Another Radial - this time 18 Cylinders

[DICKEYBIRD]

What a monumental & amazing project you're sharing with us Terry; thanks!;D

I'm very curious about your CNC lathe work as I have a similar sized machine that is now Mach3 controlled (Denford ORAC) I've been pidding with threading lately and was curious if you're using the Simple Threading Wizard that comes with the program or something else. Your threads look great!

Also, what's your spindle motor & speed control setup? Is there a thread somewhere showing your conversion?

 

[mayhugh1]

Hi,
My 9x20 lathe is a Wabeco lathe that was converted and sold by MDA Precision located in Ca. I purchased it some 6 or 7 years ago. The conversion was nicely thought out and well done but the lathe is really pricey. It uses a control board from Texas MicroCircuits located in Dallas. The motor is a Varicon 1.5 kW unit with VFD drive. I replaced the cross-slide on the carriage with a large chunk of aluminum to improve the rigidity, and this made a world of difference. This lathe shares the same weak cross-slide/carriage set-up that the rest of the 9x20 imports have. I also replaced the round style stepper motors that came with the lathe from MDA with standard NEMA motors. Their round style steppers generated way too little torque and the NEMA's greatly improved the lathe's repeatibility. I also replaced the control board with a newer version from TMC that had a built-in spindle control.
I always use the simple threading wizard in Mach even though my CAM supports threading. It's quick and easy to work with. Threading in Mach has always been a problem that wasn't fixed until Art from ArtSoft sold Mach to another party for support a few years ago. I guess he got bored and came back to Mach temporarily to figure it out. He worked with a user named Rich who ran some careful tests while Art made software changes. Remarkably, Art didn't have the hardware to test his own code. They finally figured it out on one of the open forums, and it works pretty flawlessly now and the threads look great. You have to get the latest version of Mach to be certain you have the improved threading code. I was followed their work while they were doing it and picked up an interim patch that Art made that included all his threading fixes. I applied the patch to my then current version but I've never updated to the most recent version of a Mach myself. For threading I use a partial profile insert but it still takes a few trial and error passes to come up with the right threading depth for a nice fitting thread. I've learned to let the threading tool itself turn the last .005" of the starting OD on an external thread or the starting ID of an internal thread before starting the actual threading. -Terry

 

[DICKEYBIRD]

Thanks for the info Terry! All CNC lathe stuff excites me and I'm trying to learn as much as I can. I built a CNC router 16 yrs ago to cut out r/c model airplane parts (before I got this metal disease.) I got pretty productive with it but this CNC lathe stuff is much harder even though it has fewer axes. I have Dolphin Partmaster CAM for the lathe but it's been a struggle so far.

For threading I use a partial profile insert but it still takes a few trial and error passes to come up with the right threading depth for a nice fitting thread. I've learned to let the threading tool itself turn the last .005" of the starting OD on an external thread or the starting ID of an internal thread before starting the actual threading. -Terry

So you're making the finish cut of the blank with the threading tool instead of a regular turning insert so that you're more likely to hit the intended thread depth? Good idea, thanks!

I just finished an ER40 collet chuck which had M50x1.5 threads....a tall order for my 3/4 hp DC spindle motor. I had recently added a 4:1 reduction pulley system so it has enough torque & speed stability but the thread came out a few thou too large. I attempted to rerun it with a little deeper cut but somehow fumble fingered & crashed the tool. I tried to pick up the thread but that proved impossible at my level of experience. Fortunately I was able to throw it on a manual lathe & finish it off successfully at 17 TPI; close enough!

ps: I'm using Mach v.057 which seems to be OK. If you decide to update yours, stay away from the latest one (.066) as it has known problems in Turn which probably won't ever be fixed since they're working on Mach4 now.

 

[mayhugh1]

