down to .150.  So, for a 1" internal cylinder bore, the ID of the blank would be about .9" and the OD would be about 1.05"
Pull the blank out of the lathe and Stress Relieve in the heat treat oven - 1000 to 1050 degrees F for an hour and a half. 
Furnace cool to less than 200 degrees F before air cooling the rest of the way down.  Usually I just leave it in the oven over night.
Put back in the 4 jaw chuck centering as well as possible. Turn the ID on the ring blank to final dimension, then turn the OD to final dimension. Finish the OD with emery paper.
Part the rings off. 
Wet sand (with light oil) on a piece of glass with 800 grit paper to clean up edges and get to proper height.
Cleave the ring gap.  I lightly score the top and bottom of the ring with a fine file, then use a razor blade to cleave the ring. I hold the razor blade so its cutting edge is in the filed groove, then tap the back of the razor blade to cleave the ring.
Use a fine diamond file to clean up the gap and get it to .004" in the cylinder sleeve using feeler gauges.
Use an Arkansas sharpener's ceramic rod to clean up inside edges.
Clean the rings and the heat treat fixture with acetone.
Clamp rings into the heat treat fixture. Clamp means finger tight, everything will expand with the heat.
Set the heat treat oven to 1050 degrees F and place the loaded ring fixture into the oven.
When the oven reaches a temp of about 300 to 400 degrees, pull the fixture out of the oven and rub borax all over the exterior of the rings.  This does a good job of preventing scale, it is easy to see where you miss a spot after treating.
Stress Relieve the rings in the heat treat oven - 1000 to 1050 degrees F for an hour and a half.  (my reference is the study performed by the Naval Research Laboratory on stress relieving cast iron dated 1948)
Furnace cool to less than 200 degrees F before opening the furnace.
Remove the fixture and drop into a tin can of boiling water to remove the borax.
Lightly scotch brite the rings exterior, then remove them from the fixture. Clean the rings as necessary.
Perform Terry' light test to determine the quality of the seal of the rings against their cylinder sleeve.
Measure each ring, note in the log, coat each with light oil, and place into labeled zip lock bags.





Heat Treat oven in use for cast iron stress relief






Heat Treat fixture just out of the Oven.  I use a single sacrificial ring to insure the stack is flat against the fixture.






Finished ring installed in its cylinder sleeve with computer screen back light. Ring Gap can be seen at the top of the ring and is .004".








Light Testing Essentials








Good light test, only the ring gap lets the light through.  In a dark closet here,  I needed a little ambient light for the photo.  You need to twist the cylinder and look straight down the walls to see if there are any light leaks.

What was my biggest lesson learned?  Make all of your cylinder sleeves with exactly the same internal diameter!  I made one 1.000" and another 1.006".   I just finished making a set of rings for one cylinder, now I need to repeat the process for the other.  It would have been better to make hone both cylinders1.006" and all the rings the same.


----------



## Eccentric (Aug 5, 2021)

I am thinking I want to tackle the riskiest  parts next.  The rings are definitely one-this is behind me, the valves and their ability to seal against their valve cages are another.  the cam is also one.  I am not too worried about the timing gears.  OK, It is decided.  I am going to tackle  a couple of valves and their valve cages and build a test fixture to verify their ability to seal.  I really like what Terry M. did in this regard.  I have 303 stainless for the valves and some bronze rod for the valve cages.  I'll use the 3D printer to make the test fixture out of ABS and some O-rings.


----------



## Charles Lamont (Aug 6, 2021)

That image shows far too great a width of the valve seating.

Usual practice is to machine the seating square edged, and if necessary (it usually is) cut a very fine chamfer with a home-made seating cutter used by hand, then gently lap the valve in with a fine, soft paste. Brass polish may be enough.


----------



## Jasonb (Aug 6, 2021)

I'm not a fan of seating cutters I prefer to turn a chamfer with the topslide set over to 45deg at the same setting that the valve guide is reamed at so all stays concentric. This can require some complex setups when there is no separate insert and the seat is machined directly into the head, one below was about the most out of balance I have done.

Width of seat varies from one design to another but I've yet to see one shown with a square edge, most seem to range from 1/16" to 1/8" wide.


----------



## Eccentric (Aug 6, 2021)

Charles Lamont said:


> That image shows far too great a width of the valve seating.
> 
> Usual practice is to machine the seating square edged, and if necessary (it usually is) cut a very fine chamfer with a home-made seating cutter used by hand, then gently lap the valve in with a fine, soft paste. Brass polish may be enough.


Thanks for the information on the size of the valve seat.  I really appreciate it.  A seemingly insignificant detail such as this can result in a valve does does not seat and an engine that does not run and endless furstration.  thanks again.


Jasonb said:


> I'm not a fan of seating cutters I prefer to turn a chamfer with the topslide set over to 45deg at the same setting that the valve guide is reamed at so all stays concentric. This can require some complex setups when there is no separate insert and the seat is machined directly into the head, one below was about the most out of balance I have done.
> 
> Width of seat varies from one design to another but I've yet to see one shown with a square edge, most seem to range from 1/16" to 1/8" wide.



That is an incredible setup.  Bravo.


----------



## Basil (Aug 7, 2021)

Interesting! I've been wondering how to approach the valve seat angle cutting and how wide to make it. I build many small Honda engines and they make this tool which works well for final seat finishing. I plan to fashion something similar in miniature. For reference OS engines use quite a narrow seat width (pictured in head) while Saito use a wide seat. The little OS 20 valves are very nice!


----------



## CFLBob (Aug 7, 2021)

Basil said:


> Interesting! I've been wondering how to approach the valve seat angle cutting and how wide to make it. I build many small Honda engines and they make this tool which works well for final seat finishing. I plan to fashion something similar in miniature. For reference OS engines use quite a narrow seat width (pictured in head) while Saito use a wide seat. The little OS 20 valves are very nice!



This is a great turn in Eccentric's build thread for us newbies, and I don't want to de-rail it, but what I like about this is the Honda tool.  

Most of us don't mind special setups like the cylinder head in the four jaw chuck, but for a factory, having to do special setups all the time can be a big expense.  So custom tools are analyzed to see if they can save money.  If the tools can save money over different setups, they'll do it.


----------



## Steamchick (Aug 8, 2021)

My only real experience of valve and seat size and design is from the 1960s, when I was "part-time apprentice" at a friend's engine overhaul workshop. I was tasked with re-grinding valves on the Delapina Valve grinder... and fitting new seat inserts and grinding seats in old worn cylinder heads... mostly where the original seats had been directly cut in the head castings. Seats at near enough 1/8" were standard, form Mini 850cc engines to truck engines that had valves 2" diameter. The seal-line was about 1/16" wide after lapping. (Same width as a pencil lead was ideal). But MODEL engines have such tiny valves, I imagine that starting with a square edge of the valve port and lapping to a full line on the valve AND SEAT will be OK.... Spring pressure, hammer when closing etc. are all affected by "scale" factors, (squares and cubes particularly) and the usage is not thousands of hours but hundreds of minutes. If the valve is 10mm across, then 1mm of seat seems sensible. As a maximum...
But I am really only guessing...
K2


----------



## Weldsol (Aug 8, 2021)

Basil said:


> Interesting! I've been wondering how to approach the valve seat angle cutting and how wide to make it. I build many small Honda engines and they make this tool which works well for final seat finishing. I plan to fashion something similar in miniature. For reference OS engines use quite a narrow seat width (pictured in head) while Saito use a wide seat. The little OS 20 valves are very nice!


