HPCC and toolpath filtering

[?Mark]

Looks like toolpath filtering using arcs doesn't play well when running HPCC. I get either illegal arc or plane error, not always but often enough for me to start considering not using toolpath filters.

Do you turn filtering completely off when using HPCC or just arcs?

Am I missing something here?

 

TIA

[Tony35]

i stopped using a big tolerance (.015+) in the arc filter when in HPCC it was banging the ballscrews to much

my filter is set to a total tol. of .001 now or i just use points for SGI on the makinos

 

i have never had any of those alarms

[friggenbozo!]

Looks like toolpath filtering using arcs doesn't play well when running HPCC. I get either illegal arc or plane error, not always but often enough for me to start considering not using toolpath filters.

Do you turn filtering completely off when using HPCC or just arcs?

Am I missing something here?

 

TIA

 

 

there's 3 arc filters, dont check on the lower 2...filtering in g18,g19. Only use the G17 filter(x-y plane, the top one. Might be your problem.

[Guest CNC Apps Guy 1]

Don't allow out of top plane arcs and you shoudl be good. I usually set my tolerances to .0025 to .0015 when roughing and .001 or better when finishing. Usually around .0008.

 

HTH

[?Mark]

What surprised me is that unchecking the the xz and yz arcs didn't make much of the difference. I had to uncheck all three to get rid of alarms on some occasions. I don't think the total tolerance really matters here, but I never ever go more that .005 and that is for a large tool surface roughing thru material at 305+ ipm.

Which brings me to assume that what Tony does might be a key, points only and no arcs...

 

Thanks all <cheers>

[?Mark]

HPCC doesn't like arcs period when in ramping.

 

Sample:

G2 X2.2355 Y-6.2702 Z9.0857 I-1.2401 J-.8966 (gives an alarm in xy plane)

[Tony35]

odd

i run HPCC all the time for any milling etc (thanks to cnc apps guy1)

i never have had an alarm even when ramping

might have to tweak some arc tol. parameters in the control

 

just a thought

[NOTW Programmer]

I ramp down on all my HPCC paths and have never had this issue. The only time I did have it was while using the Volumill add-in; it created an arc so small that the machine control could not make the move, it was a clearance move to return to the begining of the cut. I set my tolerances to a 2:1 cut tol. .001 that always seems to work.

[Cannon]

Same thing in our fanuc 18i with HPCC, no ramping arc moves or we get alarm. Fanuc guy said it is an option that the MTB did not get.

[?Mark]

Funny, just this minute I found out the same thing from our maintenance guys after they talked to fanuc. (there is hpcc and there is hpcc with helical motions)

I'll ask for a quote to have it added to our 3 niigatas.

<cheers>

[Tony35]

ahh helical interpolation yes that is an option

[Guest CNC Apps Guy 1]

It's crazy that it's an option. Blame the builder, it's not like FANUC is hiding anything.

[MIL-TFP-41]

Everything...and I mean EVERYTHING is an option for Fanuc. MTB's should be wise to this...and include things like this.