CNC12 EX Rotary erratic speed

Has anyone else had erratic rotational speeds with their rotary axis with the new CNC12 EX controller?

See two videos (having issues embedding them):

  1. Avid rotary very slow

  2. https://vimeo.com/1053101960 (more erratic)

These are simple 3D roughing toolpaths - Z layer by layer - from VCarve Pro. This means there is very little X movement (only a step over) and all the wrapped Y movement is pure A rotation. There is no Z plunging during the A rotation. Watch how unequal the rotation speeds are from one direction to another, how slow the X stepover is, and in the second video, after two passes, how fast the chuck speeds up. The chuck speed should be consistent all the way through.

This is untenable - I cannot make a toolpath feedrate to compensate for going that slow, but then not crashing/ stalling or breaking the bit off when the chuck speeds up. At the moment, the Mach4 processor was far smoother with the rotary. Something is wrong. Anyone else have these issues?

When I tried Exact Stop smoothing and did a toolpath along the X axis (no rotation, no Z plunging), the X motion was fine, but a tiny stepover in A rotation caused a good 10-15 second pause at the turn-around point. If the bit had been in the stock (rather than beyond it or doing an air pass) the bit would have burned the wood.

I’m running the new CNC12 EX controller with a 5x10 Pro machine with rotary recess-mounted along the X axis pointing towards -X (chuck at +X end), running profile 5.22, using Contouring Router smoothing.

Can you post your G code here?

File 1a (video #1) had a very slow feedrate (probably around 5ipm) because of abundant caution about the erratic rotary speed.

This ended up so slow that for file 1b (video #2) I increased the feedrate up to 25ipm (while slowing down the plunge), although 25ipm is still slow; I never would have had more like 100+ ipm in Mach4.

You can read the gcode to see that there are pure A0 - A360 rotary movements without weird pauses at the beginning of the file. Since there aren’t multiple rotation gcode lines making up a single full rotation, why would the EX controller be slowing down at random points?

Why the gcode speeds up on deeper Z-level passes I likewise do not understand. That shouldn’t be how the file is post-processed; it was not the case with Mach4. The different Z-levels are still the same Y-feedrates for the unrolled surface in VCarve. Is the EX controller trying to adjust for a reduced perimeter distance the closer the endmill gets to the A axis? If so, that would be terrible for attempting deep cuts; the endmill would stall trying to ram through the material at the top of the flutes.

Thanks
1a-Rough top strip shallow chuck depth.cnc (8.3 KB)
1b-Rough top strip shallow 25ipm.cnc (8.3 KB)

I took a look at your g code. It’s posted correctly, however your feedrates are VERY slow:

So the controller is executing the G code exactly as it should. The problem lies in how you have your file setup.

For reference the max rate for the rotary is 12000, you’re feeding at .2. Your Z moves are 85 IPM.

Check the settings in your VCarve/Aspire file and try again, or post the file here and I can take a look

The issue might be the post-processor. My shop computer is NOT hooked up to the internet, so the post-processors it is using are the ones downloaded from the Avid support document site (avidcnc-ex-posts-for-vectric-1.1.zip) and imported into VCarve. That computer/ VCarve created the gcodes used in this issue.

My office computer IS hooked up to the internet. So within VCarve, I went to Machine/ Update Post-Processor Database, then Machine/ Machine Configuration/ Associated Post-Processors and selected the two Avid EX inch processors (XY and Along X).

Now you might say that the two post-processor methods ought to produce the same results. But they don’t.

The shop computer’s gcode from the manually-updated, Avid support site typically only lists one feedrate for a section of rotational moves, and on gcode line numbers that match the unrolled XY-processor gcode, and match the feedrates for Mach4 Y2A, while the office computer with the internet-updated gcode gives a new feedrate for each line of rotational moves, which matches more of the style of Mach4 but not the exact same numerical feedrates.

Which is your latest version?

