Rotary + CV + G00 = Clunk

[spinningwood]

Running a CNC Router with a rotary axis.

Running a vcarve toolpath (lots of short movements and moves up to safe z for rapids) that carves on a cylinder.

Using CV I get a clunk from the motor on the z-axis (probably losing steps) on a lot of the G00 moves to up safe z which preceedes a G00 move to a new A.  Sample code that clunks:

N680 G1 X0.0965 A-19.6482 Z0.1927
N690 G00 X0.0965 A-19.6482 Z0.4050
N700 G00 X0.0965 A-30.9263 Z0.4050

I get the clunk from the z motor on line 690.

If I switch from CV to Exact Stop, I don't get any clunking.  This toolpath runs very smooth with exact stop set.  Changing motor tuning (velocity / acceleration) makes no difference with CV, unless I drop to super low levels that would be crazy to use.  Tried different values for CV distance tolerance and angle, but it didn't help CV run this toolpath smoothly.

If I take the exact same toolpath and run it on a flat surface (using y instead of the rotary A), I can run with CV and it is completely smooth.  No clunking on the G00s. 

I don't have any long arcs (with multiple segments) in this particular toolpath so I can run it with exact stop.  But that may not always be the case.

Is there some setting somewhere when using A as a rotary axis that will allow CV to work like it does in the flat world?

It's almost like Mach3 is picking up the acceleration from the A axis (which is really high) and using it for the z axis when it is doing the G00 move to safe z with CV on.

My A Axis (rotary) is velocity 18810 and acceleration 3151.

My Z Axis is velocity 200 (inch per min) and 50 acceleration.

I could see where slamming the z motor with an acceleration of 3151 might result in a clunk or two.

I'm new to Mach and still learning the ropes, so I apologize if I didn't explain things clearly.  I tried searching the forums but didn't find anything that helped me.

Any and all help welcome.

Thanks,

Ed
 

[Tweakie.CNC]

I think your problem relates to the exceptionally high speed you have set for the rotary axis and because it's movement is on the same GCode line as the X and Z you are getting a 'Blended Feedrate' which is higher than either your X or Z can individually tolerate - thus the 'clunk' and missed steps.

Tweakie.

[spinningwood]

Hi Tweakie - Thanks for the reply.

The numbers on the Rotary A axis are big, but they are in degrees per minute.  They equate to around 50 rpm which isn't very fast.  But if Mach doesn't differentiate between degrees per minute and inches per minute when computing a blended feed rate then it would definitely overdrive the x / z axes.

I could drop the speed of the A axis way down, but that creates other problems for me.  But I'll do it as a test to see if that solves the problem.

If I'm understanding you, even though only the z value changes from line N680 to N690, Mach will still do a blended feed rate because the A parameter is on the line (even though it doesn't change).  I'll try another test where I strip each line down to just the changed parameter and see if that solves the problem (e.g. line N690 would just be "N690 G00 Z0.4050").  I don't think I can get my postprocessor to do that for me, but I can write a little bit of code to handle the task.  A post post processor of sorts.

But I'm still wondering if I overlooked an option somewhere that would prevent Mach from using the Rotary degrees/min as though they were inches/min to compute a blended feedrate.

I tried the rapids overide which I would expect to keep the velocity within the range that x/z could handle.  That didn't solve the problem.  Maybe if I had an acelleration overide as well.

Off to do some testing.  Will continue to hope that I spot some option checkbox somewhere that will magically solve it all.

Ed

[docltf]

try changing your g00 to a g01

[spinningwood]

Hi docltf - I tried changing G00 to G1 (should be the same as G01?) last night.  It didn't help. 


Thanks for the suggestion though.

Ed

[spinningwood]

After a lot of trial and error, here's the combination of things that seems to work for me.

Dropped A axis to 9000 (degrees/min) velocity and 1000 acceleration.
Dropped X/Z axes to 150 (inch/min)  velocity and 17 acceleration.
CV on.
Set CV Dstance Tolerance = 1
Set Stop CV On Angle > = 89


The good news is that I haven't found a toolpath that will lose steps (clunk a motor) with these settings.

The bad news is that some toolpaths that previously ran really fast and smooth are now running not quite so fast, but smooth.

I'll run with this for a while and see how it goes.  I may eventually create a couple different profiles for mach so I can push each toolpath to optimal performance, but for now it's probably better to limit the number of variables on each job as I'm working my way up the learning curve.

Thanks to all who replied.

Ed

[stirling]

My guess here is that with those settings you're probably effectively turning CV off and that's why the problem *appears* to have gone away.

Back to your OP...

Using CV I get a clunk from the motor on the z-axis (probably losing steps) on a lot of the G00 moves to up safe z which preceedes a G00 move to a new A.

The thing of interest here is that CV is not (or should not) be doing anything anyway in this situation because it doesn't (or shouldn't) blend a rapid into a rapid.

In the three lines you've shown, the only blend should be between the first two lines and even then it's a "straight" blend (Z into Z)

what happens if you put a a zero length dwell (G4 P0) bewteen 680 and 690?

Ian

[spinningwood]

Hi Ian - If I just switch off CV, then I get really jerky movement on toolpaths with arcs.  With CV on and the settings I am now using I get smooth movement.  So it is still having some effect with those settings.

But I'm willing to try other things to see if I can solve the problem in another way that gets my speeds back up a bit.

I'll try your suggestion on G4 P0 later today and report back on what happens.

Thanks for the suggestion.

Ed

[docltf]

ED

my settings are

checked  Set CV Dstance Tolerance = 0.023
unchecked  Set Stop CV On Angle > =0

bill

[spinningwood]

Summary of trying Ian's suggestion for "G4 P0":

Returned to my original settings:

A = 18810 vel and 3151 accel
X = 200 vel and 50 accel
z = 200 vel and 50 accel
CV = on
Set CV Dstance Tolerance = not checked
Set Stop CV On Angle > = not checked

Ran a quick test putting a "G4 P0" between lines 680 and 690 (in my OP).  Clunking gone.  Didn't have time to check and see how the overall results compare to my previous solution (motors tuned down and cv options on) for overall speed and quality of cut.  I'll run some test cuts tonight.

If the "G4 P0" turns out to be a better solution, I'll have to figure out how to insert them.  Not sure I can adjust my post processor to do it.  I can probably write my own post post processor to add them (there are a bunch of them needed), but it would sure be easier if there were an option to check in Mach 3 somewhere that would have the same effect as inserting those "G4 P0" codes.

Anyway, thanks for the lead on another possible solution.  I'll keep working on it.

Ed