Arc error in Vericut

[Bob W.]

I keep getting this warning in Vericut when running a simulation

 

"Arc start and end points might produce undesired motion in Fanuc controls"

 

Any idea what might be causing this and how I can go about fixing it?

 

Thanks,

Bob

[Mick]

I've never seen this warning before. What are the settings for the Circle tab under G-code settings?

[Bob W.]

Circle center mode = incremental

Method = from start to center

Pitch specified with IJK = No

Output for circular motion = circle

[Guyinthedesert]

I keep getting this warning in Vericut when running a simulation

 

"Arc start and end points might produce undesired motion in Fanuc controls"

 

Any idea what might be causing this and how I can go about fixing it?

 

Thanks,

Bob

Are the start and end points too close together?

[gcode]

could you be turning on CDC with an arc move??

[Bob W.]

Here is the code. The warning is generated by the middle line and there are probably a few dozen of these warnings in my NC file

 

G3 X4.6713 Y-6.3732 Z14.797 I.2889 J-.4733
X4.4291 Y-6.9801 I1.0686 J-.7783
X4.6703 Y-7.9442 I1.2378 J-.2026

[gcode]

the first line has a Z move with no K

if there really is no Z motion, try adding a K0 to see if the alarm goes away

[Mick]

Circle center mode = incremental

Method = from start to center

Pitch specified with IJK = No

Output for circular motion = circle

 

They're the same settings as mine (Okuma control, but the control file was based on a Fanuc).

 

Try putting a G3 on the lines that don't have it (in case it is some kind of modal thing not set in Vericut).

[Bob W.]

the first line has a Z move with no K

if there really is no Z motion, try adding a K0 to see if the alarm goes away

 

I am currently reposting. Is there a mod that I can do in my Mastercam control definition or post to fix this?

[Guyinthedesert]

Here is the code. The warning is generated by the middle line and there are probably a few dozen of these warnings in my NC file

 

G3 X4.6713 Y-6.3732 Z14.797 I.2889 J-.4733
X4.4291 Y-6.9801 I1.0686 J-.7783
X4.6703 Y-7.9442 I1.2378 J-.2026

 

Do you have a G17 active?

[Bob W.]

Do you have a G17 active?

 

Yes, G17 is active. It appears to be related to the Z value without any K value. Any ideas where I need to look to remedy this?

[Mick]

Z needs K? Not if it is a helix. Z would need a K value if the arc is in a XZ or YZ plane wouldn't it?

[Watcher]

Bob, what version are you using....

 

I suppose 7.2.3? If so, try this: (But first try to understand if this warning is not helping you before you disable it - Read the info below)

 

Try this:

 

[Watcher]

Do you have a G17 active?

Here is the code. The warning is generated by the middle line and there are probably a few dozen of these warnings in my NC file

 

G3 X4.6713 Y-6.3732 Z14.797 I.2889 J-.4733
X4.4291 Y-6.9801 I1.0686 J-.7783
X4.6703 Y-7.9442 I1.2378 J-.2026

 

Can I have the block before the 1st G3 so I can test my solution for you?

[MrFish]

Had this error even on our Heidenhain post after upgrading to Vericut 7.2.3 - CG tech tech support sorted it out with a new control def .xctl file

[Watcher]

Had this error even on our Heidenhain post after upgrading to Vericut 7.2.3 - CG tech tech support sorted it out with a new control def .xctl file

 

7.2.3 has a bug interpreting some arcs.

 

They sent me 7.2.4 pre-release. Problem solved.

 

Perhaps your problem was solved with the solution above, which is not intended to fix a bug, it's the software functionality to prevent gouges that VERICUT could not detect before because of FANUC changes between FS15 and FS16. When that is the case, the warning can be eliminated with a change in the control.

 

My problem with arcs was really a bug introduced in 7.2.3. The error does not occur in 7.2.1.

[Bob W.]

Watcher, thanks a ton for that information. Sounds like that is what the issue is.

[Colin Gilchrist]

Hi Bob,

 

Can you also send me a snippet of the code a couple lines before and after the issue? Have you tried plotting the gcode values in Mastercam to see what the size of the arcs are? You can adjust the min/max arc sizes in both the Toolpath filter settings, and in the Control Definition tolerance pages. Anything below that threshold should get linearized.

 

There are some filter settings that you can use to linearize the entire path as well. This can be useful on some machines if you are using the machine's high speed control functions.

[Bob W.]

Here is some code. The issue is on line 5.

 

 

X5.7386 Y-1.315 I-.0236 J-.1654
G1 X5.73858 Y-1.32771 Z15.16421
X5.73853 Y-1.55203
X5.73854 Y-1.55293
G2 X5.7385 Y-1.5538 Z15.1642 I-.169 J-.0025
G3 X5.7866 Y-1.612 I.06 J.0006
G2 X5.8345 Y-1.6288 I-.0437 J-.2015
G3 X5.8472 Y-1.6302 I.013 J.0586
X5.8532 Y-1.6243 J.006