Quarter Scale Merlin V-12

[Blogwitch]

Terry,
I have to disagree with you in that commercial ones are not available. Have a look at this video from Mircona, start at 1 minute and it shows the type I bought from off ebay for about £25 each, I bought a left and right hand one, plus a load of different tips, including half round ones for giving the stress reducing corners in deep cuts. The advantage of these tools is that they can cut in all directions, not just in and out, but side to side as well (within logical reason). The ones I bought will give a depth of cut of around 1.5".

[ame]https://www.youtube.com/watch?v=ZUwJXZEyctI[/ame]

I am not trying to persuade you into buying any, but maybe to have a look at how they are made, to give you that long range support. I know of a couple of people who I sent the link to and have copied this design and fitted their own tips to it, and they have worked very well indeed.

This is mine at work doing a bit of deep parting.

[ame]https://www.youtube.com/watch?v=BG4qEw3eMcQ[/ame]

Great work and best of luck with the rest of your build.


John

 

[digiex-chris]

I was able to make an 1/8" HSS parting blade into a bifurcated tool for this purpose and make it perform cutting sideways by making a toolholder for it instead of using a standard parting blade holder. Rather than clamping down like most parting blade tool holders do, I cut a slot in the side of my tool holder the depth of the parting blade, then made a clamp to clamp the blade sideways, giving it more side-to-side support. I also used a T shaped blade, so that it was easy to round the edges and make some relief on the sides. I broke the tip with the edge of my grinding wheel. I also added a few degrees of top rake to ease the cutting somewhat. I used it mostly for light finishing cuts and cleaning up the corners. I'd done the roughing on the milling machine using my dividing head to turn it.

 

[DICKEYBIRD]

Can you set up a faceplate on the 4th axis & a tailstock in the mill and make the roughing cuts with an endmill? A rougher in your Tormach would move metal quickly.

Some of the videos of "real" crankshaft manufacturing show it being done that way. I think they were mounted on center and the Z-axis traveled up & down in sync. 'Tis somewhat beyond hobby CAM though!

Just a thought.

 

[mayhugh1]

John,
Thanks for the heads-up. The Mircona tools look like an optimum solution. I checked Ebay but only found some inserts currently available. I wish they had a US distributor since overseas purchases directly from the manufacturer don't typically seem to go well for me, and they nearly always end up with my credit card being suspended even when I warn my credit card supplier.
What I was referring to in my post was the lack of a deep blade holder for my Iscar GIP inserts. These inserts cut steel very nicely, have a usable corner radius; and I was even able to do limited side-to-side cutting with them. The holder I have for them is a similar style to the Mircona holder but nowhere deep enough (I need 1.7" depth), and since the insert shape is different, the method of gripping it is different.
I also have a number of no-name GTN inserts and a usable deep blade holder for them. Although, on a good day, I can usually use the combination with aluminum, these particular inserts work poorly with steel, and there is no side-to-side cutting with them. There is a bewildering selection of inserts available, and it's expensive to buy and test especially when the name brands can cost more than $20 each; and a minimum buy of ten is often required. I may use what I have for the interrupted clean-up of the mill-roughed bearings, but so far George's cutter looks like the best solution for finishing without investing a bunch of money. - Terry

 

[mayhugh1]

Can you set up a faceplate on the 4th axis & a tailstock in the mill and make the roughing cuts with an endmill? A rougher in your Tormach would move metal quickly.

Some of the videos of "real" crankshaft manufacturing show it being done that way. I think they were mounted on center and the Z-axis traveled up & down in sync. 'Tis somewhat beyond hobby CAM though!

Just a thought.