I had to make a similar tool for the sealion 
Paul


----------



## Eccentric (Aug 9, 2021)

Paul,
You are a better man than me putting eight valve seats in a head without valve cages.  I can imagine the sweat on your brow as you cut each one hoping not to ruin your head with its innumerable hours already invested.

I remember reading one of Westbury's articles where he suggests installing the valve and then giving it a wack to form the valve seat.


----------



## Weldsol (Aug 9, 2021)

Eccentric said:


> Paul,
> You are a better man than me putting eight valve seats in a head without valve cages.  I can imagine the sweat on your brow as you cut each one hoping not to ruin your head with its innumerable hours already invested.
> 
> I remember reading one of Westbury's articles where he suggests installing the valve and then giving it a wack to form the valve seat.


I used a 3 step D cutter as per ETW's recommendation so you cut the hole for the valve guide / then for the porting / and the chamber all in one operation so that everything is in line then you link the round chamber parts together to for the full chamber size.
Yes it was a heart stopping moment on each one considering the amount of machining which would have been wasted  by just one slip up.
The valve seats were cut after installing the guides and I used a DTI on the end of the pilot pin to measure the depth ( all cut by hand power )

Paul


----------



## Nerd1000 (Aug 10, 2021)

Steamchick said:


> My only real experience of valve and seat size and design is from the 1960s, when I was "part-time apprentice" at a friend's engine overhaul workshop. I was tasked with re-grinding valves on the Delapina Valve grinder... and fitting new seat inserts and grinding seats in old worn cylinder heads... mostly where the original seats had been directly cut in the head castings. Seats at near enough 1/8" were standard, form Mini 850cc engines to truck engines that had valves 2" diameter. The seal-line was about 1/16" wide after lapping. (Same width as a pencil lead was ideal). But MODEL engines have such tiny valves, I imagine that starting with a square edge of the valve port and lapping to a full line on the valve AND SEAT will be OK.... Spring pressure, hammer when closing etc. are all affected by "scale" factors, (squares and cubes particularly) and the usage is not thousands of hours but hundreds of minutes. If the valve is 10mm across, then 1mm of seat seems sensible. As a maximum...
> But I am really only guessing...
> K2


On my Webster I machined the valve seats square. Lapping with the valve established sufficient seat width. Would probably cut a small seat on larger valves.


----------



## Eccentric (Sep 11, 2021)

I have been developing the capability to cut the gears for the Wallaby.  I will be using the tools and techniques I picked up from Chris over at ClickSpring.  If you are not familiar with his work, look him up on YouTube, he is very talented and makes beautiful videos. I will not repeat his instructions here as I could not do them justice.  To make a gear you need to be able to cut the spaces between the teeth with a properly shaped cutter, and to make the cutter you need special lathe cutters, mandrels, cutter blanks, and sharpening tools.  This is where I started.  Below is a picture of the print for one of the spur gears and an aluminum test gear, the final spur gears will be made of brass and the pinions of steel.







This is the print for one of the two pinions






Sheet two has the information necessary to create the cutter to cut the space between the gear teeth.






Below I am practicing making gear tooth cutter blanks from 01 tool steel.








Below is the beginnings of one of the button cutters that will cut the profile into the gear tooth cutter.  these are precision diameter made from 01 tool steel and hardened. In the back ground is a tool that allows the proper relief angle to be cut into the button cutters and is also used to precicley sharpen them.






As seen below two of these button cutters are mounted in a holder and cut the proper profile into the cutter on the lathe.





Then the mill is used to create the face of the cutter.






Below is the gear tooth cutter ready for heat treatment.












This is a rotary table that I picked up from Amazon and uses the same chucks as my lathe.  I use some Arduino code and a PC to advance the gear blank the correct amount so the mill can cut each tooth space.






I cut the gear blank to diameter on the lathe, then move the entire chuck and work piece to the rotary table on the mill.  then I cut each leaf (the space between the gear teeth).






Finally I move the chuck back to the lathe and perform the other operations to finish off the gear.


----------



## Steamchick (Sep 12, 2021)

Eccentric, I am impressed with your work. Toolmaking and gear-making puts you in a class or 12 ahead of me! - Well-done Sir!
K2


----------



## Richard Hed (Sep 12, 2021)

Eccentric said:


> I have been developing the capability to cut the gears for the Wallaby.  I will be using the tools and techniques I picked up from Chris over at ClickSpring.  If you are not familiar with his work, look him up on YouTube, he is very talented and makes beautiful videos. I will not repeat his instructions here as I could not do them justice.  To make a gear you need to be able to cut the spaces between the teeth with a properly shaped cutter, and to make the cutter you need special lathe cutters, mandrels, cutter blanks, and sharpening tools.  This is where I started.  Below is a picture of the print for one of the spur gears and an aluminum test gear, the final spur gears will be made of brass and the pinions of steel.
> View attachment 129021
> 
> 
> ...


This should work for steel as well as alu, right?


----------



## petertha (Sep 12, 2021)

Thanks for showing these details!

Post 61 shows the Cad diagram of the gear & then on separate sheet looks like you are developing the resultant button diameter & spacing. Did you import the gear solid model from a vendor website or develop it yourself? Just wondering because there was a good YouTube video showing gear tooth generation for Solidworks (which looks like you are using?) entirely using equation driven dimensions for the tooth profile. I don't have it handy but could locate it. But taking it to the next step for cutting tool buttons is very crafty. I was told to be wary of manufacturer downloads because they can vary in their details depending on the source. Some are quite accurate with important details like relief & fillets etc. Others are just meant for spotting into assemblies with no real intent to make the gear itself.

Can you show some more details of the fixture that cuts the relief angle? How did you determine how much to off center the cutter? Then you mentioned re-sharpening - how is this accomplished


----------



## Eccentric (Sep 12, 2021)

Steamchick - thanks for the kind words.  I don't think there is anything I am doing here that is not standard machining practice and well within your abilities.

Richard, you are correct, this will work for steel.  My two pinions will be made from steel and the two spur gear will be made from brass.  I am working in aluminum now to refine my technique.  But the smaller gears (pinions) will be cold rolled mild steel, then I will case harden them with the case hardening compound available from Brownell's.  It is difficult cutting steel gears so as not to harm the cutter, it is very important to keep the chips cleared and to progress slowly, both the cutting speed and the spindle speed.  I will make several passes to cut each leaf.  Brass is different, one pass works well.

Peter - you are correct, I used the built-in SolidWorks gear tool to create the drawing, BUT I am NOT using this profile to make my cutters.  Involute gears have a complex tooth shape that can be closely approximated with a constant radius arc.  I am using Chris'  spreadsheet (Clock Making and Home Machining) to calculate the dimensions shown on the second sheet of my gear drawing.  The button cutters are turned on the lathe from 01 tool steel as shown in my last post, and bonded into a block of steel as shown in the following fotos.  The button cutters are mounted with a 15 degree relief angle, and they themselves are cut at 15 degrees.