I started over with my SolidWorks modeling of the heads but this time with the machining sequence in mind. I started with a 'generic' head that contains features common to both the front and rear row heads, and from this I created the actual two head models. I think the design is pretty much finished except for some decisions about filleting the edges of the fins between the valve towers and in the spark plug area. I'll probably need to see some actual parts before I finally decide. The model tells me filleting looks better, but I know there'll be issues with me convincing my CAM to properly blend the skewed intersections. I left the models in the photos un-filleted for now. I ground and hardened two filleting cutters, a 1/32" corner rounding cutter and a concave radius cutter with a 1/32" full radius profile, for some some experiments though.
The majority of the fin profiling will be done on the lathe using grooving code and a full radius grooving tool similar to what I did on the cylinders. The fin area between the valve towers that's un-reachable by lathe tooling will be done on the mill, and a Woodruff cutter will be used for the undercutting. Undercutting will be another new CNC experience for me, and it's only 'somewhat' supported by my CAM.
I decided to start a pair of heads to begin documenting a build process and to create test beds for some of the tricky CAM coming up. I don't expect either of these to end up as final parts. I started by sawing two pieces of 2-1/2" dia 6061 just under 2" long. To prepare them as head blanks, I reduced their diameters (turns out, by too much) and faced the ends on my manual lathe. I also roughed the combustion chambers by pre-drilling one end with a shallow recess using a 15/16" drill.
The blanks were chucked in my CNC lathe, and the finished conical combustion chambers were turned. The ID's were then threaded to match my cylinders. I went through each of my completed cylinders and searched for the one with the closest fit to use as a gage.
At this point I turned a threaded mandrel so the heads can be supported by their combustion chambers for the remainder of their lathe work. The next step was to determine the machining parameters for the grooving operation. I decided to run some single groove test programs on scrap rather than my head blanks to avoid ruining them early on. I was hoping these experiments would go a lot smoother than the ones on the steel cylinders.
Because of the OD profile of my head design, a left-hand grooving tool holder and left hand inserts are required. I had to order these, and after a few hours of frustrating results I discovered my new Nicole tool holder had been mis-machined and was not supporting the insert truly vertical. After re-machining the holder, I was able to find a sweet spot of 2 ipm and 1400 rpm that seemed to work on my little lathe. With the 12L14 I used for my cylinders, I ended up with 1 ipm and 1000 rpm; and so the aluminum chip load was, disappointingly, only about 50% better. However, the deep full-width grooving passes still sounded very rough, and the stringers coming off the workpiece were ragged even though the part's surface finish was great. Interestingly, increasing the federate made things even worse. I switched to 7075 aluminum; and the grooving not only sounded better, but the stringers coming off the workpiece were nicely uniform and peeled away from the workpiece a lot more smoothly. The full radius C6 inserts I'm using have a rather low rake since they are designed for steel, and they don't seem entirely happy with the soft 6061. The 7075 is somewhat harder and maybe a little better match for them. So, I decided to switch the head material to 7075. I also ordered a few C2 inserts. Their rake is probably the same, but I'm hoping their built-up edge resistance will be better than I'm experiencing with the mist lubricated C6 inserts. The grooving time looks like it will be just over 20 minutes per head.
I was able to use one of the partially finished heads to verify the narrow clearance between the bottom-most front row cylinder and the front-end of the oil sump which is already irreversibly mounted on the crankcase.
The next step will be to be to create the milling fixture(s) and figure out a strategy for removing workpiece material from the valley between the valve towers as well as the area above the intake/exhaust flange recess. -Terry

 

[mayhugh1]