I'm going to rough the mains out on the mill but with the workpiece held in a vise and manually indexed. I'll probably use the fourth axis for the crankpins. I just found out I can remove material a lot faster if I put the cutter directly in an R-8 collet rather than use a TTS toolholder, but this causes clearance problems between the fourth axis and spindle. The vise also gives me a more rigid set-up for roughing. - Terry

 

[mayhugh1]

I decided to tackle the main bearings first. My hope is to completely finish them before starting on the crankpins so I'll have all the needed cutting tools in hand and some experience with them before dealing with the more complicated offset turning. Finishing the main bearings first will also make them available for extra workpiece support during the offset operations.
After some playing around with my CAM software I found I could easily generate the g-code needed to rough out both the main and crank pin bearings. I could have used my fourth axis to automatically index the workpiece, but I was concerned about the rigidity of the relatively long workpiece during the heavy roughing operations even with tailstock support. I chose, instead, to support the workpiece horizontally in my mill vise and to manually rotate it in 60 degree increments for the main bearing roughing. For roughing, precise indexing isn't really required; and an electronic protractor on the end flats of the workpiece provided more than enough accuracy. This setup will be more troublesome for the crankpins with their deeper roughing depths because of interference with the vise. The fourth axis becomes more attractive for roughing the crankpins since I'll be able to support the center of the crank with a bearing block under the center bearing.
Because I have no experience with machining Stressproof, I ran some experiments on my Tormach to find a set of usable feeds and speeds. My tests were with a 4 flute 3/8" carbide end-mill using a 1.7" stick-out since I'll need this later for the crankpin machining. With the cutter mounted in the spindle in an R-8 collet (no TTS toolholder) I eventually arrived at a .150" DOC running at a 20 ipm and 2500 rpm. I tested a portion of the g-code by roughing out a full bearing in a piece of scrap. There was little to no chatter, the chips came off with a light straw color, and the load meter showed my mill was running at only about .6 hp. With this removal rate the roughing operation for all seven main bearings required about 70 minutes of actual machining time. After it was completed I saw no visible wear on cutter, and so I'll be able to re-use it on the crankpins.
The workpiece was then moved to my lathe's 3-jaw plus tailstock for the next roughing operation. This time the hexagonally shaped main bearings were turned to get them circular. I used an NGTN-3-PV52 carbide insert in a blade holder extended 1.7" beyond the tool post with the lathe running at 120 rpm for this interrupted cutting operation. This particular 1/8" wide blade and a companion box of equally wide no-name inserts was one of my first Ebay tooling purchases many years ago. It taught me that my lathe didn't like cheap 1/8" imported inserts, and so the parts had been languishing in one of my drawers. I decided to try them on this interrupted cutting operation since I was worried about chipping my more useful ($) inserts. I won't say the cutting went smoothly, but it was fairly quick, and plunge cutting accomplished what I needed. Once the bearings were turned fully circular and the insert was cutting continuously, though, the chatter was too excessive to continue especially on the bearings downstream from the chuck.
I was left with nearly .100" excess diametral stock that I needed to remove from each of the seven bearings before moving on to the finishing operations. I used a Dremel diamond abrasive disk to cut a Britnell notch in the center of the cutting edge of the insert to reduce its contact area with the workpiece. This totally eliminated the chatter and produced a beautiful surface finish. This particular insert had enough side clearance for limited side-to-side turning. Even though I ground relief on the inside of the notch, my side-to-side d.o.c. was limited to about .005" due to the side flex of the 1/8" wide blade holder.
The last roughing, or semi-finishing, step on the main bearings was to clean up the faces of the webs on each side of the bearings. During the mill roughing operation I ran the cutter down the right side of the slot while it was cutting 100% of its width, but on the return pass it was engaged by only a fraction of its width. Tool deflection during the full width pass caused the cutter to remove excess material on the right side of each slot. Indexing left a pattern of deep machining marks. I included excess stock in the g-code to account for this, and so the purpose of this last roughing operation was to remove just enough material to clean up the web faces so their locations can be consistently measured. The widths of the bearings will be brought to their final dimensions later during finishing.
To face these walls I used a small boring bar mounted as a conventional radial turning tool. This set-up nicely handled the left web faces, but I had to invert the cutter and run the lathe in reverse in order to face the right-sides.
The final step on the main bearings will be to complete their finishing operations. In order to do this I plan to grind one of George's HSS bifurcated tools. I thought about just continuing with my notched insert, but a HSS blank will allow me to increase the effective blade width nearly 50% for improved rigidity and elimintate the holder for the blade. I also need .020" fillets on the corners of the tool, and these will be easier to grind on a HSS blank than on a carbide insert. In addition, I'll likely also construct the fixture needed to support the driven end of the workpiece against my lathe's faceplate so I'll have the option of finishing the main bearings between centers. - Terry