The following picture shows the formed cutter fit into the forming tool.








Here is a closeup of the cutter tool for the gear cutter, you can see the 15 degree relief marked in red.






Below is the mandrel used to cut the gear cutter.  the gear cutter is mounted off center in order to create the 15 degree relief angle when actually cutting the gear.  The pin holds the cutter in the proper position as the cutter profile is turned on the lathe, then the cutter is rotated to the next position and the lathe operation is repeated.  This mandrel is also used in the mill to cut the notches which reveal the cutter faces.






Below is the setup for sharpening the gear cutter.  It presents the face of the cutter perfectly to the grinding stone. This same set up is used to sharpen the button cutters. I have highlighted in red the holes that the button cutters are mounted in while they are sharpened.






You asked the question: How did you determine how much to off center the cutter? Below is a drawing of the gear cutter blank, I have circled in red the desired 15 degree relief angle that is presented to the gear as it is cut.  Then I have also circled in red a small point that represents the rotational axis the cutter blank needs to be turned on in the lathe to create this relief angle. 






Below is a test fit of the practice aluminum gears on the engine.  How do you like my precision carbide 1/4" gear shafts?  The top right gear is connected to the cam shaft and the bottom gear drives the oil pump.






Below is a mega close up of the two small gears meshed.  The leaf cut depth is .07" for scale.


----------



## Richard Hed (Sep 12, 2021)

Eccentric said:


> Steamchick - thanks for the kind words.  I don't think there is anything I am doing here that is not standard machining practice and well within your abilities.
> 
> Richard, you are correct, this will work for steel.  My two pinions will be made from steel and the two spur gear will be made from brass.  I am working in aluminum now to refine my technique.  But the smaller gears (pinions) will be cold rolled mild steel, then I will case harden them with the case hardening compound available from Brownell's.  It is difficult cutting steel gears so as not to harm the cutter, it is very important to keep the chips cleared and to progress slowly, both the cutting speed and the spindle speed.  I will make several passes to cut each leaf.  Brass is different, one pass works well.
> 
> ...


It seems to that your clearance of 15deg on the cutter is not necessary.  Would 6 or 7 work just as well?  If it would, as you sharpen it it would not be used up as quickly.  Maybe this is moot as how often will it be used?  Not likely every day, probably not more than once or twice in a year.


----------



## xpylonracer (Sep 15, 2021)

With aluminium the cutting forces are not as great as when cutting gear steel so I wonder if the stepper will have sufficient torque at standstill to prevent the workpiece moving away from the cutter, recently there was an article on the Emco F1 cnc mill iO group detailing the addition of a brake to prevent movement should the need arise.


----------



## Eccentric (Sep 15, 2021)

Hi,

The torque of the stepper in the rotary table is reasonably secure, but I can grab the chuck and rotate it using both hands using some effort.  I do not think what you describe will be an issue  though (but we will see, I'll let you know).  To turn the chuck when the stepper is energized and holding position I need to apply a fair amount of radial force to the chuck.  However,  when cutting the leaf (the space between gear teeth) the forces are not radial to the chuck, that is they do not try to turn the chuck.  The cutter is attempting to push the work piece into the chuck (an axial force vector) and at the same time pushing the work piece away from the cutter (a longitudinal force vector). Because of the force pushing away from the cutter, using a tail stock is a good idea.  

You have made a good observation,  there is quite a bit of vibration cutting steel due to the nature of the interrupted cut, and the chuck cannot move even slightly or the shape of the gear teeth will be compromised.  A solid chuck brake would address this.  I am hoping my small gears do not give me this problem, but we will see.


----------



## Eccentric (Sep 24, 2021)

Now that I have made my gear cutters and a set of practice gears in aluminum it is time to make the real deal. I have two brass gears to make and two steel; I'll start with the brass.  I have to say that I love working in brass, it machines so nice.




I mount a mandrel in the four jaw chuck, I like using a centering four jaw for cutting gears as they are a little more rigid.  I face the mandrel end and cut a few grooves for the super glue to flow into.







I then super glue the gear blank to the mandrel. I use a rag so I don't drip super glue on the ways.  The tail post is used to press the work piece onto the mandrel.  You can see I have punched a center point and scribed the rough gear blank outline.  I have found that the thin super glue works better for me than the thick glue shown in the picture.






This particular brass gear will drive the oil pump and is mounted on a 1/4" shaft, so the first operation is to face the brass, drill and ream to .251".  I then follow up with a #20 drill into the aluminum and tap for a 10-32 screw.  This provides extra holding power to the mandrel while turning down the outside diameter and cutting the gear leafs.






I use a stepper driven 4th axis on the mill table to cut the gear.  It uses the same chucks as my lathe so I transfer the entire chuck and am able to maintain concentricity.  It is very important to precisely establish the correct Z position for the mill spindle, it needs to align with the gear blank center or the teeth will be misshapen.  If you look at the bottom of the gear you can see some scratches in the dykem.  I get the cutter as close to center as I can, then I scribe a line on the blank with the cutter.  the gear is then turned 180 degrees in the 4th axis and the cutter Z position is compared with the scribed mark on the opposite side.  If it is off a little, the cutter Z position is moved to split the difference and the test is repeated.  I have had very good results with this centering method.

Brass cuts so nicely that I cut the leaf full depth at one go, I run the spindle at about 2000 RPM and use the X table power feed to make the cut.  I find that if I cut both directions, I end up with a better finish on the gear tooth.  I use the sound of the cut and the size of the swarf to set my cut speed.





I then transfer the chuck back to the lathe to finish the machining.






My first attempt at making  a steel gear was a fail, the cutter wore out before I made it half way around the gear.  In hindsight I was being too aggressive in my cuts and I was running the spindle too fast.  I may have gone to the other extreme, I successfully used a spindle speed of 500 RPM and I removed .007" of material in a pass.  My cutter cut two pinions of 20 teeth each with no noticeable wear.  I also constantly bathed the cut with oil.  You can see my cardboard splash guard in the right side of the above photo. Another change I made was the tempering I put on the cutter.  The first cutter I made, the one that wore out, after heat treating the 01 tool steel cutter I tempered it to a pretty dark straw color, almost into the blues. This trades off some hardness for less brittleness.  Since the first cutter did not fracture, but wore down, I tempered the second cutter a light straw.  This can be seen in these photos.

An aside: I was wondering what the difference is between a "pinion" and a "gear".  A pinion and gear mesh, the pinion is smaller, is the driver and the gear is driven.  I also have a secondary "pinion" between the crankshaft pinion and the camshaft gear that is really an "idler".  A spur gear is a straight cut gear like mine, these are the simplest kind.  A bull gear is the larger of  two meshed spur gears, ... I digress.

The procedure I used to cut the steel pinions differed from the way I manufactured the brass gears.  

First I made the steel gear blank turned to proper diameter, all machining on both sides completed, the center hole drilled and reamed; basically complete except the teeth.  Then I mounted an oversized steel rod in the lathe chuck to form the mandrel. I turned an area smaller than the internal leaf diameter so the cutter would not cut the mandrel, then I turned a spigot on the end matching the diameter of the pinion blank center hole and not quite as long as the width of the pinion.  Finally I faced and spot drilled the end of the mandrel to interface with a dead center.