The simple threaded mandrel that I made to hold the heads for their turning operations worked OK on the lathe since the cutters created only tightening forces. The heads do end up pretty snug on the mandrel, though, and have to be carefully 'wrenched' off. The milling operations, though, create both tightening and loosening forces; and so I made a second, threaded and expandable, mandrel for use on the mill.
I created a few single and double groove test disks in order to try my hand at generating code to eventually undercut and fully radius the fins between the valve towers. I was pleasantly surprised to find that my CAM performed well on these new (to me) operations. After coming up with the machining parameters for my fin cutting tools, it was time to generate the tool paths to continue the machining on my two test heads.
I then started a week long trip to Hell. It all began during my CAM simulations when I began getting tool collision warnings created by my fin radiusing tool. These warnings surprised me because in my CAM these particular operations work only with curves and aren't supposed to consider the part or workpiece at all. But, they were legitimate, and I eventually realized they were happening because I hadn't fully taken my tooling into account in my head design. The troublesome areas were where the profiled fins in the tower valley and intake/exhaust flange areas blended into the existing fins in the lathe-turned blank.
About this time I suddenly came down with some really bad flu-like symptoms. Instead of resting, I decided to make a new cutter to see if I could avoid redesigning the head, So, I started with a carbide reamer, a diamond hone, and a handful of Harbor Freight diamond Dremel points. The carbide decision was irrational and totally flu-related. Anyway, two full days of work later I had a working tool with perfect contours and proper cutting edge clearances, but it still wouldn't pass my simulations. I had also made a .031" corner rounding cutter out of carbide reamer.
At this point, and in no physical or mental shape to make such a decision, I suddenly didn't like my head design anymore. So, instead of fixing the tool interference problems with the current design, I started over - again. This time, knowing my CAM was capable of what I needed, I became obsessed with the minutia of perfectly blending the fillets, radii, and undercuts together at all the complicated intersections I was creating in the new design. Getting the necessary tooling clearances simultaneously with the esthetics I was looking for turned out to be much more complicated that I had ever imagined. I spent dozens and dozens of hours on such incredibly small details that probably only I would notice.
All the CAD file saves I was doing caused me to bump into a SolidWorks bug. My file sizes had begun growing exponentially even though the many design changes I was continually making to the design were minor. This turned out to be known bug with the old (2007) version I'm using. My one meg design file had blown up to some 200 meg and 199 meg of it was SolidWorks bloat that slowed my computer to a crawl. Just when I was almost finished with the design, I had no choice but to delete all my cumulative design work and start over. I had never run into this problem before, but then I had never made so many changes to the same file either. Several days later, I had a design ready to submit to my CAM. The CAM work went smoothly, but after my flu symptoms began subsiding, the jpgs of my original design started looking better to me than my latest design. Unfortunately while in a mental stupor earlier, I lost all my early design versions in a major delete accident.
After getting a successful simulation, I set one of my two blanks up on the mill, started the program, and held my breath. To my amazement, the part came out exactly as I had visualized it. I found three minor tool gouges at the rear of the part that my CAM, as expected, had failed to flag. I was really lucky I didn't break either of my one-of-a-kind cutters. I tweaked the design slightly to improve the tool clearances before regenerating the tool paths to start the second blank. The second part ran cleanly and looked as good as I had hoped. After seeing the two parts in actual metal, I'm very happy with the result.
There are four more operations needed to complete the head, but these are simple compared with what I've already done. Figuring out the work holding for them will be the most difficult part as all four operations are at unique angles to the axis of the head and new coordinate systems and fixtures need to be created for each one of them.
I also plan to re-work the rocker arm support design as what I've shown earlier has only been a placeholder. That should be an opportunity for me to jump down another rabbit hole. -Terry

 

[Scott_M]

Hi Terry
Absolutely beautiful !
I came down with the flu last week too. I had trouble working the remote for the TV....I have no idea how you pulled that off.
The cutters look great and the end result in metal is a sight to behold.
Nicely done.

Scott

 

[gbritnell]

CNC or not those are some gorgeous looking pieces. When I worked as a CAD modeler and cutter path generator I had a computer system that had almost unlimited storage so huge files weren't a problem. How did you reduce the size of you Solidworks files to an acceptable size? I have modeled a lot of my engine parts in ver. 2005 and some are quite complex but the files sizes don't seem to be that big.
Oh and by the way I also have to compliment you on the tool making, once again first rate.
gbritnell

 

[mayhugh1]

Thanks all for the compliments.
George, I don't have a way to reduce the file size. The current file size is just over 60 meg and I'm probably two saves away from it becoming too unwieldy to work with anymore. So, I don't plan to make any more nice-to-have changes to it. I'm saving my last 'save' for my new rocker box design if one is needed. My understanding of the problem is, that for some reason, SolidWorks is storing multiple display modes of the same model in the file to cause all the bloat. This was discovered by users in ver 2007. SW never found the root cause of the problem until 2010, but they released a utility in an update to delete these excess display modes late in 2007. My version doesn't have the utility; and I don't have the $3k-$5k needed to get a new version, and so I'll just have to deal with it. This is the only project out of hundreds I've done where this has become a major limitation. There is something about this design or the way I keep creating it that has SolidWorks confused. Terry

 

[Rivergypsy]

Beautiful work as usual Terry - well done!

 

[robcas631]

Amazing work!

