Little Demon V8 - helpful hints (hopefully)

Home Model Engine Machinist Forum

Help Support Home Model Engine Machinist Forum:

Carbuilder

Well-Known Member
Joined
Feb 2, 2015
Messages
90
Reaction score
60
Location
Bolton, ON, Canada
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

Well-Known Member
Joined
Feb 2, 2015
Messages
90
Reaction score
60
Location
Bolton, ON, Canada
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.

Screen Shot 2022-02-17 at 8.24.10 PM.png

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.

Screen Shot 2022-02-17 at 8.24.39 PM.png

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
 

Carbuilder

Well-Known Member
Joined
Feb 2, 2015
Messages
90
Reaction score
60
Location
Bolton, ON, Canada
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

Well-Known Member
HMEM Supporting Member
Joined
Dec 29, 2020
Messages
311
Reaction score
692
Location
Southern California
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

Well-Known Member
Joined
Feb 2, 2015
Messages
90
Reaction score
60
Location
Bolton, ON, Canada
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

 
Joined
Dec 18, 2013
Messages
539
Reaction score
524
Location
Australia
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

Mill.jpeg
 

Carbuilder

Well-Known Member
Joined
Feb 2, 2015
Messages
90
Reaction score
60
Location
Bolton, ON, Canada
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
Screen Shot 2022-04-16 at 9.34.46 AM.jpg
 
Joined
Dec 18, 2013
Messages
539
Reaction score
524
Location
Australia
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

Well-Known Member
Joined
Oct 24, 2010
Messages
110
Reaction score
62
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

Well-Known Member
Joined
Feb 2, 2015
Messages
90
Reaction score
60
Location
Bolton, ON, Canada
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

Project of the Month Winner!!!
Project of the Month Winner
HMEM Supporting Member
Joined
Oct 24, 2007
Messages
1,285
Reaction score
4,303
Location
Central Texas
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

Well-Known Member
Joined
Dec 23, 2010
Messages
367
Reaction score
90
Location
Norfolk, UK
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

Well-Known Member
Joined
Feb 2, 2015
Messages
90
Reaction score
60
Location
Bolton, ON, Canada
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

Well-Known Member
Joined
Oct 24, 2010
Messages
110
Reaction score
62
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.
 
Top