I then super glued the pinion blank to this mandrel and moved it over to the 4th axis on the mill.  If you look at the above picture you can see I am using a dead center in the tail stock that has been relieved on one side to clear the cutter.  This provides a ridgid setup.






The total depth of cut for the leaf was .070", for each I made multiple passes of .007" depth increments until I hit .063" then moved on to the next leaf, when all leafs were cut to this depth I locked the mill Y axis at .070" and made another complete turn of the pinion cutting each leaf to this final depth.







The above picture shows the cutter after cutting my two pinions and it can be seen that there is no noticeable wear.  I consider this a win.  



I used excel to create the GCode for the 4th axis.  I know how many steps it takes to turn the spindle 360 degrees so I simply divided this by the number of teeth on the gear.  this is an example:

G1 F500     <-------- this sets the feed rate, or in my case how fast the spindle moves from tooth to tooth.

M18 S5000           <-----------  this sets the stepper motor timeout, if it is too short the motor will

                                                   de-energize before the cut is done and you will lose your place.

G92 X0    <----------- this command sets the current position to zero on the axis

G1 X0.00               <--- this tests to see if we are really at zero

G1 X-5.93             <--- then each of the following commands move to the next tooth position

G1 X-11.85

G1 X-17.78

G1 X-23.70

G1 X-29.63

G1 X-35.55



I copy and paste one line at a time to my motor controller when the time comes to move to the next cut position on the gear.  I am doing this on a laptop with a usb cable to my motor controller.

In my next post I will show the gears mounted on the engine.


----------



## Steamchick (Sep 25, 2021)

Brilliant! Thanks E. I have learned a lot (but probably never try myself).
Keep up the detailed posts.
K2


----------



## awake (Sep 25, 2021)

Eccentric said:


> My first attempt at making  a steel gear was a fail, the cutter wore out before I made it half way around the gear.  In hindsight I was being too aggressive in my cuts and I was running the spindle too fast.  I may have gone to the other extreme, I successfully used a spindle speed of 500 RPM and I removed .007" of material in a pass.  My cutter cut two pinions of 20 teeth each with no noticeable wear.  I also constantly bathed the cut with oil.  You can see my cardboard splash guard in the right side of the above photo. Another change I made was the tempering I put on the cutter.  The first cutter I made, the one that wore out, after heat treating the 01 tool steel cutter I tempered it to a pretty dark straw color, almost into the blues. This trades off some hardness for less brittleness.  Since the first cutter did not fracture, but wore down, I tempered the second cutter a light straw.  This can be seen in these photos.



Eccentric, I am surprised by the speed you are running the cutter. The rule of thumb that I have always used is 500 RPM for a 1/2" diameter HSS cutter cutting mild steel.  If if I understood correctly from an earlier post above, your gear cutter is actually 1.125" in diameter, which calls for a little less than half that RPM. Using a high-carbon cutter such as you have made, I'd want to drop it down even slower.

But since you report that you are getting good cuts at 500 RPM with no discernible wear, either you made one heck of a cutter, or the liberal use of cutting oil is keeping things cool, or the rule of thumb I learned is malarkey - or maybe all three! In any case, well done on making the gears.


----------



## Eccentric (Sep 25, 2021)

Andy,

Thanks for the input, I did not calculate the best spindle speed as I should.  I have seen calculators, but never used one. I think I got lucky with the high spindle speed as I used a small depth of cut and a slow feed rate.  The steel swarf came off as tiny bits of glitter in the dripping oil.  

When the spindle speed is running slower I have a hard time hand feeding the work piece into the cutter slow, a little bit of a jerkiness will present too big of a cut and the cutter makes a twack sound.  The power feed will run this slow, but it kind of drives me crazy because at the really slow feed rates it takes what seems like a long time to take up the backlash when starting the cut. I know, I know, I need to be more patient, right?


----------



## Nerd1000 (Sep 26, 2021)

You probably got away with it because of the low radial engagement of the cutter, basically each tooth only cuts for a fraction of a revolution then has the rest of its time to cool down (by conducting heat into the body of the tool) before re-entering the cut. If you tried the same speed with a carbon steel tool in a turning operation it would probably burn up in no time.

My general rule of thumb is that carbon steel cutters need to run about 1/2 the rpm of HSS. Have even machined 4140 HT with carbon steel in this way, but it took forever and needed a lot of water based coolant to keep the temperature down.


----------



## L98fiero (Sep 26, 2021)

Nerd1000 said:


> You probably got away with it because of the low radial engagement of the cutter, basically each tooth only cuts for a fraction of a revolution then has the rest of its time to cool down (by conducting heat into the body of the tool) before re-entering the cut. If you tried the same speed with a carbon steel tool in a turning operation it would probably burn up in no time.
> 
> My general rule of thumb is that carbon steel cutters need to run about 1/2 the rpm of HSS. Have even machined 4140 HT with carbon steel in this way, but it took forever and needed a lot of water based coolant to keep the temperature down.


Carbon steel cutters should generally be run about 18-20 surface feet per minute. As for which 'carbon steel' to use, A2 is slightly better than O1 but not much, it's used more industrially because it's an air hardening steel and doesn't require oil quenching/tempering and that makes the heat treating process quicker and cheaper. Here is a chart from the book 'Heat Treatment, Selection and Application of Tool Steels' by William E. Bryson, it's a good general tool steel selector.


----------



## Nerd1000 (Sep 28, 2021)

L98fiero said:


> Carbon steel cutters should generally be run about 18-20 surface feet per minute. As for which 'carbon steel' to use, A2 is slightly better than O1 but not much, it's used more industrially because it's an air hardening steel and doesn't require oil quenching/tempering and that makes the heat treating process quicker and cheaper. Here is a chart from the book 'Heat Treatment, Selection and Application of Tool Steels' by William E. Bryson, it's a good general tool steel selector.View attachment 129420


Hmm so that would be more like 1/4 the speed of HSS. Perhaps I got away with 1/2 due to only taking light cuts and keeping it flooded. Or maybe the tool was actually some kind of strange HSS that spark tests like high carbon steel, I got it in the toolbox with my lathe so I'm not entirely sure what it is. Concluded that it was carbon steel when I sharpened it and the sparks were yellow white feathery sparkles rather than orange lines like you get from HSS.


----------



## Eccentric (Sep 28, 2021)

In My Humble Pinion





While I am in the mode of making gears, I thought I would make the last two, the oil pump pinions.  They are .375"  in diameter, 32 DP, 20 degree pressure angle, and have 10 teeth.  I am going to make them in brass so I figured I could get away with a single flute fly cutter to cut the gear leafs.  I am making the cutter from 01 tool steel on the CNC router. I use a gear profile spreadsheet I have for the cutter design, then capture the cutter in SolidWorks with an 8 degree clearance angle. To cut this clearance angle I clamp the 01 tool steel blank at an 8 degree angle as seen in a few photos below.  So I take a section of the cutter in the following CAD model to present this tilted cutter blank to the mill.