 

[Charles Lamont]

I strongly recommend against taking the mains to finished diameter before getting the pins rough milled and turned to the same stage as you now have the mains. You just don't know what built in stesses there may be in the bar, nor how these may cause distortion when you take metal away asymmetrically. I would suggest you rough the whole thing, everything, including webs, weights, and holes, leaving the bearings +10 to 15 thou on diameter, before going for finished dimensions on anything.

 

[mayhugh1]

Charles,
That's probably good advice that I think I'm going to follow. The only legitimate reason I had for finishing the mains first was that I was hoping to get to run the lathe at a higher rpm for their finishing operation before I unbalanced the heavy workpiece. But, as I've since learned, my cutters are limiting me to 120 rpm anyway.
My understanding of Stressproof is that it shouldn't create the warping issues that Zapjack ran into with his crankshaft using SAE 4140. George Britnell mentioned in his flat head build that he has seen no evidence of warping in his cranks since he started using 1144. In any event, I can see no downside to roughing most the feature before beginning any of the finishing operations, and so I'm revising my plan. I'll still have to leave the boring operations that hollow out the bearings until after finishing, though, because those operations remove all my machining references on both ends of the finished crankshaft. Thanks. - Terry

 

[mayhugh1]

I decided to take Charles' advice and hold off finishing the main bearings until after I complete more of the roughing. Since a lot of what I'm doing right now is in new territory for me it's also best I gain my experience during the more forgiving roughing phase. As a precaution and before doing additional cutting on the workpiece I measured and logged the current locations of the roughed-in main bearings to verify I actually had the excess web stock that I had planned.
For the crankpin roughing I used my mill's fourth axis to support and index the workpiece instead of manually repositioning it in the mill vise as I did for the main bearings. The deeper cuts needed for the crankpins would have required many error-prone repositioning and re-referencing steps in order to work around the vise. The downside of roughing between centers on the fourth axis, though, is a considerable loss of rigidity compared with using a mill vise. A 4-jaw chuck added to the fourth axis to support the front end of the workpiece would have blocked my spindle's access to a significant portion of it since I'm not using a toolholder for the cutter.
I machined a fixture for a close slip fit over the crankshaft's front spigot which was previously machined with three peripheral flats and the four axial center-drilled holes that define the four axes of the crankshaft's bearings. The crankshaft is secured in the fixture by cup setscrews bearing against the three flats, and the whole assembly is bolted to the fourth axis face plate. I machined the mounting slots in the fixture so it can also be used with my lathe's faceplate while turning between centers on any of the crankshaft's four axes.
In use, after positioning the desired axis of the crankshaft between centers, the setscrews are tightened against the flats, while the assembly is rotated to align the fixture's mounting slots with those on the machine's faceplate. Once this is initially done for one offset axis, the setscrews may be loosened and, with the tailstock withdrawn, the workpiece can be simply pulled out of the fixture and rotated to an alternate offset axis without touching the fixture's mounting bolts. The axial alignment is controlled entirely by the machines' centers. This fixture allows me to move the crankshaft between either of my lathes or mills' fourth axes without worrying about losing axial alignment. The fixture merely adds the rigid support needed at the front of the workpiece. The rear of the crankshaft is supported by the centers in the machines' tailstocks. The fourth axis can be zero referenced by indicating the appropriate flat on the tailstock end of the crankshaft.
