Arc point error check - FANUC

[Greg Williams]

Hi Guys,

 

I have a rather fussy FANUC mill that seems to like cutting full circles (inverse result) instead of programmed small sections of large arcs when running dynamic toolpaths. I know that the problem can be fixed by increasing the “Minimum arc length” and the “minimum distance between arc endpoints” in the control def, but to what value? Obviously I could just put 1mm in there and that would work but I am thinking as engineers there must be a better way.

Do you guys have any ideas for a test to determine what value we need to have in the minimum arc length in the control def to stop the full arcs on the machine?

I tried to create one by drawing a Ø100 circle in Mastercam then trimmed the arc back to 0.25mm long which gives me the below code but to no avail as all runs correctly and it cuts the small section. I am guessing there is more than one Parameter on the control to set the value?

G21

G0 G17 G40 G49 G80 G90

T1 M6

G0 G90 G54 X50. Y0. A0. S1000 M3

G43 H1 Z25.

Z10.

G1 Z0. F300.

G3 X49.999 Y.25 I-50. J0. F600. ---------------------- Also tested Y.2, Y0.15, Y0.05

G0 Z25.

M5

G91 G28 Z0.

G28 X0. Y0. A0.

M30

Thanks for your help.

[#Rekd™]

Vericut gives a warning and I alter it. See the attached photo (old photos I kept for reference). I found switching this number from 0.005" to 0.01" makes the warning disappear in Vericut. Also setting the minimum arc length to a 3 digit number like 0.005"

 

The other option is to linearize all of your arcs.

 

 

[gcode]

4 hours ago, Greg Williams said:

I have a rather fussy FANUC mill that seems to like cutting full circle.

There are parameters in the control that set the allowable tolerance for arc endpoints, though it can be a difficult problem to solve.

We had a VTL we bought about 15 years ago that liked to do loops when it got an arc numbers it didn't like.

Opening up the arc endpoint tolerance in the control solved the problem.

Another solution is to take what #Rekd suggested a bit further.

Set your min arc length and radius to something big like .015" / 020.

That way tiny arcs will be linearized and hopefully eliminate this issue.,

[Jasond0530]

Easiest way is just to break arcs. if your control can handle the extra code.

 

[crazy^millman]

Change NC precision in the control definition out to 6 places in inch and 5 places in Metric and see if that helps. There is a major issue with rounding and truncation going on that has been present since X came out. When they allow the NCI to have more than 8 places past the decimal then this issue might finally get resolved. Did this on some HAAS, Mori and few other machines and these arc errors went away on all but one file. That one was not the machine, but the source file. Metric project converted to inch using a post.

[Werktuigbouwer]

In the past we also had this error on one Mori machine. Even after adjusting the settings nothing helped.

Our solution was to add a line to the post:

round_opt$: 21

This changes how the post round the values. Use at you're own risk

[Greg Williams]

Thanks Guys, will run a few test