Above is how the cutter will sit in the vise and how it will be cut.  The blue area is the remaining part to be used, the rest of the model is trimmed away. This CAD model is then transferred to Fusion360 to generate the tool paths






I am using a two flute 3/32" flat end mill because I have an internal radius of less than.125", otherwise I would have used my go to 1/4" end mill.  I am making lots of tiny little cuts.  Above is a simulation of the tool paths.





Above is the completed cut in the CNC router vise.  I have used a second scrap cutter blank to even out the vise clamping force. You can see that it is clamped at the 8 degree angle.






This is the standard heat treating kit with the MAP gas torch, boric acid to eliminate scale and quenching oil.  The tin can is used to hold boiling water to remove the boric acid after heat treat.  I warm the cutter tip and roll it around in the boric acid which adheres and melts.  Then I bring the cutter tip to a bright red hot and plunge in the quench oil. 



After removing the melted boric acid by rinsing in boiling water, I temper the cutter by heating it with the torch on low.  I aim the heat at the middle of the cutter and watch the color change propagate out toward the tip, when I see the light straw color I am aiming for, I again plunge it into the quenching oil.  Finally I sharpen it on the Arkansas stone.





Above is the mandrel used to hold the cutter.





I prep the pinion blank by bringing the OD to size, drill and ream the 1/8" hole down the middle.  Then I transfer the blank and chuck to the 4th axis on the mill.





I set my gear cutting rig up with a tail post, but the pinion is so small the cutter hits the dead center in the tail post, even though it was relieved.  Cutting the pinion hanging into space like above causes the blank to vibrate and there are slight machining artifacts on the teeth.  since this is not a set of power train gears, these should have no effect on the function of the oil pump.





Once the teeth are cut, it is back to the lathe to part them off and finish the ends.







Done with gears,  whew.


----------



## Basil (Sep 28, 2021)

Thanks, nice work. I have not made gears yet!


----------



## Eccentric (Sep 30, 2021)

This is the current state of my design for the Wallaby:





I need to complete the work on the front of the engine including the Oil Pump housing, ignition triggering system and the distributor.  The oil pump housing needs its intake and output on the same side, so I need to work on that. I think the timing sleeve with a magnet for the ignition trigger is straight forward, but I need to design the little housing for the hall effect sensor.  The distributor for the two cylinders will be driven from the end of the camshaft.

But I am going to direct my attention to the design and fabrication of the camshaft next.  I have deviated from Westbury's design by using ball bearings at each end of the camshaft.  I will be using 1018 cold rolled steel and case harden the cam lobes.  This is the current state of the camshaft design:




I know this is not dimensioned using proper GD&T standards, but when I am machining I like LOTS of dimensions. 

Below are the lobe designs using numbers gleaned from Westbury's construction article:  Cylinder 2's lobes are 180 degree mirror images of cylinder 1's. The nose radii are reference dimensions, to specify them would over constrain the design as all curves are tangent and sufficient to describe the cam profiles.





My machining approach is to use the lathe to turn all features with the exception of the cam lobes themselves.  I am going to then use a 4th axis on the mill to machine these. This will be the adventure.  I am going to machine some aluminum test articles first.

One thing about model engines (and full size engines as well) I dont' quite understand is the need to be able to adjust cam timing.  The timing of the valves with repect to the crankshaft are rigidly defined by an engine design, so why do I need to adjust the cam position on the cam timing gear?  Is it because of variation in manufacture of the timing gear train?  Am I just adjusting out slop or inaccuracies in the manufacture of the associated components?


----------



## Basil (Oct 1, 2021)

When receiving a performance cam they come with a degree sheet showing open and closing events and duration usually at 0.050” lift . Degreeing a camshaft with a degree wheel on the crankshaft and dial indicator on the lifter just makes sure the setup checks out as designed. Adjustment brings everything in line if not correct.
When dynamometer testing it is sometimes advantageous to advance or retard a cam to improve low end torque or to improve top end power.
Valve lash to some degree can also help with getting the desired opening and closing events and adjusting such things as overlap.


----------



## Eccentric (Oct 9, 2021)

*Camshaft Continued*

The majority of the last week has been spent working on tool paths for the Camshaft Lobes.  This is my first exposure to using a 4th Axis on the CNC Router. Below is my first attempt cutting an exhaust cam lobe on a piece of test aluminum rod.  I used a ball end mill for the entire operation.





Operation in process





Operation complete.  I was quite pleased with the surface finish and the dimensional accuracy.





I continued to experiment with various tool path options ending up using a 1/4" flat end mill for the roughing and then a final pass with a 1/4" ball end mill.  I offset the tool .3" to the side so I used the edge of the cutter, not the center.  I worked initially in aluminum, then a final test with steel.





The camshaft print.  





First I rough machined the camshaft focusing on the cam lobe blanks.  These are 5/8" in diameter and 5/16" wide. I went back and forth on how much lathe work I wanted to do before milling the cam lobes.  I finally decided to minimize the amount of lathe machining before moving to the CNC router to minimize lost work in case of a failure there.





Instead of creating a tool path for the entire camshaft, I created two tool paths for the intake lobe and two tool paths for the exhaust lobe (roughing and finishing).  This required four set up changes as I would re-zero the CNC router and rotate the camshaft to the proper orientation for each cam lobe before starting the machining on each.  To insure I didn't skip a step or mess one up, I created a checklist for the machining of the cam lobes.





Here three of the four cam lobes have been machined from a 1018 cold rolled steel rod on the CNC router.





Back to the lathe to complete the machining.  Above I have completed both bearing surfaces, you can see a bearing test fit next to the live center in the tail stock.  And started working on the taper that will secure the cam timing gear. 





Once I finished the machining and cut off the cam I found that the camshaft was too tight between the bearing holders and the taper need some more material removed to properly mesh the cam timing gear with the idler timing gear.  I had to figure out how to chuck up the camshaft again to do this work.  Gotta love collets.






Camshaft Installed in the Engine.  The outside lobes are exhaust and the two center lobes are intake.  You can see the timing of the lobes.

I still have a little bit of clean up on the camshaft, then I need to case harden the cam lobes.  I sure hope this does not ruin it.


----------



## Eccentric (Oct 13, 2021)

Valve Train



I have been working on some odds and ends in the valve train.






This is a rocker arm cut from 1/4" mild steel.  I mount it on a mandrel and machine the sides in the lathe.





The rocker arms are handed, that is the spigot is longer on one side than the other






Included in the above photo is the rocker arm pivot bracket.

Below are some shots of the fabrication of the Tappet guides cut from bronze.





Using a tap in the lathe, quicker and easier than cutting threads.





A threaded fixture used to cut the hex heads on the tappet guides.






Finished tappet guides, they will thread into the four yet unthreaded holes in the crankcase



Below is the final operation in the fabrication of a valve guide.




I am using a split bushing to mount the valve guide in the mill vise to prevent marring and deformation while drilling the side hole.





Completed valve guide.





The valve guide is test fit into the head, the small 45 degree valve seat is highlighted.  This was cut using the cross slide set to 45 degrees in the same setup used to drill and ream the internal holes.


----------



## Eccentric (Oct 14, 2021)

Wallaby Valve






This morning I made a valve for my 4-stroke Wallaby.

