Jerky 4th Axis Simulatenous with Haas (Programming, Machine help)

Howdy, I'm a noob trying to learn how to machine with CNCs, so bear with me.

I'm using a Haas VF2SS with NGC and a Haas rotary A-axis mounted to the table. Using Fusion 360 to program a spiral rotary toolpath to rough square stock into a cylinder with simultaneous milling. The code posts just fine and the machine will accept it, but the rotary movement is jerky and I can't seem to fix it. Here's a link to a short video of the dry run so you can see what I'm talking about. Ignore the ghetto lathe center setup.

I've followed Haas's troubleshooting for jerky simultaneous milling and everything seems good with my machine settings. The machine has HSM, so I get as much look-ahead as I can. The code is posted using G93 which is Inverse Time feed, I guess? This seems to be what people suggest based on what little info I can find, and the machine won't accept me posting it as DPM feed anyway for some reason. I've also tried tolerance values in Fusion 360 from .0004 to .1, and while the bigger tolerance values make the toolpath a little smoother, it doesn't solve the problem. The problem also persists if I change the toolpath to a circular one, with no X-axis movement for cuts(minus stepovers), so it doesn't seem tied to constant X-axis movements.

I can't find any info on how else to solve this, so does anyone here have any ideas?

Post your code.

CNCPleb said:

The code is posted using G93 which is Inverse Time feed, I guess?

Click to expand...

Yes, G93 is inverse time feed. You need a feedrate on every line and your feedrates will look much different than IPM rates.They will be much larger values.

Inverse time is making sure that all commanded axes arrive at the destination at the same time....per line of code being executed.
If you used G94 and told it(assuming a start point of X0Y0A0) X1. Y1. A156, X and Y will get to 1 while A is still rotating to 156. Not good.

I've had the same problem and was never able to figure it out. 2015 "classic" control. Looking forward to an answer.

TeachMePlease said:

Post your code.

Click to expand...

Attached here is about 200 lines of the code while I figure out how to upload a bigger file. Tolerance in Fusion 360 is set at .050 just because I think that's what I was testing in the dry run video I posted.

its in the code,, I do a LOT of 4th axis stuff but its mostly production parts so I hand code all of it ,,if you post up the code we can look into it ,

In Fusion do you have the Manufacturing Extension add on with the Rotary Toolpaths? I thought that was the only way to get simultaneous toolpaths. I had it during the free demo and made some great toolpaths only to have it no longer available without kicking in the $1600 a year. If you know which toolpath to use to get simultaneous 4th without the add-on Rotary package I would love to know.

CNCPleb said:

Attached here is about 200 lines of the code while I figure out how to upload a bigger file. Tolerance in Fusion 360 is set at .050 just because I think that's what I was testing in the dry run video I posted.

Click to expand...

Are you just trying to mill a round cylinder? Or does it have a shape to it? Is that why your Z is moving all over the place?
Does Fusion have a setting where you tell it a max angle change per line or something similar to that nature?

Mtndew said:

Are you just trying to mill a round cylinder? Or does it have a shape to it? Is that why your Z is moving all over the place?
Does Fusion have a setting where you tell it a max angle change per line or something similar to that nature?

Click to expand...

I'm trying to roughly mill a round cylinder with a ball mill using a spiral path. I think there are a bunch of Z moves because the tolerance was .050 and Fusion was interpreting that however it felt like. Even if I lower the tolerance, there will still be Z moves, but they'll be a lot closer. A .0004 tolerance value outputs Z values that only move .0002 or so at a time. I don't think Fusion 360 has any parameter that affects maximum angle change per line.

For what it's worth, someone at the Autodesk forums said to halve the speed. I tried that, and halving the feed from 43 in/min to 21.5 in/min made the toolpath effectively continuous and lowering the tolerance to .01 or .001 effectively made it smooth. It wasn't perfect as there were still slightly different F values and stuff in the code, but it was truly continuous without stopping. Does this mean my machine was just outrunning the program trying to figure out all the code or something?

Jaxian said:

In Fusion do you have the Manufacturing Extension add on with the Rotary Toolpaths? I thought that was the only way to get simultaneous toolpaths. I had it during the free demo and made some great toolpaths only to have it no longer available without kicking in the $1600 a year. If you know which toolpath to use to get simultaneous 4th without the add-on Rotary package I would love to know.

Click to expand...

Sorry, but I'm on a student license because I'm learning machining at a community college. I get unlimited free credits, so I have free access to the manufacturing extension for the Rotary toolpath.