In order to handle the heavy crankpin roughing I felt additional support was needed at the center of the workpiece. Since I planned to rough the crankpins with the fourth axis aligned with the axis of the main bearings, my vision was to anchor to the mill table a bearing block having a close slip fit to the center main bearing. This would allow the fourth axis to freely rotate, but it would limit any flex or vibration at the center of the workpiece. After a few machining attempts I realized I probably wasn't going to easily get the fit I wanted to my roughed-in bearing. I settled, instead, for a tight fitting block that provided the support I wanted, but one that would have to be loosened to allow rotation of the workpiece. As a result I divided my roughing program into six smaller programs that required me to manually index the fourth axis before running each one. Actually, I've learned from experience that my equipment and its operator are usually much happier if long untested grueling programs are broken into a number of smaller programs. A lot of things can go wrong, and when they do it can be difficult to recover a valuable workpiece.
I had to increase the stick-out of my 3/8" cutter by an additional .2" for a total of 1.9" in order to clear the fixture while machining the front of the workpiece. This left only about 1/2" of the cutter's shank inside the R-8 collet during the 18 ipm, .150" d.o.c. roughing operation. I monitored the slip, but it amounted to only .004" over the entire two hour machining time.
Since I really didn't like interrupted lathe cutting operation that previously turned the hexagonal mains into circular bearings I decided to clean up the crankpins in the mill while the crankshaft was in the fourth axis setup. Since typical mill cutters do not have flat bottoms due to the relief ground into them, the roughed-in crankpins did not end up with perfectly uniform diameters across their widths. I couldn't use my center support for this operation, and the chatter while machining the two central crankpins was severe enough that it affected the surface finish.
I moved the crankshaft and its fixture over to my lathe to verify my work-holding scheme actually worked there and also to clean up the crankpins. Even though their roughed-in states were just fine as they were, I'm going to be looking at them for quite some time; and their surface finishes bothered me. I also faced the webs to remove the spoke-patterned grooves left by my mill's roughing operation. These grooves were significantly more shallow than those left on the main bearings. I suspect part of the problem with the main bearings' webs was created by an inconsistent manual repositioning on my part. These re-facings allowed me to make and log consistent measurements to determine the actual locations of the crankpin bearings and the excess stock that will eventually be removed.
For these operations I initially ran the lathe at 100 rpm, and all the carbide cutting ran fine with no chatter and excellent surface finishes. I eventually speeded the operation up to 300 rpm, and this was the point where chatter just began to set in. However, it wasn't severe enough to affect the surface finish. The oscillating assembly, though, while running at 100 rpm was just too hypnotic; and my focus seemed to be continually and dangerously drawn into it.
I added a counterweight to the faceplate to balance the rotating assembly at 300 rpm. I also changed my tailstock's dead center to a live center when it dawned on me how much time this workpiece is going to be spending in the lathe.
My next step will probably be the roughing-in of the web counterweights. I'm currently planning to use my CAM software to try to coax my Tormach into doing most of the work for me on its fourth axis. - Terry

 

[petertha]

That's quite the setup. Looking good!

- on the end-milling operation, have you noticed any advantage or disadvantage to types of end mills? By that I mean those notched, toothy roughing end mills vs. more conventional spirals. Only reason I mention is I tried one for the first time the other day & was pleasantly surprised. Aside from nice short curly shavings, seemed like less load when ploughing through material & interrupted cuts.

- I've seen CS build pics where some guys epoxy in supporting wedge blocks progressively between the webs when the centers are in off-center positions - I assume to prevent 'accordion distortion'. But maybe that's more related to lathe-mode cutting vs your milling + support post. Have you found a need for anything like this so far? (I'm not really sure how one would measure its actually bowing anyway unless it was returned to neutral axis).