The valves are machined from 303 stainless steel.  I started with a fail.  I had too much stick-out when I tried to cut the retaining ring slot.







I had success with the slot by cutting it with no stick out at all:






Then I continued machining in a couple of smaller segments




This works so much better than the last time I made valves, turning the whole length on centers.













I tested the quality of the seating of the valves using a technique I learned from Terry Mayhugh.  My method is much simpler and less scientific.  I  pull the vacuum through the rear of the valve cage, past the stem of the valve.  I seal the side hole and then take time measurements to see how long it takes to bleed down in different configurations.  With the valve held slightly open it takes 3 seconds to bleed down--this is my baseline.  This measures the leakage between the cage and the valve stem.  Lightly holding the valve closed with my thumb the time jumps to 30 seconds to bleed down, this represents the valve spring holding the valve closed.  If I do not press on the valve with my thumb and just rely on the vacuum  to seal the valve it takes 15 seconds to bleed down. 




Since I pull the vacuum down past the valve stem, the bleed down times do not mean much in themselves and cannot be compared to times others may get.  They do indicate that the valve is sealing against the cage and that there is not a misalignment or major flaw in either the seat or the valve.  The quality of the seal really can't be determined by this simple method, just that there is a seal.





I feel confident that I have the techniques down now to build the balance of the valve cages and valves.  Back to it.


----------



## Eccentric (Oct 22, 2021)

*Flywheel*

The most important aesthetic criteria I have for a flywheel is that it runs truly true.  I want my flywheel to appear to be a stationary blur, if that makes sense.  So I strive to machine all surfaces in one setup, and a setup representative of how the flywheel mounts to the engine.  As far as the functional design, I follow George Britnell's advice: "The flywheel in total doesn't need to be heavy but rather just the weight at the rim. Most flywheels (hit and miss type) are spoked. This is to reduce the overall weight while still providing the force needed to overcome the compression. If the flywheel is too light the engine will still run but it won't run slowly. If the flywheel is too heavy the engine will run but won't respond to throttle openings properly." 

I liked the look of my finished gears with the six lightning holes, so I went with that design here.  I also like to use a separate split taper collar as opposed to tapering the crankshaft.   In the picture below I have highlighted the taper collar, unfortunately it is almost the same color as the flywheel and hard to discern.  I use the compound to cut the 10 degree inclusive angle on the flywheel and split taper collar, and use the same setup to do both to insure the angle is identical.  I make the taper collar first, then leave the 5 degree offset in the compound, machining the flywheel using just the cross slide until the internal taper is cut.




(Bonus question,"What is wrong with the pistons in the above model?")





Design of the flywheel and split taper collar.

I face the front of the flywheel to create a relatively flat side that I then mount in the centering 4 jaw chuck.  I drill the center hole to the small diameter of the taper collar, then cut the taper into the flywheel, using the collar to test fit until it is just even with the faced surface (back side).





I fabricate a mandrel to the same dimensions as the crankshaft. Then I mount the flywheel just as it will be mounted on the engine.






At this point I machine the complete flywheel in this one setup.  I even take a tiny skim off the back of the flywheel as deep in the X direction as I can without hitting the collet nut, to true this edge as well.








Then it is over to the mill to drill out the large lightning holes.  I drill these in five increments not including the center drill.  I use parallels underneath to support the work piece, moving them to insure they don't get hit with the drill bit. I use aluminum packing to protect the outer surface.

Here are a couple of pictures of the flywheel test fit on the engine.








The flywheel ended up weighing 19 ounces.  I still need to balance it and I think I would like a larger chamfer on the center mounting spigot.


----------



## Eccentric (Nov 6, 2021)

*First Assembly*

I completed the first assembly of all of the major components on the Wallaby project.  This felt like a major milestone. I ran into a minor problem with my CAD model that was realized in the actual build- the pistons interfere with the crankcase at the very bottom of the stroke.  If I had done a more thorough study of the CAD model I would have discovered this.  So my crankshaft only turns through about 350 degrees.

The two following photos illustrate the area of interference with the second photo being an extreme close-up of the actual interference area.  This was very easy to fix as I clamped the crankcase in the mill vise and took off a little extra material.  I also corrected the CAD model and drawings, of course.









I have also been working on some of the smaller details such as drilling the oil gallery holes in the crankcase.  Oil is delivered under pressure from the oil pump to the side of the crankcase where it is routed to the end of the cam shaft and to the middle main crankshaft bronze bearing.  Oil will then travel down the cam shaft and through small holes to oil each of the camshaft lobes.  Oil delivered to the crankshaft middle bearing will travel through oil galleries in the crankshaft to the two big end bearings of the connecting rods.










I have also been in a production mode for the rest of the parts in the valve train.  I had to fabricate multiple valves, valve cages, rocker arms, push rods, and rocker arm bearings.  I slip into a different way of working when I am building multiples of something that I have already developed the process for fabricating.  Developing these process is part of making the original prototype where it can take me several parts to get the steps down.  When I go into the production mode I will often perform each operation on all the parts before moving on the next.  For example, I might complete the lathe operations for a set of parts before I move to the mill for milling operations.  One thing I have learned, I should make more than just the right amount of parts; I should make an extra.  There are a couple of parts that I made a mistake on, now I have to repeat the whole production process for a single part.  You can almost fabricate multiple parts in the same time as a single part.






I also worked on the display stand for the engine.  I need to figure out the other items such as radiator, fuel tank, electronics, etc. I have seen many fine examples on this forum.


----------



## Eccentric (Jan 22, 2022)

Tappets

Today I got back to making parts for the Wallaby, these are the tappets.  They were a pretty straight forward lathe job, I used a 1/8" ball end mill to make the pocket for the 1/8" push rods.  These are made from 5/16" drill rod, the shank is turned down to 3/16" for a smooth fit in the tappet guide.  I have not decided whether I will harden them or not.






I have been distracted from the Wallaby by work in my new design, a 97 cu in Offenhauser Might Midget engine.  I have been toying with the idea of creating a YouTube series on its construction.  Below is a video of the machining the inside of the Wallaby piston on a CNC router.  This video was the second I produced and I am still on the fence whether I want to get into this new way of sharing my projects.  Let me know what you think.




Thanks,  Greg
GregsMachineShop.com


----------



## Charles Lamont (Jan 23, 2022)

Have you checked how the tappets ride on the cams? If the faces are only 3/16" diameter, I think it is highly likely that that you will get corner contact.

(Later, for the record: this post was based on a now corrected typo in eccentric's post above. But for that typo, I probably would not have noticed the problem)


----------



## ownthesky2010 (Jan 23, 2022)

When I built my flat twin engine I also machined the internal piston features in my CNC mill. The easiest way was to machine the piston from square and leave about 3mm of excess square stock on the crown to use for indexing and location and then just face it off after.


----------



## xpylonracer (Jan 23, 2022)

Greg

If the push rods are 3/16" diameter wouldn't it be better to use a 3/16" ball end mill to make the pocket in the tappet or are the push rods tapered to 1/8" at the end ?

xpylonracer


----------



## Charles Lamont (Jan 23, 2022)

Out of interest, I have now had time to do some calculations on the cams. If the cams are made to Westbury's specification, the inlet cam would have a nose radius (which he does not specify) of 0.040" , and to ensure that the the full 3/16 width of the cam was always in contact with the flat face of the tappet, the latter would need to be 13/32" diameter. Allowing the contact line length to drop to 3/32" at the extreme would mean you could get away with a tappet 3/8" diameter.