Even so, both computers gave rotational feedrates of F 0.8 and F 0.2 for 25ipm and 5ipm, so perhaps the VCarve file has a glitch in it. I’m sending you that file to test.


COMPARE Rough top strip 5ipm_P50_XYpostprocessor.cnc (7.8 KB)
COMPARE Rough top strip 5ipm_P50_ExAlongX.cnc (8.2 KB)
COMPARE Rough top strip 5ipm_P50_ExAlongX2.cnc (9.4 KB)
COMPARE Rough top strip 5ipm_Mach4 Y2A.txt (8.4 KB)

You’re right… but there are two issues going on here… let me explain:

The posts pulled from Vectric or manually downloaded from our site should be identical, and they aren’t.

I’m going to get that corrected quickly, but lets focus on getting you up and running.

The issue is that when you’re doing moves that involve for example just the Z axis they should be in IPM, and ones that involve the rotary should be in deg/m.

The posts from Vectric had it correct, and our hosted posts didn’t have that 100% correct. What should have been happening is that feedrate should be set for each rotary move, and it was only set once. So it still worked, but it was not allowing Vectric to update speed if it thinks it needed to.

So when you ran your file you got only one feedrate set for A moves. Your feedrate was VERY slow, which points to your second problem. Since Vectric only had a chance to set it once, it was probably for a very short line segment that happened to have a very low setting.

You mentioned your feedrate to be 25 IPM, that seems incredibly slow. I see you’ve got a long thin bit on there, you might consider bringing that up to 100 IPM or something. Not saying that this was the problem, but it was a contributing factor.

For contrast I was able to run a file with the post that was not putting out feedrate changes at the right time at 250 IPM and it ran pretty good, although smoother and more consistent with the “correct” post.

So, what I did was go back through our posts and I made a few tweaks to them and bumped the version to 1.2 (we have 1.1 hosts on the site right now)

They’re attached here. I’d love for you to give them a try. I tested them out today and they are running well, and putting out the speed changes that are appropriate.

What I would do is go into VCarve/Aspire and just clean out any machine configurations and posts you have… just delete them all so there’s no confusion. I say this because these posts are named the same as the old ones.

Check this video to see how to install these posts:How to install rotary test posts | Loom

Posts 12.zip (8.3 KB)

1 Like

You’re right as well. At my shop this afternoon, I came to the same conclusions you did.

Both post-processors were labeled as V1.1 but were not identical.
The Vectric-downloaded p-p, with its many feedrates, ran far smoother than the Avid-downloaded p-p with its singular feedrate.

The reason the file was down to 25ipm (or even 5ipm) was that when I was running the Avid-downloaded p-p with the rotary rotations out of control at 150ipm, I tried reducing the speed again and again, without much success.

I’ll try the new p-p tomorrow. The Vectric-downloaded V1.1, even though it worked better, did seem to have some irregularities in the speed of purely X-axis moves (even understanding that Contour Router smoothing was on). Hopefully V1.2 solves that.

I tested this one and the speed was very consistent. I think this will totally solve your issue. Please let me know how testing goes

The new post-p v1.2 is consistent and speeds do resemble the toolpath feedrates. Nice. What did not seem to be visible was any acceleration/deceleration smoothing. Even though Contouring Router was on, the machine acted more like Exact Stop was on, except without pausing. Perhaps my test file was too primitive or the ipm was too slow to trigger smoothing. I’ll run another test or two before trying an actual job file.

That sounds normal. You can play with the sliders on those presets too to make the machine more “mushy” or “notchy”

Honestly, I’d just leave it on Precision or Countouring router and go with it.

Glad to hear they’re working though!

We’ll post an update to those posts soon, but feel free to keep using those, and please provide feedback

Hey @FlynnAD wanted to check in to see how those rotary posts were working for you?

I only had custom glued-up material on hand which I was unwilling to use on rotary tests. Making some foam blocks now to try with the next project’s toolpaths. Will let you know. Thanks!

Sweet, you can always do air cuts too