 

[mayhugh1]

Peter,
I've tried those HSS corncob roughing cutters in aluminum, and they do work really well. I have no experience with them in steel, though, and since the ones I have are relatively low end I wasn't confident enough in them to try them in this new (to me) steel. The cutter I used for these roughing operations was a 4 flute variable helix cutter that I purchased with no other information on it at a show two years ago. It has a dark purple coating on it that still shows no sign of wear. I used tbis same cutter on 304 stainless during my 18 cylinder radial build. I wish I knew more about it but it has no markings on it.
I've seen those wedges also, and my own questions about them was one of the reasons for the center support that I used for the heavy cutting. The only roughing that is left is on the webs, and I hope to use some kind of support while milling them also - maybe even the wedges. Since I now have nice clean turned faces on all of the webs I should be able to tell by indicating them if the crankshaft does warp either from relieved internal stresses or from the forces of heavy cutting. Finishing all the heavy cutting before starting the finishing, as Charles pointed out, might let me recover from any induced distortion. - Terry

 

[mayhugh1]

We got to spend the past week with our grandkids, and so my shop time was limited to only a handful of late night hours. The break did give me an opportunity, though, to re-think my order of the crankshaft machining operations. I've not been looking forward to the through-drilling and associated counterboring specified for the Merlin's main and crankpin bearings. My next step was going to be to rough machine the webs. The original plan was to delay the through-drilling until after all the finish machining was completed since this drilling will remove the four center-drilled holes on each end of the workpiece. These center-drilled holes are required for all the remaining machining operations, and they will have to be replaced with machined buttons if the drilling is moved forward in the process.
Early on, it was obvious that the crankshaft would be very difficult to fixture for drilling on the mill after the webs were machined. Therefore, I had been planning to do it on my lathe using a custom made steady rest. After thinking about the design of this steady rest, though, I realized that it was going be a very significant project all by itself. I also began thinking about the forces generated by the offset drilling and how they might bend a completely finished crankshaft. There was also Charles' warning to leave ALL the finishing to the very end.
So, I decided to through-drill the bearings on the mill and to do it now before the web machining. With the workpiece vertically supported under my mill's spindle, the headspace was barely enough for the long drill I needed to use. Since there was no room for a drill chuck, I modified the diameters of the though-holes specified on the Merlin drawings so I could use an R8 compatible drill size. The drawings actually specify a slightly smaller hole size for the crankpin bearings than for the main bearings. Since I'll later have to make a special inserted counterboring tool to machine the counterbores, I elected to make both holes the same diameter. I selected the R-8 compatible drill size to be very close to the hole specified for the crankpins so I wouldn't significantly affect the crankshaft balance. I also had to shorten the shank of a very expensive long parabolic drill that was specially purchased for this operation.
The hole centers were accurately located using a spindle microscope, and the holes were reamed after being drilled so I could get an accurate fit to the buttons. The finished diameter was selected so I could use a piece of standard size drill rod later when I make the piloted counterboring tool. The buttons, themselves, were machined from steel although a softer metal could probably have been used since, with the live tailstock center, there's little relative motion between the machines' centers and the workpiece. I made several spare buttons with various degrees of light interfering fits so I could maintain a close fit in case the reamed holes open up later during use. (Actually, these 'spares' were my failed attempts to machine a pair with just the right fit.) The hope was that even if the new button centers did not precisely correspond to the original centers, the remaining machining would correct the crankshaft's axes to them.
There are some important recesses that must eventually be bored on each end of the crankshaft. These recesses locate power take off shafts at each end of the engine, and they must be concentric to the main bearings. I considered also boring these while I had the workpiece fixture'd on the mill, but adding them at that time would have complicated the button design. A reasonably simple steady rest will be needed to bore these on the lathe after the remainder of the machining is completed.
After all the drilling was completed, I installed my best fitting pair of center-drilled buttons into the ends of the workpiece on the main bearing axis. I installed the workpiece on my Tormach's fourth axis to prepare for the web roughing operation and also so I could check the resulting runout of the main bearings. I was pleasantly surprised (shocked, actually) to find it measured less than .001"
The next step will finally be the rough machining of the webs. - Terry

 

[gbritnell]