Westbury's specified 5/16" is too small, and this is an error he made on several engines. Mind you, he would have been designing with pencil and paper methods, while I arrived at the figures above with a combination of pythagoras theorem and CAD. The whole lot could have been calculated, but the CAD saved me a bit of trigonometry.


----------



## Eccentric (Jan 23, 2022)

Sorry, I misspoke. The tappets are made from 5/16" drill rod, the shank is turned down to 3/16" for a smooth fit in the tappet guide. I used a 1/8" ball end mill to make the pocket for the 1/8" push rods.



Charles,  what you describe about the size of the tappet head is very interesting.  Below is a cutaway of the engine:






And below is a close up of the cam lobe contacting the tappet as the lift begins/ends. I can see what you describe, the tappet head is too small and the cam lobe is pushing against the edge of the tappet, not the face.






And with the valve full open, the tappet needs to rise into the hole above it, which now is .406".  So your suggested 3/8" should fit at full lift.





Now with your suggested 3/8" top:






Closeup






Even the intake lobe with the smaller cam lobe nose radius pushes on the bottom of the tappet, not the side.



Below is a closeup cutaway on the other axis and it can be seen with the larger tappet face, we are still OK.








Thanks Charles,  I never would have noticed this.  Well I guess I'm back in the workshop making new tappets.


----------



## Mechanicboy (Jan 23, 2022)

And the cam is in off side to tappet to prevent wear out the cam and tappet? With cam off side to tappet help to rotate the tappet and lasting long time.


----------



## Charles Lamont (Jan 23, 2022)

As you see, I have updated my post with a drawing. The exhaust cam will have a larger nose radius, and that makes the situation easier.


----------



## CFLBob (Jan 23, 2022)

Eccentric said:


> I have been distracted from the Wallaby by work in my new design, a 97 cu in Offenhauser Might Midget engine. I have been toying with the idea of creating a YouTube series on its construction. Below is a video of the machining the inside of the Wallaby piston on a CNC router. This video was the second I produced and I am still on the fence whether I want to get into this new way of sharing my projects. Let me know what you think.



If it's not too late to open this can of worms, I tend to like videos, but you're spot on about needing a whole bunch of skillsets to pull off good ones.  Good video editing software is a must.  As is writing a script and reading an audio track in once you get the video sequences you like.  You need a place with both good acoustics and good lighting.   There's a guy whose stuff I've watched (Russtuff?) who generally doubles or triples the video playback speed for things like hollowing out that piston (as you did when you showed the cutter digging in at the bottom of its cut).  

I've put up many videos of some operation or another but have yet to take the plunge on a microphone and recorder.   Because of that, they'll be like one pass around a part or something simple like that.   Nothing like a complete look at how to make a particular part.

Good videos can condense the information: the old "a picture is worth a thousand words" line.  Getting good videos isn't trivial.  Too many kids just turn on the camera.  All the hard stuff needs to be planned in advance and I think it's likely to be a pile of work.


----------



## awake (Jan 24, 2022)

CFLBob said:


> If it's not too late to open this can of worms, I tend to like videos, but you're spot on about needing a whole bunch of skillsets to pull off good ones.  Good video editing software is a must.  As is writing a script and reading an audio track in once you get the video sequences you like.  You need a place with both good acoustics and good lighting.   There's a guy whose stuff I've watched (Russtuff?) who generally doubles or triples the video playback speed for things like hollowing out that piston (as you did when you showed the cutter digging in at the bottom of its cut).
> 
> I've put up many videos of some operation or another but have yet to take the plunge on a microphone and recorder.   Because of that, they'll be like one pass around a part or something simple like that.   Nothing like a complete look at how to make a particular part.
> 
> Good videos can condense the information: the old "a picture is worth a thousand words" line.  Getting good videos isn't trivial.  Too many kids just turn on the camera.  All the hard stuff needs to be planned in advance and I think it's likely to be a pile of work.



As someone who has made a grand total of two (two! count 'em! two!) tutorial videos, I agree with everything CFLBob says above. I will add one other thing: consider carefully whether the videos actually need to show your face. In general, a "talking head" is less appealing to me than other options (e.g., a voice-over of clips or even stills of the machining process). But IF it is important to show your face, consider investing a few bucks in a simple teleprompter. It is astonishingly easy to put one together, using anything from cardboard to 3d printing, that works very well indeed. The key ingredients are a piece of clear glass or plastic at a 45° angle, through which the camera looks, but which reflects the image of a tablet or even a cellphone. Here are a couple of pictures of one I made, that I use with a surplus Android tablet and the nanoPrompter app in my fancy (?), high-tech (?!?) home studio:


----------



## Eccentric (Feb 2, 2022)

*Oil Pump*

Made the oil pump today.  Both the oil pickup from the sump and the oil gallery fitting in the crankcase are on the same side of the engine.  So I had to do some creative oil routing in the pump so the fittings could be on the same side of the engine to simplify the oil tube routing.

I fly cut a piece of stock on both sides to the correct thickness, then cut the inside and outside features on the CNC router.






When I made the oil pump gears I beveled the edges of the gears, not a good idea for the oil pump gear as you do not want any leakage around the gear corners.  Fortunately the gear were a little to tall, so I put them in the oil pump housing and fly cut one side....





then flipped the gears over and fly cut the other side flush with the oil pump housing.




The gasket between the oil pump housing and the oil pump cover should provide enough space for smooth operation.

Then I reamed the shaft holes...




Then I milled off the oil pump housing from the base stock.  Drilled and tapped the holes for the oil line fittings.




 Still need to deburr the holes with the counter sink tool, but I think the pump will pump.




The gear with the shaft turns counter clockwise, delivering oil from the bottom fitting to the top.


----------



## Eccentric (Sep 2, 2022)

Wallaby – Distributor​




The first run of the Wallaby was done without a distributor, I used two separate ignition systems triggered by the same hall sensor on the fly wheel firing both spark plugs simultaneously.  This was just an expedient to get to first run, but now I want to complete the distributor and use a single ignition system.
I planned to machine the distributor body, cover and rotor from Delran, and 3D printed the parts first as prototypes.  But the quality of the parts are good enough to use.  The distributor body is separated from the engine by the timing case so should not get too hot.

The distributor design is straight forward, the rotor mounts directly on to the end of the camshaft and there are a number of precision brass parts that make up the electrical distribution system.

An exploded view of the distributor is shown below.  





I first printed the plastic parts on the 3D printer. Below is the Distributor body still adhered to the 3D printer bed.  I used ABS filament which does not get soft until 105 degrees C.





Now its time for the brass parts. I made the center rotor contact by first drilling the three mounting holes and rough cutting the part from a 1/16″ sheet of brass.





Then I mounted it on a prepared fixture and turned the outside diameter to spec on the lathe. Finally the flat was machined back on the mill.





The three mating contacts were first turned on the lathe, the center hole drilled and countersunk.