 

[happykingkong]

HELLO Is the best job I've ever seen

Looking forward to can see him run

你好 这是我见到最好的作业！ 期待它可以运行起来！

 

[mayhugh1]

I appreciate the interest that my little project has generated. I've been getting a number of personal emails from readers asking to purchase or somehow obtain the drawings for the engine I'm building. As I mentioned at the beginning of this thread, I'm working from a set of online photos published by Chaos Industries which is a great looking engine they designed around, I think, Hodgson's twin 18 cylinder plan set. I have no dimensions to work from; and so I've been designing my own parts, as I go, in SolidWorks 2007. Not being an experienced engine builder or even machinist, for that matter, I've been using the Hodgson nine cylinder plan set that I own to fill in some of the missing DNA for this engine. I've incorporated the cam ring design as well as several basic and internal crankcase dimensions from the H-9 engine into my own twin-18 design. But, pretty much every part has started from a clean sheet of paper (or should I say new CAD sketch). That being said, I don't feel comfortable with distributing the entire set of CAD files or drawings because they will contain content owned by the Hodgson family. I have absolutely no interest in making any money associated with this engine, and if it weren't for the Hodgson IP content I would be thrilled to give it all away. However, I feel the cylinders and heads are a different story. I think my design, when finished, may make a significant cosmetic improvement over the H-9 counterparts. And, with all the work I'm putting into them it would be a shame to have only the only set in existence. I've been designing them to be drop-in replacements for the H-9 heads, but there is no way for me to tell if they will drop into the Hodgson twin-18 engine. I don't know yet how I would make them freely available since the file sizes would preclude emailing them, and so I'm open to suggestions. I would prefer to minimize any additional work on my part and just give away the SolidWorks files I created. I could probably call upon a friend with a recent version of SolidWorks to 'scrub' them to remove the accumulated bloat and save them out to a more recent version that I'll no longer be able to read, but I'm sure the file sizes would still be too large for email. -Terry

 

[stevehuckss396]

I don't feel comfortable with distributing the entire set of CAD files or drawings because they will contain content owned by the Hodgson family. However, I feel the cylinders and heads are a different story. I think my design, when finished, may make a significant cosmetic improvement over the H-9 counterparts. And, with all the work I'm putting into them it would be a shame to have only the only set in existence. I've been designing them to be drop-in replacements for the H-9 heads

Maybe you could make your head design available to whoever wants them. If they purchase the plans from Lee and opt to use your head design there should be no problem with infringment of any kind. You would simply be making available an add on.

 

[mayhugh1]

Yeah,
I guess that's what I was trying to say. Thanks. -Terry

 

[mayhugh1]

The first off-axis milling operation is the pocket for the intake/exhaust flange. This one is simple since the spindle axis is perpendicular to the axis of the head, and so the part is just supported by its mandrel in a horizontal rotary. I machined a tee-square tool for a close fit between the linear edges of the fins in the valve tower valley for use in vertically aligning the part. The machining of the pocket and the reamed holes for the intake/exhaust ports went smoothly in both test parts and produced a nice surface finish.
The machining of the spark plug port and the valve guide bores, however, is a totally different animal. The axes of these operations are at 25 degrees to the axis of the head, and they each intersect the axis of the head at different points.
An engineered fixture is needed to accurately and consistently perform these operations. The operations for the spark plug port are probably the most critical. If the spark plug port doesn't end up accurately between the already finished fins the appearance will be spoiled.
After designing a complicated fixture that I wasn't even sure I could machine, I realized I already had two components of the fixture that I need: 1) the Hodgson fixture that I used to machine my H-9 heads and 2) a completed spare H-9 head. I designed my twin-18 heads with the same basic geometry of the H-9 heads so they can replace the heads in an H-9 engine. The valve towers and the spark plug ports of both engines are on identical axes. My twin-18 heads don't have the straight-wall o.d. of the H-9 heads, however, and so they can't be directly held in the H-9 fixture. So, I reduced the o.d. of my threaded expandable mandrel, which does have straight walls, to match the i.d. of the fixture. Then I bored out the fixture's center so it could accept the mandrel. The plan is to insert an H-9 head into the fixture and then align it to the fixture for either the plug or tower machining operation using the head's exhaust flat exactly as I did when I originally machined the H-9 head. The mill spindle is then positioned over the center of the already machined H-9 feature. The H-9 head is then removed and replaced with the twin-18 head on its mandrel. The twin-18 head is rotated and locked into place in the fixture after being properly aligned to it using the linear edges of the valley fins. Some simple trigonometry corrects the z and x axes for the displacements created by the mandrel. After going through this calibration procedure with the H -9 head one time, the twin-18 heads can then be fed one after another into the fixture and the spark plug operations finished. In order to get the best possible seal, all the spark plug operations are done in the same setup including manually threading the port with a spring-loaded tap starter under the spindle. Using this procedure the spark plug ports appear to have come out perfectly centered in both test heads.
One of the goals of my head design is to shroud a large portion of the upper body of the CM-6 spark plug so it does not appear so far out of scale in this engine as it does in the H-9. The photos show side-by-side comparisons with the H-9 heads.
The last head operations are the machining of the valve tower tops for the rocker arm supports and the bores for the valve guides. I should be able to use a fixturing scheme similar to what I came up with for the spark plug operations. I don't have this portion of the design finalized yet, and so that will be my next CAD project. Our Texas winter is starting to subside, and I want to get the head production underway before the shop heat returns. I think I may start to bring a batch of 25 heads up to the current stage of completion while I finalize the design of the rockers. I've already sawed 25 pieces of 2-1/2" dia. 7075 to begin making the blanks. -Terry