Hi Terry,
In my experiences of using 1144 steel I have been very satisfied with the accuracy when machining. When roughing the main journals and throws I took some fairly aggressive cuts with a 4 flute end mill and like you ended up with minimal distortion.
The only crank I ever ground was the one in my 302 engine. At that time I had a 9 inch South Bend lathe and made a tool post grinder for it. The biggest problem I had was finding a grinding wheel narrow enough to traverse the journals to get about .020 overlap at the center. I purchased a wheel .250 wide and then while spinning it I used a single point diamond dresser to thin the wheel to about .180.
This was back in the days when I was just starting out making multi-cylinder I.C. engines and the only steel I knew of was 1018 or tool steels and really didn't want to tackle anything like 4130 or 4140. I had machine some 8620 for a fellow who wanted to make a full sized camshaft for a diesel engine fuel pump but I only had to rough turn it. It was then case hardened and ground.
Some fellows use 12L14 steel and while I do make miscellaneous parts from it I haven't made a crankshaft.
Your vertical drilling/reaming setup looks a lot like what I do. When working in the pattern shop we had some large, very accurate V-blocks and they worked great for doing vertical machining operations on both rectangular and round stock. I have always wanted to buy one but the cost for something like an accurate 8 or 10 inch V-block was more than I wanted to spend.
I'm following along to see the further operations.
Even though this is your first foray with this type of crank and seeing your other work I have no doubt that it will be a thing of beauty.
gbritnell

 

[mayhugh1]

George,
Thanks for the comments. The 'long' vee-block in the photo is actually two short ones separated by a 2-3-4 block. The clamp on the top of the stack is holding the sandwich together and keeping it from tilting when when it is drawn up toward the vertical reference plate. I also have a ground bar between the vertical plate and the reference flat on the bottom end of the workpiece for good measure.
Might I ask what is the minimum d.o.c. you are able to take off with your HSS bifurcated tool? I'm still trying to make a carbide grooving insert work, but I don't seem to have control over the d.o.c. to better than .002-.003" (diameter). - Terry

 

[gbritnell]

Hi Terry,
As I recall I didn't take much more than .02 per cut (dia). The biggest reason being that as the the bifurcated tool was moved into the material once it got to the depth of the groove it would start to chatter so I didn't press it. The one thing I did do was to move the tool left and right as I was plunging in. This allowed me to take a slightly deeper cut.

 

[mayhugh1]

My next step in the crankshaft construction was to rough machine the webs. The webs on this crankshaft are pretty complex, and a lot of metal has to be removed from the workpiece in order to form them. Since I had good success with the crankpin roughing on my four axis Tormach, I decided to rough machine the webs similarly. I chose to manually index the crankshaft around the axis of the main bearings so I could again use my shop-made center bearing support since I was expecting chatter from the deep passes on the relatively thin webs. I also limited the maximum cutting depth at each indexed position to half the diameter of the workpiece so I could use a minimum stick-out for the cutter. I configured my CAM software to create g-code that would allow me to manually index the workpiece in 90 degree steps for two complete revolutions. I removed most of the excess stock during the four 90 degree increments of the first revolution using a d.o.c. of .15" and a feedrate of 18 ipm. This coarse waterline operation left .15" tall steps on the machined surfaces in addition to a .015" base layer of excess safety stock. This coarse stepped surface would have been OK if I had known for sure that I will be able to later run a continuous four axis finishing pass. Right now, though, that's not 100% certain. Continuous four axis machining was the holy grail for my particular CAM package (Sprutcam) during its past several years development. This feature, with a number of restrictions, was first made available in the version of the software that I upgraded to some four years ago. But, with only the modest effort I've put into it so far, I've never been able to actually machine a real part using this new operation. To make things a little more interesting there also seems to be issues with inverse time feed-rate in my particular version of Mach3. This G93 mode is used by my CAM's postprocessor for this particular operation, and it tells Mach3 the time to be used for each incremental blended move rather than specifying an actual feedrate. (This is done because mixed units of inches and degrees are being blended.)
Because of these uncertainties, another roughing pass was run during the second revolution, but this time with a d.o.c. of .015". This second pass reduced the size of the surface steps just in case I have to manually finish the webs' radial surfaces.
Since I already had a lot of time accumulated in this workpiece I did something that I rarely intentionally do. I created a short dummy workpiece from a piece of scrap steel so I could test a portion of my web roughing code on a single pair of webs. The test ran pretty much as expected except the feeds and speeds I had been using for Stressproof seemed much too high for the cold rolled I was using for the test. I had to drop the 3/8" cutter speed from 2500 rpm to 2100 rpm and the feed rate from 18 ipm to 10 ipm in order to bring the chip color back down from deep purple to light straw. This really surprised me because I was expecting the machinability of my cold rolled blank to be somewhat better than that of 1144. But, since I don't know where it actually came from, it's possible that my test blank is just a chunk of garbage steel. I found the uniquely rolled shapes of the Stressproof chips interesting enough to include a close-up photo. Maybe I've not worked very much with quality steels, but I'm learning to really like this material.
The three hour web roughing operation nearly doubled the amount of metal removed from the workpiece so far, and it is finally starting to look like a crankshaft. Except for the end spigots, the rough machining is now completed.
My next step will be to put some more effort into working with my CAM software to generate the toolpaths needed to finish machine the radial surfaces of the webs. If I can generate the tool paths I'll have my test part with its pair of roughed webs to use for testing. If I'm not successful, then I'll likely run some additional finer roughing passes in order to further reduce the amount of manual finishing. - Terry