A fixture was made that would allow the inside and outside diameters to be turned on the lathe.  First I turned a bit of scrap aluminum with a center hole for a zero reference point on the lathe, then transferred it to the mill.  On the mill I centered the part and placed mounting points for the contacts equidistant from the center reference point.





Then back to the lathe where I first turned the outside diameter.





Then bored the inside diameter.








Below is a test fit of the rotor contact.





Looks good.





Below are the finished contacts:





The contacts fit well in the distributor housing.





The wire terminals were then machined.  I drilled and threaded the holes in the brass rod first.





Then turned the outside diameter and drilled the small hole for the spark plug wire.





I am using 22 Gauge wire with 40KV rated insulation for the spark plug wires.  Below is a test fit.





The terminals were then soldered to the wires.





Above is the final installation on the engine.  I am pleased with the smooth motion and tight tolerance of the distributor contacts.  We will see how the 3D printed parts hold up.


----------



## xander janssen (Sep 3, 2022)

Very nice. How big is the gap between the contacts?


----------



## Eccentric (Sep 6, 2022)

Xander,

I went for .005" gap, but in the real world, the rotor is not perfectly restrained in the distributor housing and the center rotating contact is not perfectly concentric with the outer fixed contacts.  I found that the center contact was touching one of the contacts and had about .010"-.005" clearance on the other two contacts.  But there was no resistance when turning rotor and the engine ran fine.  It is OK if there is a small spark gap between the contacts.


----------



## Eccentric (Sep 7, 2022)

Below is a short video of my 30cc Wallaby running. The Wallaby is my second IC engine build and my first to actually run successfully. I developed a set of plans for the engine from a construction article by Edgar Westbury published in "The Model Engineer" in 1962. Mine is built completely from bar stock and thus does not use any castings. The design changes include the use of ball bearings on the crankshaft and camshaft, but most changes were to ease the manufacturability of the components from bar stock.




I still have a few issues to iron out. The aquarium pump I use to circulate the coolant stops once the engine starts running, and when the engine quits, the pump resumes running. It is a DC brushless drive pump and I assume that my ignition system is interfering with the internal drive electronics of the little motor.





The DC brushless fan used on the radiator runs fine.



Most of the finishing work left is on the display stand and the packaging of the support equipment such as coolant system and ignition system. I designed my own electronic ignition using an Arduino UNO and I would like to package it nicer.







I created two versions of the plans, one assumes the use of a CNC router on some parts, and the other simplifies a few components to allow construction with only a mill and a lathe. If anyone is interested in building my version of the Wallaby, please feel free to contact me.


Greg


----------



## jamesmattioli (Sep 15, 2022)

Eccentric said:


> Below is a short video of my 30cc Wallaby running. The Wallaby is my second IC engine build and my first to actually run successfully. I developed a set of plans for the engine from a construction article by Edgar Westbury published in "The Model Engineer" in 1962. Mine is built completely from bar stock and thus does not use any castings. The design changes include the use of ball bearings on the crankshaft and camshaft, but most changes were to ease the manufacturability of the components from bar stock.
> 
> 
> 
> ...



Ciao,  mi piacerebbe fare un motore come il tuo,  chiedo se hai tutti i disegni per usare tornio e fresa , grazie mille


----------



## Eccentric (Oct 16, 2022)

I've been having fun making videos recently, so I decided to make a youtube series on how to build the Wallaby from Scratch.  I've been working the last couple of months putting the finishing touches on the plans and am now ready to capture the build process on video.  The first in the series:


----------



## D and D (Oct 17, 2022)

Eccentric said:


> I've been having fun making videos recently, so I decided to make a youtube series on how to build the Wallaby from Scratch.  I've been working the last couple of months putting the finishing touches on the plans and am now ready to capture the build process on video.  The first in the series:



Tremendous thing you are doing. Lets hope we see a few more. top shelf job thanks.


----------



## Eccentric (Oct 23, 2022)

Here is the first machining video in the 30cc Wallaby 4 stroke engine construction series.   I am starting with the simplest parts first to ease into the construction process.


----------



## Eccentric (Oct 30, 2022)

In Part 1B of the "Build your own Wallaby 30cc Twin" series. I go into depth on how to use Fusion360 to create toolpaths and Gcode for a simple 2D profile part used in the engine display base.  Then I cut it out on the home made CNC Router. 

The plans and fusion360 files can be found here: Downloads – Wallaby Twin Four Stroke IC Engine – Greg's Machine Shop


----------



## NapierDeltic (Oct 31, 2022)

Hi Greg, I like very much your build and I appreciate much more your effort in presenting a full tutorial + plans. Though not first on my list - I'm aiming for a more basic design that could be my first 4 stroke IC motor, I consider it a straight forward. I like it, like the presentation style and consider it very valuable -if I can say so (including CAM, though I'm not able to). IC engines are very complex things and many attempts fail due to lack of linking several parts of the chain (I mean what somebody intend to and what they find related). There has to be a balance between thinking and doing and many times info - though valuable in content - puzzles people and mislead them. Too much options or not applicable top options... I hope I'll have the wisdom for myself... Good luck in  your enterprise! And for sure your project is in top 5 on my list.


----------



## Eccentric (Nov 3, 2022)

Here is the next video in the Wallaby build series. These initial videos are building skills that will be used throughout the build.  This one covers lathe work focusing on a simple custom form tool to create an inside radius for a cosmetic washer.



This is the Wallaby engine display base we are building first to challenge ourselves with some simple lathe and mill work.


----------



## Steamchick (Nov 4, 2022)

I like the attention to presentation. Beats my recycled cardboard boxes!
K2


----------



## Eccentric (Nov 10, 2022)

This is the first in the 3 Part Mini Series on how to machine the Wallaby Cylinder block.  Is this how you square up stock? 



Plans for the Block are here:


			Downloads – Wallaby Twin Four Stroke IC Engine – Greg's Machine Shop


----------



## Eccentric (Nov 19, 2022)

Finishing up the Cylinder Block for the Wallaby:


----------



## lantain1982 (Nov 23, 2022)

Eccentric`s approach to Westbury`s Wallaby is a fresh approach to a well established model.   
Have decided to follow the project and have just completed the engine stand with some minor modifications regarding shape and profile and fastener concept.    This departure was prompted by personnel choice and material availability.
Currently the cylinder block is being worked on.        I would point out that all my machining will be by manual means, no CNC or digital readouts.   Traditional measurement means and the height gauge should get a bit of a workout.


----------



## e.picler (Nov 24, 2022)

Hello Greg!
Congratulations on your project. What you are doing with the videos is a real School on how to develop and machine a Model Engine.
Very nice initiative.

Edi


----------



## lantain1982 (Nov 29, 2022)

The "Westbury" cylinder block has been machined.   A great deal of material had to be removed and one had to take care not to push the 1/4" end mill too hard when working at full depth.  Climb milling was adopted which also gives a smooth into corner blending.    Crank case and sump material has been purchased with timing case component making out taken place.
Photo to follow.


----------



## Eccentric (Nov 30, 2022)

Lantain1982,

You have a great beginning on your 30cc Wallaby. I would like to see  more pictures and follow your build log.  What would you think about starting your own build thread? I will be an avid watcher.


----------