 

[Walltoddj]

Maybe you could make your head design available to whoever wants them. If they purchase the plans from Lee and opt to use your head design there should be no problem with infringment of any kind. You would simply be making available an add on.

You could talk to Lee about it since I got my plans many years ago they have had a couple of revisions. Yours is a major revision that looks great one problem with Lee as with most engineer type they just see the plans, I tried to see if the plans had been revised again when Bill was doing his build and Lee had no idea which revision I was talking about due to lack of revision numbers just a date. This to me is not a good way to keep track of print changes.

Todd



Sent from my iPad using Model Engines

 

[mayhugh1]

The object of the head blanks is to have consistent workpieces that I can feed into the canned lathe and mill finishing operations that I generated while creating my first two test heads. This step could be bypassed with the production-level CNC equipment, but hobby-level machines are better suited at giving their user the ability to profile parts that would be impractical with manual machining than they are at efficiently producing large numbers of the same part.
The o.d.'s and the lengths of the blanks were manually skimmed to consistent dimensions that are slightly over the maximum dimensions of the finished part. I roughed-in the combustion chambers using a 15/16" tailstock drill bit on my 12"x36" Enco lathe which was used for the blank preparation. A semi-finishing operation involving a portion of the eventual bottom-most fin was also completed at this time on the blank in order to save a tool change in the first lathe CNC operation. The machining time per blank averaged about 20 minutes, and the total blank preparation time including rounding up and pre-sawing the material was about a dozen hours spread over four days. - Terry

 

[mayhugh1]

The first CNC operation is lathe operation to finish the conical combustion chamber. The portion of the i.d. that will be threaded later is only semi-finished at this time. I can't seem to hold the tolerances I want when doing lathe tool changes, and so when I run batches of parts I typically do only what I can in any given operation with a single tool in a single set-up. In addition, I add code to each of my lathe programs that rapids the tool away from the part after the operation is completed and to an X-axis location that corresponds to a key measurable diameter on the part. I then correct the X-axis DRO to the actual measured diameter on the current part before running the next part. Although this extra step adds to the cycle time it typically allows me to hold 2-3 tenths over any size run. The Z-axis is re-referenced when each new piece is chucked, and so this axis is continually corrected. On this run of 25 parts I only had to correct the DRO once. When taking heavier cuts or working with steel, I sometimes have to make corrections every two or three parts.
For internal profiling operations such as the one within this combustion chamber I use a SVJCR tool holder that I've aggressively ground for increased axial clearances. Even the bottom of the insert is ground for a little additional clearance. All 25 parts were done on a single edge of a single Korloy insert that still showed showed no wear at the end of the run.
The average machining time per part was about 10 minutes and so I ran about 5 consecutive parts and then allowed the machine (and me) rest for an hour or so. The headstock on my lathe gets pretty warm after 30 minutes or so of continuous running, and so I try to avoid extended running times especially when the shop temperature gets above 80F.
The second lathe operation uses an internal threading tool but it finishes the head gasket sealing surface as well as threads. The previously semi-finished gasket surface is skimmed with the not-intended-for-cutting end of the threading insert. The threading tool is also used at high rpm as a boring tool to finish the i.d. of the combustion chamber to the minor diameter of the 1-1/4 x 24 internal thread before the actual threading operation. The i.d. is then measured, and the X-axis DRO is corrected for the next part as described earlier. Keeping the starting minor diameter consistent is key to keeping the thread fit close and consistent over the entire batch of parts. This operation results in the gasket surface being machined square to the axis of the threads for the best seal against the cylinder. After threading, each part is checked with the thread gage that I made during my H-9 engine build. I also selected a few completed cylinders for their close fit to the two test heads I previously made and used them to spot check their fits with my new heads. The threading with all its secondary operations and manual checks required an average time of about 12 minutes per part. Since the actual lathe duty cycle was low I threaded all the parts in a single grueling six hour run. The total machining time invested in this run of 25 parts is now at 22 hours. -Terry