CNCPleb said:

I'm trying to roughly mill a round cylinder with a ball mill using a spiral path. I think there are a bunch of Z moves because the tolerance was .050 and Fusion was interpreting that however it felt like. Even if I lower the tolerance, there will still be Z moves, but they'll be a lot closer. A .0004 tolerance value outputs Z values that only move .0002 or so at a time. I don't think Fusion 360 has any parameter that affects maximum angle change per line.

For what it's worth, someone at the Autodesk forums said to halve the speed. I tried that, and halving the feed from 43 in/min to 21.5 in/min made the toolpath effectively continuous and lowering the tolerance to .01 or .001 effectively made it smooth. It wasn't perfect as there were still slightly different F values and stuff in the code, but it was truly continuous without stopping. Does this mean my machine was just outrunning the program trying to figure out all the code or something?

Click to expand...

What if you were to just hand write a line something like:
G01G93X.05A180.Fxxxxx (whatever feed you need)
G01G93X.1A360.Fxxxx
Is it smooth then?

Mtndew said:

What if you were to just hand write a line something like:
G01G93X.05A180.Fxxxxx (whatever feed you need)
G01G93X.1A360.Fxxxx
Is it smooth then?

Click to expand...

So I wrote this in MDI:

G91
G01 G93 X.05 A180. F22.989
G01 G93 X.1 A180. F22.989
G90 M30

Very roughly 43 ipm assuming a diameter of 1.181 in. like in my program. The machine stopped briefly after running the first G1, and then started the second G1 movement. So the issue must be figuring out each line of code, right? Wrong. I tried writing it with half the feed (F11.495) and the machine ran PERFECTLY SMOOTH. No stops between the G1 movements. Just for GPs, I tried writing this:

G91
G01 G93 X.05 A180. F11.495
G01 G93 X.1 A360. F11.495
G01 G93 X.1 A360. F11.495
G90

First G1 is half feed (roughly 21.5 ipm) and the second and third G1 are roughly the feed I wanted (43 ipm). No stops between first and second G1, stop and start between second and third G1. So, the issue seems to be tied to feed rate or inverse time feed as well as the lines of code, because everything will run smoothly at the higher feed rate if it's one line of code and will run smoothly at the lower feed in spite of many lines of code (like I posted earlier).

Someone at the Autodesk forums mentioned that I should keep the rotary's max speed in mind, but the HRT160 I'm using is capable of 21.6 RPM, which works out to about 80 ipm at the diameter of my part (not including the tool, so my possible feed would be higher). Also, I accidentally programmed a A360. F22.989 line which was twice the feed I wanted, and the rotary ran fine even though that speed was theoretically above it's speed capability according to my math, so it must strictly be a code issue.

Also, a different person at the Autodesk forums suggesting using G187, which is a Haas smoothing function. The code generated a G187 P1 line, which caused my 43 ipm program to have more jerky motions, but the stops and starts were closer together and the rotary stopped/slowed down LESS, meaning the rotary was actually more consistent and closer to continuous despite the additional starts and stops. Just FYI.

Kind of at a loss here. Anyone have any ideas?

Rather than try to figure out the problem you're having with CAM, I'd try hand coding this. I don't remember if I've ever used this example on my Haas mill with a 4th but I've done it on a Fanuc lathe.

It's rather easy to program you just need to do a bit of simple math. From the start point, figure out the total distance you want the tool to travel (ex. 3"). Next, determine how much of a step over you want per A-axis revolution (say .05"). Divide 3" by .05" and you get 60. So the A-axis will turn 60 times to move 3". Now multiply the total number of rotation (60) by 360 (degrees in a circle). You end up with 21,600. This is your H value. Your line of code would look something like this:

G01 X3.0 H21600. FXXX.

You would have to play with the feed to get it right. I'm writing this from home so I'm not able to test it out. Also, you probably have to put one more line with just H360. for the A-axis to make one full rotation without moving in X to make the wall flat since the previous line finished with a helix.

Hopefully this works for you, I'm really curious. Oh, and in case the rotary is turning in the wrong direction (ie, conventional cutting), try making the H value negative. Good luck!

Just checking... I know there are a few post processors for HSM and Haas. Maybe roll back a version or two? Sounds like your commited to the CAM from Autodesk. Also, When we did our post processor for 4/5, there were a number of 'REM' comments in the post processor where you needed to input key values and details. Might be different in your newer PP file than ours.

You noted this page: Where there any issues
The Mill Jerks or Shudders During Simultaneous 4th- or 5th-Axises? Milling | Customer Resource Center

Based on post #12 this isn't a CAM or post issue, it's a machine issue. I found similar results on mine.