Little Demon V8 - helpful hints (hopefully)

[Carbuilder]

Yes, I cut 2 cam lobes a bit too thin on my first one. I think a key point here is to blue and mark all the cuts first, so you can see that they all look correct before cutting.

 

[Carbuilder]

Finally, I have a camshaft!

I know I could have produced the cam in a fraction of the time it took me if I made it in the traditional way; indexing it around on the lathe and taking cuts every 5 degrees or so. But I was determined to do it on the 4th axis of the CNC. And after many weeks of trials, incorrect software settings, and broken cutters, it is done. It was cut with a carbide 3/32" 4 flute ball nose cutter, with very conservative speeds (after breaking too many cutters). Thus, 6 1/2 hours of CNC.



After the lobes were CNC'd, I did mess up the end that the gear goes on. Got it just a bit undersized. So I machined it down to about 1/8" diameter and made a thin steel tube to press/locktite on. Then machined it to the proper dimensions.



One interesting thing I found (that turned out to help me a lot) is that with the spacing of the lobes at that end of the cam it grips in the 1/2" collet perfectly centred, as you can see in the picture.

My wife says she never wants to hear the word camshaft as long as she lives.....or maybe just as long as I live?

Rick

 

[stevehuckss396]

Nice work. Did you capture any video of the machine running?

 

[Carbuilder]

Thank you Steve. No, I didn't video any of that one. I did take some video early on when trying to see what the issue was with my CNC. That is when I saw the cam stop rotating but the program kept running, along with the 4th axis indication changing (when it wasn't actually moving). So video of the final machining would have been pretty boring since it was very slow.

I machined it with what DeskProto refers to as "around A-axis" machining. The cam rotates and the cutter moves up and down, centred on the axis of the cam. Then it moves over on the X-axis and repeats. It does it with a rough pass and then a finish one. Over, and over, and over............

 

[Eccentric]

Congratulations on finishing your Camshaft. I know the process of getting the CNC working with the 4th axis was a real challenge, but next time will be a breeze. You must really feel satisfied to have worked out all the kinks in the process and have a nice camshaft to show for it. Great job.

 

[Carbuilder]

Got back into the engine project. Some of the delay was buying a Taig CNC lathe. Found a used, but not used (person bought it but never actually used it), one and it took time to set it up and learn how to program it; different than a CNC mill. The first items were the lifters for the engine. After a LOT of trials, learning, mistakes, finally made some nice parts.

Working on the valves now.

I put together a video on making the lifters.

Rick

 

[michael-au]

Very good Rick
Good find on the lathe, works great, nice looking parts
You will be finished in no time

Some of my delay is setting up the mill with a new controller, slowly getting there

New parts are inside the line

 

[Carbuilder]

Don't know about being finished in no time. If I would spend less time on the CNC stuff and just make parts then maybe.

I'm finding a lot of inconsistencies with trying to get the dimensions correct on the parts. Once it is done and ready to go I can make one after the other with almost dead-on precision. But I run a trial piece, measure it, tweak the program or setup, make another one, and maybe it changes the way I intended and maybe not. It has to be something with mach3. I've briefly looked into Masso and Centroid Acorn as alternatives. I'm used to mach3 on my CNC mills, but on the lathe it seems to be a whole different story.

Trying to get that little slot at the end of the valve the correct depth is driving me crazy. According to a simulator it should be cutting the part almost in 2. But when I run it, it barely cuts into the part. Very strange.

Hope everything works out with the new controller for you. We'll get there eventually!

Rick

 

[michael-au]

I have the valve partly done, need to finish them off with wet and dry sand paper so the are nice and smooth
I am going to make a piece of round aluminium with a hole the valves fit through and then cut a slot down the side so it can be clamped in the lathe chuck, then I will turn the groves on the end

Valve looks good though, I found there is a big difference programming the lathe over the mill too

 

[bob shutt]

Not sure how far you are turning back to put groove in. I only turn far enough to clear groove tool leaving as much strength as you can. Then come back in with turn tool.

 

[Carbuilder]

Yes, that is how I'm doing it. I turn it down to .098" dia for a short length, cut the groove, then come back and turn it to .094" dia up to the point in the stem where the diameter changes. So it isn't a deflection issue with the groove. It must be something wrong I'm doing. I did get the groove close to the correct depth a couple times, but then tweaked things a bit to get it correct and sometimes it works and sometimes works the opposite.

I'm using EziLathe to generate the code, which is a pretty cool program. When I run the code in that simulator the groove almost cuts the part in half. In reality it doesn't cut deep enough. So that is the strange part. The tool setup is correct on the machine. Something strange I'm finding is that if I stop the machining before it is complete (like if I see that something is not right and don't want to complete the test part) and return tool #1 to 0,0 it isn't the 0,0 that it started out at. So something is changing the 0,0 point and that is throwing things off. But not if the machining completes. A setting in mach3 that is wrong? I should probably ask on the mach support forum and post my code.