 

[Scott_M]

Hi Terry
Looking good !
If you can find an long end mill like you are using with a corner radius of about .015" your waterline steps will blend really nice. A finish step of about .005" to .007" with a .015" corner radius would be really smooth and require little blending.

Just a thought, but I bet you already knew that

Scott

 

[mayhugh1]

Scott,
Thanks for the suggestion, and no that didn't occur to me. If I can't get Sprutcam 7's rotary machining operation working for me on this I'll run another roughing pass just as you suggest. - Terry

 

[mayhugh1]

My ancient version of Sprutcam (7) software contains the first version of what the vendor called a 'Rotary Machining' operation. There are some restrictions, but this particular operation was designed to produce g-code with blended moves of three linear and one rotary axis to produce a continuous tool path for machining camshafts and crankshafts. I have respect for any software that can generate 3-D tool paths, but when a rotary axis is included I'm truly humbled. I've been playing with this particular operation on and off for the past several weeks and hoping I could apply it to the complex web peripheries of my Merlin's crankshaft. Most of my problems with this particular operation have been related to the fact that being a first release, it wasn't hardened against a newbie's attempts to use it. The manual for this software has never been one of its strong points, and so I typically learn new features by trial and error. Once I learned where the dark corners were, I stayed out of them, and eventually I was able to get some useable simulation results.
Even though this operation is categorized as a finishing operation, and unlike the other finishing operations in this package, a workpiece can be included in the simulation. In fact, I was able to import the simulation results of my roughing operation into this finishing program for use as a starting workpiece.
The software is capable of working with a variety of end mill types, but this particular operation seems to prefer a ball mill. Because the webs have relatively wide flat surfaces, I spent a lot of time trying to make a 3/8" cylindrical end mill with .060" radius'd corners work. The radius'd corners were helpful in reducing the machining marks left on my test part during some of the complex reverse rotary moves.
Unfortunately, and this may be a common issue with other four-axis packages, a truly flat bottom is assumed for a cylindrical cutter even though nearly all endmills have bottom relief ground into them. I tried using a flat bottom counterbore on a test part, but the chatter was excessive and the surface finish was poor probably because this tool wasn't designed for side cutting. I've read that Sandvik makes a special cutter for this application, but I was unable to locate it. It sure would be useful when I start working on the camshafts.
The cutter relief in a stepped-over rotary operation will create a series of ridges around the machined part instead of a nice flat surface. The simulator isn't much help in tuning out these imperfections since it doesn't understand the cutter relief.
The software allows two choices for orienting the cutter: 1) normal to the cutting surface or (2) through the axis of rotation. My best cylindrical cutter results with acceptable machining times were obtained using a normal orientation and a spiraling .025" step-over. These parameters were finally determined by cutting actual profiles on a test part. The ridges left behind were high enough, though, that they would have to be manually ground or filed away.
I eventually migrated to a 1/2" ball cutter normally oriented to the part's surface with a lead angle of 10 degrees. This lead angle moved the zero SFM center point of the ball cutter off the tool path for a better surface finish. I was initially surprised to discover the ball cutter produced a nicer finish than the radius'd cylindrical cutter for the same step-over. The simulator also properly handled the material removed from the workpiece with the ball cutter. According to my calculations the theoretical scallop size was only .0002", and the machining marks easily polished out with a Scotchbrite pad.
