Is it possible to use Mach on a lathe to grind a camshaft lobe?

I'm restoring an old motorcycle single lobe camshaft for which there is no master. I've modeled the lobe profile in Fusion360 and can generate a toolpath on the mill to cut out the cam profile from a blank. However, I have to finish the hardened faces of the lobe on the lathe with a tool post grinder. Is there any way to index the X axis movement of the toolpost with the spindle rotation? Mach knows, given a specified rpm, the angular position of a part in the spindle that is indexed to the tool (grinder position in X). How do I make the X axis move in and out in relation to the angular movement of the part in the spindle?

Andy Pugh, lead LinuxCNC developer in the UK, has this video showing what he did.

https://youtu.be/z6dK41_usfQ

Hi,
I've done a similar thing in Mach4 but imagine it could be done in Mach3 also.

It requires position loop control of the spindle, ie it becomes a C axis.

What you have proposed (constant velocity spindle results in linearly increasing angular progression) is NOT position
control, but requires Mach to integrate velocity, it will not be accurate enough, you require precision within a few tenths
of a degree whereas integrating a constant speed will result in angular error of several degrees (forever increasing) after
only a few revolutions.

Craig

Thanks Craig.

Would the same angular velocity issue apply to a rotary table configured as the A axis into which I put the cam lobe and then attach a grinding wheel to the mill spindle?

Hi,

Would the same angular velocity issue apply to a rotary table configured as the A axis into which I put the cam lobe and then attach a grinding wheel to the mill spindle?

No, the critical phrase here is 'as the A axis'. Its the fact that it is an AXIS, ie capable of positional control and can therefore
in incorperated  into  a coordinated interpolated movement. Because the A axis can be interpolated your grinding program would
work fine.

If you had a spindle that had positional control and thereby become a C AXIS, it to could be used in a coordinated interpolated
movement.

Mach is not suitable as a feedback controller by virtue of the motion buffer imposed by Windows OS's. If however you
required a very low bandwidth feedback loop, then if your spindle were fitted with an encoder you might achieve your aim.

Lets say you have an encoder fitted to the spindle, and at the moment the angle is 45.89 degrees from some nominal
home or index position. You could use Mach to calculate the required X axis position to grind the surface of the lobe from
your previously calculated lobe profile. Mach would issue an X axis movement. The motion buffer would mean that the
movement would ocurr  but delayed by 200ms or so, the length of the motion buffer.

Now the spindle is rotating, and as you will see, rotating very slowly. Lets say that is has rotated by one degree, now
46.89 degrees. Mach could again calculate the required X axis position to grind the lobe and send the required movement
instruction via the buffer to the machine.

Provided the spindle rotated VERY slowly then the X axis would follow the proflie you want. If however you allow the
spindle to rotate to fast the Mach movement instructions to the X axis will be wrong by virtue of the motion buffer delay.

Having a motion buffer, with its associated delay, is an inescapable fact of using a Windows based PC.

You could achieve a sufficiently accurate X axis following PROVIDED you rotate the spindle slow enough OR have
a genuine C AXIS.

Craig

You would need the spindle set up as the C axis to maintain the relationship of the X and C axis, so it is possible but not on a X&Z axis lathe.

Thank you Craig and Graham

Craig, I now understand what you meant by the problem of interpolating angular movement due to the motion buffer. I run a PMDX411 which they say can do upto 100KHz on four axes, but maybe, that would still be an issue even at a low spindle rpm.

If I created the profile in Fusion360 and can generate a mill tool path do you know if I could use that to grind a cam that is fixed in a CNC A axis rotary table fixed on the mill table? I would either mount the grinding wheel on the mill spindle or to a rigid external attachment. I assume the tool path would be the same whether it is an end mill cutting out the cam lobe profile or used to move a grinding wheel along the same profile.

Joe

It all depends on the shape of the profile, if it has negative areas then the cutter size is critical, too big a tool will over cut and too small a tool will under cut.

Yes, Graham, the size of the wheel is critical. I've calculated effective diameter of the wheel given the profile. It's a cam from the early 1930s and not very complicated. My question is, assuming I have the correct diameter, would the tool path for machining the profile be the same for the grinding wheel to follow. Since Fusion lets you choose the tool size for milling I would have to create a custom tool with diameter of the "tool" being the diameter of the grinding wheel.

However, if I had a CNC rotary table that I set up as the A axis, is there a Mach grinding program that anyone has written that I could use?

Joe