I don't have issues with mach3 on my CNC mill or router. If something is not machining correctly I can usually find what I did wrong. But the mach3 turn seems to be a whole different story. After doing some searching around on the net it does seem like most people agree with this. I'm always up for learning new things so thought it might be interesting to dump mach3 on the lathe and get something else. Why not start a whole new system with its frustrations?

Rick

 

[mayhugh1]

Yes, that is how I'm doing it. I turn it down to .098" dia for a short length, cut the groove, then come back and turn it to .094" dia up to the point in the stem where the diameter changes. So it isn't a deflection issue with the groove. It must be something wrong I'm doing. I did get the groove close to the correct depth a couple times, but then tweaked things a bit to get it correct and sometimes it works and sometimes works the opposite.

I'm using EziLathe to generate the code, which is a pretty cool program. When I run the code in that simulator the groove almost cuts the part in half. In reality it doesn't cut deep enough. So that is the strange part. The tool setup is correct on the machine. Something strange I'm finding is that if I stop the machining before it is complete (like if I see that something is not right and don't want to complete the test part) and return tool #1 to 0,0 it isn't the 0,0 that it started out at. So something is changing the 0,0 point and that is throwing things off. But not if the machining completes. A setting in mach3 that is wrong? I should probably ask on the mach support forum and post my code.

I don't have issues with mach3 on my CNC mill or router. If something is not machining correctly I can usually find what I did wrong. But the mach3 turn seems to be a whole different story. After doing some searching around on the net it does seem like most people agree with this. I'm always up for learning new things so thought it might be interesting to dump mach3 on the lathe and get something else. Why not start a whole new system with its frustrations?

Rick

One or two things to check for with lathe CNC: 1) make sure that both you and your software(s) are using the same definition for depth-of-cut, i.e. radius or diameter, and 2) make sure that both you (during zeroing) and your software(s) are using the same definition for tip of tool.

I ran into both the above when using mach3 with my CAM software when I first started. I still have issues when trying to do precise profiling. I'm not sure my CAM software accurately handles the tip profile of some of the cutters I use. - Terry

 

[xpylonracer]

Rick

Check to make sure you haven't got a backlash problem on the X axis as that could cause loss of travel into the work after a toolchange if the
grooving tool moved out from the job to provide clearance before making the groove cut.

xpylonracer

 

[Carbuilder]

I'll double check for backlash, but pretty sure there is basically none. The grooving cutter moves into position and then slowly makes the cut. But the depth of it is not consistent with what I've programmed. The other dimensions are generally good. But like I said, sometimes when I return to tool #1 and zero it, it isn't where it started; maybe .050-.100" off on the X-axis.

The radius/diameter thing seems to be good since the part is being machined to the correct size, other than the groove. I'll post a bit of the code in case anyone is curious. I am slowly learning the different codes, what they mean and what they do. The reason for flood coolant being turned on instead of the spindle is that the spindle outlet on the control box didn't seem to work, but the coolant does. Since I'm not using coolant I plugged the spindle into that outlet and use it to power the spindle. It starts with this:

(EziLathe Version 1.7.3.0 Mach3 2022-04-09 12:58:59 PM)
(Dxf file = Valvex Bar = 0.25)
G18 G40 G49
G90 G94 G80
G20 (Inch)

T0101 ( tool cuts with left side)
(Process = O.D. Turning - Cut Right to Left)
M08 (Flood Coolant On)
G00 X0.35 Z0.05
(Rough #1 R-L)
G00 X0.245
G01 Z-0.1754 F5.0
G01 X0.35
(Rough #2 R-L)....

that goes on a bit and machines the end of the blank where the groove will go. Then the groove cuts:

T0303 (slot .028 wide)
G00 X.100
G00 Z0.1
G00 Z-0.08
G01 X0.01 F0.25
G00 X0.105
G00 Z.1

See how this should be cutting the part almost in 2 (X0.01)? It doesn't come close to that depth.

Something wrong with the initial codes at the start?

Rick

 

[bob shutt]

Call up the offset for the tool on the rapid line
T0100
GO X 0.300 Z0.050 T0101

T0300
GO X0.100 Z0.100 T0303

Sometimes lathes do not want to pick up right unless it is moving.

 

[oldCB]

Now that the wordy introduction is done, on to the crankshaft.

I’ve never made a crankshaft like this before and from everything I’ve read, it was going to be a challenge. The issue, as far as I could see, was that the drag of a lathe tool against a fairly flimsy crank can easily lead to it bending, jamming, and being ruined. So how to minimise this?

Here is how I did it. I do have a rotary table for my CNC mill; the 4th axis. But the mill is not huge and there is not room for the 4th axis and a 6” length of material sticking out of it. Here is where things get weird.