 

[mayhugh1]

The third lathe operation was fun because it's about as close to a real shop production run as I'll ever get. I set my threaded mandrel up in the 5C chuck, and touched off the tool's Z-axis to the mandrel's reference surface. Then I threaded the part onto the mandrel and started the cutting program. Ten minutes later the part was removed, and its maximum diameter and length were measured. The lathe DRO's were corrected if needed, and then the next part was then ready to go. The difference between my run and one in a commercial shop, though, is that I was scrambling during the entire operation to guide the hot, sharp stringers away from a tiny gap between the mandrel and the chuck collet and from behind the chuck where they seemed to be drawn by some mystical force to create a scary coiled up mess. This is a common problem when cutting aluminum with a CNC converted lathe that doesn't have a slant bed.
The purpose of this operation is prepare the part for the final lathe operation which is the fin profiling. It removes a lot of material, and the shape of the head finally begins to emerge. It's most important function, though, is to present an optimally shaped workpiece to the fin grooving operation. The flat workpiece surfaces above the eventual fin grooves help make my CAM's grooving operation happy so it will behave and generate the pecking cuts that my lathe likes to see.
I expected the fin profiling operation to be the most stressful step in the entire head machining process. During the first two test heads the deep grooving in the rightmost three or four grooves felt like they were on the verge of uncontrolled chatter. I had to continually vary the spindle speed vernier manually in order to quell an audible tone that was my indication that trouble was beginning. Modulating the spindle speed kept the surface finish pristine, but the whole process was scary and tedious at the same time. And, I was about to do it 25 more times. The C2 inserts that I had switched to for this run really didn't seem to help much. In addition, during the entire operation I have to continually clear stringers again; but this time it's more critical. In this operation the stringers have to be quickly fished from the bottom of each groove before the grooving tool continues with its finishing passes at the bottom of the narrow filleted groove. The full radius inserts that I'm using aren't designed for the lateral finishing that I'm doing, and so if the chips aren't kept cleared the insert can become jammed in an ensuing mess at the bottom of the groove. After some practice it really isn't all that bad, but I really have to stay focused throughout the whole 25 minute operation.
Then serendipity stepped in. I was on the third head of my run of 25 when I noticed that I didn't seem to have a chatter problem anymore. Sure enough, it was also completely gone on the next two heads. While clearing stringers I was trying come up with a reason why my insert might somehow becoming 'conditioned' with use, but eventually decided that wasn't sensible. Then I realized I had forgotten to set up the tailstock on the last several parts. During the development of my cylinder grooving operation I discovered that tailstock support was required to stop the chatter while grooving those parts. I assumed it would help with the head grooving also. When I added the tailstock back into the setup for the next head the chatter returned. It seems that rigidly supporting the head between its two ends sets up a resonance that is excited by the cutting tool running in the rpm range I'm using. Removing the tailstock frees that end; and, if the resonance is longitudinal, drops its frequency a factor of two which evidently moves it out of the excitation range of my operation. This probably also explains why it was the grooves near the far end of the part that seemed to create most of the chatter. Another thing that I noticed was that if I didn't use the tailstock, the parts easily unscrewed from the mandrel when the operation was completed. If I did use the tailstock, the parts ended up so tight in the mandrel that I had to use a strap wrench to separate them. I think the vibration from the resonance was working with the tightening forces created by the tool to over-tighten the part on he mandrel. Needless to say, I quit using the tailstock.
The fin profiling operation completes the lathe work on the heads, and maybe my lathe but surely my back is grateful. My run of twenty-five parts accumulated another 23 hours of machining time during these last two operations, and so I'm now at a total of 45 hours.
Before beginning the milling operations I really have to get back to my CAD work on the rocker arm supports. I've been thinking about a new design for them, and it might affect the first milling operation somewhat. So, it's time to finalize this portion of the head design before doing any more cutting. - Terry

 

[Walltoddj]

They look better every time I see them great work. Now I'm going to have to buy a CNC lathe and it's all your fault( that's my story and I'm sticking to it).

Todd


Sent from my iPad using Model Engines