I originally intended to machine the webs in pairs instead of trying to do all of them in a single operation. I ended up, though, machining them one at a time because of the way in which the software handles the rotary roll-over. Each rotary machining operation starts out assuming the rotary is positioned at the part's zero reference position. When the first operation is completed, the rotary has to unwind its accumulated revolutions and return to zero before the second operation can begin. I found it quicker to re-indicate the rotary's starting position myself rather than wait for it to return to its starting point. This also gave me an opportunity to vary some of the operation's parameters so I could learn more about fine tuning it.
The three hour rotary machining went extremely well considering it was my first serious attempt at using it, but I've learned to leave a maximum stock of only .010" or so in the future for it to finish. The operation makes some quick and unexpected moves off its spiral trajectory whenever it sees certain types of nearby cutting opportunities. It will try to clean out deep lateral ditches in a single pass using the feed/speed parameters that were originally selected for a more modest .025" step-over, and the result can be unnerving.
I manually polished out the web machining marks, and then I returned the crankshaft to the lathe where I measured the run-outs of the bearings to get an idea of any mis-alignments created by my new button axes. The run-outs of the main bearings were less than .002" while the run-outs of the bearings on the three crankpin axes ranged from .003" to .004". I was happy with these results given the trauma I had put the workpiece through when I replaced all my original center-drilled end references. I next turned all the bearings to semi-finished dimensions since I was still experimenting with bifurcated turning tools.
Before starting to grind a version of George's HSS tool for turning the bearings, I thought I would give carbide inserts one last try. The insert I previously used with some success was a low-rake no-name import intended for heavy cutting in a big lathe. Since I had just received a 40% off coupon from MSC I went through their catalog looking for an insert designed for 'light finishing' since it would likely have more rake and have less tendency to chatter in my lathe. Because of the long stick-out required to turn the crankpin bearings, I also needed a wide blade holder to minimize flex during side-to-side cutting.

I found a .199" wide Kennametal KC5025 A2 insert (MSC #80757750) and a matching A2 blade (MSC #03266133) that seemed like my best option. I also had to purchase a blade holder (MSC #51018497) for the blade. The blade holder and one of my Aloris-type tool-holders had to be heavily modified to get the insert at the correct height for my lathe. I cut a raked Britnell notch into the insert with a Dremel diamond cut-off wheel. The stock insert came with .010" radius corners which was half what I really wanted, but I decided to live with them rather than try to modify the insert any further. For the bifurcated cutter to work properly, its cutting edge must be perfectly parallel to the lathe's axis. I tried using the broadside of the blade as an indicating surface but found it wasn't sufficiently accurate because of a very slight tilt in the toolholder. Instead, I used George's method of indicating the tips of the insert itself.
I was thrilled with the results. This combination cut with no chatter, and the surface finish appeared polished. This insert cut smoother with hand-applied moly-based cutting oil rather than the synthetic coolant I normally spray from my Micro-drop dispenser. The only issue is with the minimum depth of cut that I can take. I can easily take .010" (dia.) cuts, but the minimum depth of cut is somewhere around .001"-.002" which is limited by the insert's rake. As a result, when I finally finish the bearings I will likely have to polish more material that I had hoped in order to get them all to identical diameters.

The next step is to bring the web thicknesses to their final dimensions so the bearing counterbores can be completed. These two operations must be completed before turning the chamfers on the counterweights. - Terry[ame]https://www.youtube.com/watch?v=8vc_jYkt2eg[/ame]

 

[gbritnell]

Terry,
That's a thing of beauty!
gbritnell