Choppy transition moves

[Sigurd]

I'm using Mastercam 2021 and a Haas Minimill 2. I've programmed a Hybrid toolpath with arc filter turned on, .0004 total, 2:1 ratio of cut to line, G17/G18/G19 all checked, "Output 3D arc motion" checked, and I'm still getting tons of G1 motion both in the cut and also in the transition moves. I have Minimum Distance checked and also output feed move checked. The machine just bumps and chokes on all the line moves it generates. Am I missing something else? It's just not smooth at all.

[Jobnt]

Are you machining a spline or an arc?

[Sigurd]

It's a solid body. There's no wireframe. I just want everything to get turned into arc moves. 

[Leon82]

Do you have the filter turned on to make arcs in x and y?

It's possible that controlled definition is forcing linear moves

[Sigurd]

Yes, I have all three (G17, G18, and G19) turned on.

[Jobnt]

59 minutes ago, Sigurd said:

It's a solid body. There's no wireframe. I just want everything to get turned into arc moves. 

I'm not sure we have that kind of control with solids but it may be something in the CD?

You could try putting an arc on one of the edges and machine that and see if it puts out arcs. 

[cruzila]

HAAS G187 SETTING

[JParis]

The big questions is this...are those moves taking place in a G17,G18 or G19 plane...if they are not, you won't get arc motion

[Jobnt]

3 minutes ago, cruzila said:

HAAS G187 SETTING

That doesn't create arcs from lines it smooths the transition between the lines by sacrificing accuracy. 

[motor-vater]

I see the same behavior on our haas's all the time. I could say some not nice things about the machines but I wont. Hopefully you can use the G187 setting as mentioned above, Our machines just alarm out when I tried so I have to assume its a paid add on that we opted out of. If that doesn't work you are gonna need to play with your tolerance .0004 os pretty tight for a haas, creates alot of code and the control will chock on it.

[gcode]

How old is the machine??

Older Haas controls cannot handle a bunch of point to point code without choking.

Mastercam high speed toolpaths are going to output point to point code, especially in transition moves

no matter what settings you have on the filter page.

Personally I think a .0004 setting on the filter is way too tight for what you are doing.

I'd bump it up to .001 or .002 and see if the machine can handle the code better.

 

[Sigurd]

6 hours ago, JParis said:

The big questions is this...are those moves taking place in a G17,G18 or G19 plane...if they are not, you won't get arc motion

I would assume so, right? If I check all three, that's all three planes, XY, XZ, and YZ. Is that how it works out am I missing something?

6 hours ago, motor-vater said:

I see the same behavior on our haas's all the time. I could say some not nice things about the machines but I wont. Hopefully you can use the G187 setting as mentioned above, Our machines just alarm out when I tried so I have to assume its a paid add on that we opted out of. If that doesn't work you are gonna need to play with your tolerance .0004 os pretty tight for a haas, creates alot of code and the control will chock on it.

I will try different values for G187. I had forgotten about that.

5 hours ago, gcode said:

How old is the machine??

Older Haas controls cannot handle a bunch of point to point code without choking.

Mastercam high speed toolpaths are going to output point to point code, especially in transition moves

no matter what settings you have on the filter page.

Personally I think a .0004 setting on the filter is way too tight for what you are doing.

I'd bump it up to .001 or .002 and see in the machine can handle the code better.

 

It's a 2020. I'll loosen the tolerance and try again.

[gcode]

Here are a couple of youtube videos on filtering

 

 

 

[Sigurd]

Thanks. I'll watch them when I get a chance.

 

I did loosen my tolerance to .001 on another part yesterday and that seemed to improve things. I'll have to apply it to my problem toolpath next time it comes up.

[gcode]

Maybe high speed toolpaths should have 2 sets of tolerances.

One for the machining motion and a second for linking motion???

[Sigurd]

It would be nice. I've noticed that on OptiRough and Area Rough where the cutting motion is fine, but the transition/linking motion shakes the machine.

[motor-vater]

3 hours ago, Sigurd said:

It would be nice. I've noticed that on OptiRough and Area Rough where the cutting motion is fine, but the transition/linking motion shakes the machine.

Possible from linking motion being speed up? chocking on code?

[Jobnt]

3 hours ago, gcode said:

Maybe high speed toolpaths should have 2 sets of tolerances.

One for the machining motion and a second for linking motion???

Interesting concept...

[Kyle F]

18 minutes ago, motor-vater said:

Possible from linking motion being speed up? chocking on code?

that's my best guess.. with a total filter tolerance of .0004 paired with the fact he's outputting G0 as G1. I think even the haas NGC can't handle more than 1000 lines per second, hard to know without looking at his program but if he set that parameter to something like F500. maybe those rapid-to-feed moves are spitting too many lines.

I'm curious why OP has that output to feed checked,.. If it's to negate any doglegging when paired with the "minimum distance" on clearances... I'd try unchecking output to feed and setting full clearance at like .5 above the part and see if actually using G0 rapid helps with the jerky movement in transitions.

 

EDIT: now that I'm thinking more on it, a 2020 haas shouldn't dogleg rapid movements.. Only seen that on the older models

[gms1]

6 hours ago, gcode said:

Maybe high speed toolpaths should have 2 sets of tolerances.

One for the machining motion and a second for linking motion???

Half the time the linking motion doesn't even work anyway.