Optirough Setting for axis 'bang'

[Newbeeee™]

Hi All,

Just running an optirough toolpath, and the machine 'booms' as the tool feeds out of cut / off the part, and goes into max feedrate shooting around the profile to start it's next cut again.

I have 10% toolpath radius set, which is smooth for the majority of the part, but in backplot it doesn't look like it has much affect to the 'problem' area.

I have just upped the Arc Filter Total tolerance (currently set at our normal default of 0.02 (metric)), and this doesn't seem to do much to the backplot either.

I have 'create arcs XY' selected, and what does seem to make a difference (in backplot as this is a one off and I can't be arsed to re-post ) is'Tighten arc filter tolerance'.

 

So does anyone else have any axis banging with the HSS paths, and what do you look to do/change to stop it happening?

Cheers

[Brando]

there are usually two things that cause that, one the machine cant process the g code into motion fast enough, or the acc dec settings are not set correctly in the machine parameters,

to suppress this at the machine , most controllers have high speed g codes that enable the cnc to smoothly accelerate and decelerate at high feed rates

what kind of machine controller are you using? fanuc mazak etc? either way theres info about it in the users manual

 

in mastercam this is what i use for older machines

 

total tol set to .003in

 

then in refine toolpath window

 

ncprgm length + short

surface quality + good

calc time + normal

 

line arc filter checked

smoothing not checked

 

xy xz yz all checked

one way not checked

and maximal tol val for both

minimum arc .005 in

max arc 100. in

[tonyjohnson]

I have the same problem with small arcs.I had to set my post to (points only for 3d work).My dealer recommended this and the problem was solved.Sadly code is much longer.Certainly try above first.

[Guest CNC Apps Guy 1]

Remember also, make sure to have your machine's high speed processing active. This will tend to smooth things out as well.

[Newbeeee™]

Thanks all.

It's happening on our Chevalier VMC (fanuc 0imc - yr 2005). The acc/dec parameters we have tweaked to pretty optimal for these machines.

We're running G05.1 which is only basic lookahead on these machines as they are fanuc package B.

We have arc settings set to shorten code and to (I thought) smooth out. Interesting that the G1's actually process smoother.

Looking at the backplot in NCPlot, the point it made the 'bang' was a sequence of X***R*** lines. There were about 4 in a row where the radii ran from one to the next to the next, and it was either this whole sequence or just the one line that the machine didn't agree with.

The rest of the program ran fine and the job is done, but where this toolpath was repeated for 3 levels (as it was stepping down), it boomed on each pass at the same point (code obviously being identical except for the Z depth).

I'll have a look in the paramters when at work and see how they differ from Brandou's.

Cheers

[NOTW Programmer]

Thanks all.

It's happening on our Chevalier VMC (fanuc 0imc - yr 2005). The acc/dec parameters we have tweaked to pretty optimal for these machines.

We're running G05.1 which is only basic lookahead on these machines as they are fanuc package B.

We have arc settings set to shorten code and to (I thought) smooth out. Interesting that the G1's actually process smoother......

Cheers

We have FADAL6030 VMCs, I run SS304 running at 100IPM. These machines are not meant to do these HSM toolpaths, there is certainly no banging, I have filters set as above, however I do not set backfeed any higher than the cut feed; that way the servo does not have to slow down or speed up.

[Newbeeee™]

Brandou:-

Just checked my settings (really just the default for us)

 

Total tolerance 0.02mm

 

Refine toolpath

short>good>normal (same as yours)

Line arc filter checked (same)

Smoothing not checked (same)

Create arcs in XY checked

XZ and YZ not checked

Maximal tolerance for both checked (same)

Min arc radius 0.1 (metric)

Max arc radius 10000 (metric)

 

So all in all, very similar to yours.

 

Greyman:-

We're running F10000 (max G1 for the machine) for feedback.

For running this one off, I had the feed at 50% when I knew it would do it and all was much better.

So if I had it set at return feed=cut feed, it probably would have been ok for this instance.

 

That said, on ally we're cutting at F7000 so it wouldn't have helped here.

 

Can anyone from CNC advise on this?

Is there any pearls of wisdom we're missing?

Any 'top tips'?

Cheers

[Cannon]

We're running G05.1 which is only basic lookahead on these machines as they are fanuc package B.

 

There is different settings for this G05.1 look ahead, Q1. - Q10. If they are set up in the control, you get different "tightness" of look ahead.

[Chris Rizzo]

sequence of X***R*** lines.

 

You running R's? Try the same sequence in IJK's?

 

Just a random though and another straw to grasp at

 

 

(However that would be more data for the control, but g5.1 should be fine I suppose....:/)

[Guest CNC Apps Guy 1]

All in all, this is a machine/control issue.

 

You may want to change the acc/dec parameters. They come set from the factory with generec numbers. There's probably a dozen or so parameters related to how soon acc/dec happens before/after interpolation.

 

It does take some time to work out. BUt it's wirth the time. I think I did a Toyoda VMC in about 2 hours, maybe 3.

[Newbeeee™]

James,

You're right ref it being a machine issue. I know which ones to tweak (there's only the 2) but wanted to avoid it as the 3x machines work sweet. It's just the occasional line and it's always on back feed, when the tool XY retracts half a millimetre (ish) from the contour and shoots off at the speed of light.

When it's cutting, even at 7metre feeds we haven't had any banging.

 

Ref Tony's post above, why would G1's process smoother? I would have asumed that the less code, the smoother the processing?

Short moves = stop start or juddery motion?

Just my ignorance...

 

Chris - I have thought about changing the post to IJK ref other threads here saying how R's are bad.

Just that we have never had an issue and if it aint broke...

 

Edit:- Something just come up in the bath

James, is there a min and a max arc setting in the machines? I wouldn't have thought it's a problem with what the operation config is set at, and I'll have a look at work tomorrow to see exactly what the rad sizes where that were causing the bang.

But just wondering.

[Guest CNC Apps Guy 1]

I cannot find a max arc setting BUT, there is a max feedrate for arc radius R (#1730), related... (#1731 and #1732)

[Newbeeee™]

Thanks James - I'll have a look and report back

[Newbeeee™]

Well the code was all G3 arcs, R20 into R6723 into R2533 (metric).

The 1730 max feed for arc radius parameter is set at 4500.

So, perhaps the G1 high feed return is F1000 and then into F4500 and then back upto F1000?

Which is why Tony has G1's - it all then runs at the 1x feedrate.

I really don't want to change the 1730 as the machine is accurate at high (ish - all things are realative on a 10k spindle machine) feeds. If I raise this to 10000 (to match the high back feedrate), the machine may not be accurate when interpolating or profiling.

So it may be G1's...

 

Tony - have you any specific settings which work for you?

 

Thanks all