My new mill, the PM728 is beside the CNC mill. So I bolted the 4th axis onto the table of the PM mill, but left it plugged into the CNC mill. So I wasn’t using the 4th axis under CNC control, but just using the software to rotate it as needed manually. Here is the setup:

View attachment 132453

The idea was that I could use the mill to machine away most of the material. I figured a rotating cutter would put a lot less stress on the part compared with cutting it in the lathe. I roughed out the main journals first, as those didn’t require any offset of the crank. So far, so good.

View attachment 132454

A test cut at the right and then on to the main journals.

View attachment 132455

I’ve bought a number of kits from Hemingway Kits over the years and highly recommend them. Oh, if you do any threading on the lathe, their retracting tool holder is fantastic! But I digress. I had their Keats Angle Plate kit for a while but never got around to making it. So a time out while I made it. OK, now I’m back. This holder allows for a fairly easy setup for offset turning.

View attachment 132458

View attachment 132456

So what I did was to slowly lower the cutter in the mill spindle, while using the 4th axis control to very slowly rotate the crankshaft. I would allow it one complete rotation and then lower it another .010 or so. Of course the surface finish was not good enough for a finished journal, so I left them all oversize to finish on the lathe. This way I only had a few thou to clean up and with slow and careful work didn’t bother with putting any filler pieces between the journals to stiffen it up.

Did it come out perfect? No, but hopefully close enough. Once back on the lathe I cleaned up the main journals to get the runout near zero. I was a bit surprized how flexible it is.

View attachment 132457

I decided not to push my luck and machine the crank offsets to look more like a real crankshaft. I considered myself a bit lucky to get this far with my first crankshaft.

So that is my multiple mill, semi CNC, rotary table, crankshaft production. Of course a normal rotary table would allow you to do the same thing, just with a lot of cranking. But if machining the crankshaft right from the start on the lathe frightens you, maybe consider this method.

Rick

Nice work, well done.

 

[Carbuilder]

Finally got back to some work on this little engine.

I tossed out Mach3 and bought the touch screen Masso unit. It is really nice! Not much of a learning curve, the touch screen works beautifully, it is all-in-one so no separate computer used. I upgraded the steppers to the ones Masso sells which are closed loop; if it misses a step the system knows that and corrects. I use EziLathe to to the basic CAM programming, starting with a DFX drawing of the part....nice program!




Getting back to making the valves. I machined them in the traditional way. I did not machine the groove in the end, and when parted off I left the valve head a little thick:


I flipped all the valves around, held in a small collet, and faced the heads off to the proper thickness. Now to produce the little groove in the end of each one. That was giving me some challenges. I ground a small cutter to a thin end and used that for the first one. Then messed up and bumped it into the stationary piece and snapped it off, so looked for something better.

I machined a small mandrel, cut a slot in it for a box cutter blade to sit in, and secured it with a screw with a bit of a point. I used a carbide end mill to put a hole in the blade:





It looked good and might have actually worked. But the issue was (not enough thinking ahead here) that the screw end stuck out too far. It would hit the headstock of the lathe before it got to where the groove had to be machined. Oh well, onto MKII...

This one was actually a bit simpler to produce:



Milled a shallow recess in the end of the mandrel, put a slightly larger hole in the blade, and secured with with a screw (machined down a bit to minimize the stick-out of the grooving tool). This one worked like the proverbial charm and I got all the valves grooved:



I think the rocker studs will be next. Ideally machined and single point threaded on the CNC lathe.

Rick

 

[Carbuilder]

I completed the set of rocker studs and made a video of the machining.

The CNC machining could have been more efficient; some of the passes are a bit slow (very conservative) and the tooling paths are not optimized for production. But for home machining, time is generally not money so I tend to machine on the slow, conservative side and when things are going well, why push it.

I made the set-up pieces from drill rod since I have more of that than 12L14 steel (which is called out for these parts). The cleanup pass with the cutter after threading was required with the drill rod (the threading tended to raise some material) but not really required with the 12L14; but I left it there to be safe. So the first couple of parts are from drill rod and the remaining ones are from 12L14. The main difference is that the drill rod produced long machining strings and the 12L14 produces small chips.

I'm very pleased with how these came out and I am really getting the hang of the lathe and the Masso system. First time doing threading on the CNC lathe.

Rocker Stud Machining

Rick

 

[michael-au]

Good work Rick, I like your lathe, works very well and saves a lot of time
How are you finding the Masso, I like it on the mill, much better than Mach3

Michael

 

[Carbuilder]

I still use Mach3 on the mill and I'm OK with that. But on the lathe it was a pain, especially setting up the tools. Far easier on the Masso. Tool set up and tweaking is dead easy. I would certainly recommend it to anyone who wants to get away from Mach3. The support is very good too.

Next, the cylinder liners so I can get them in the block and then make the pistons. The plan is to drill the liners slightly undersize on the manual lathe, then program the CNC one to bore them to final size, and machine the outside. Probably a set of 2 at a time, starting as one piece twice the length. So I'll machine one, flip the piece around, machine the other one, then part it off making 2 parts. That's the plan anyways.

Rick