Official Luthiers Forum!

I've noticed on my Haas machines I get a segmented curve out at the machine rather than a nice, smooth edge....only on complex curves. This happens regardless of whether I tell MasterCam to generate arcs or line segments on contoured splines. This leaves an unsightly edge on a body which must be hand sanded and and can take a great deal of time to get smooth.

When discussing this with the fellows at Mastercam they said sometimes the controllers of certain machines respond better to I,J,K arcs in the g-code rather than R commands. I edited my post processor to do this but haven't tried it yet. I hope that works but I'm dubious. The machine can't properly process R commands? That hardly seems likely.

I'm curious if anyone else has found their machines prefer I,J,K over R commands. ??

_________________
I read Emerson on the can. A foolish consistency is the hobgoblin of little minds...true...but a consistent reading of Emerson has its uses nevertheless.

StuMusic

I can't answer your question directly as I've never tried R mode but by default, Mach 3 uses I,J,K and my arcs definitely come out nicely.

Sounds like you have this covered already but, VisualMill by default came set to output arcs as line segments - lot's of people using VM had issues with that so I actually fixed that right off the bat.

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com

I'm not a mastercam user, but it there should be a parameter somewhere in there that's sets the cordal tolerance. Back in my APT days its was "intol/outtol". Maybe that would help.

_________________
Jim Watts
http://jameswattsguitars.com

My friends Hurco does not work well in Radius mode but works fine in IJK mode.

MK

_________________
I'm outside looking in, just farther from the window than most.

Mastercam X5 not only has the ability to generate arc segments along a spline but you can also set a chordal tolerance for where they meet. I've set them to the finest possible settings and still get the same result. That's not it. Looking at the graphic display AND looking over the g-code you can see that G02's and G03's ARE being generated along the spline geometry on a contour operation...which indicates that this "segmenting" phenomenon MUST be happening out at the controller. It doesn't make much sense to me that a world class, brand name controller doesn't interpolate arcs smoothly via the R command.

Kinda baffles me really.

_________________
I read Emerson on the can. A foolish consistency is the hobgoblin of little minds...true...but a consistent reading of Emerson has its uses nevertheless.

StuMusic

Run a really low feed test to see if it's possibly the control interpolation or mechanical. If they go away then it's the loop.
Run the same test with a rotation on the part of 30-45 degrees and see if the marks line up, if they're the same then it's not mechanical.

If the marks stay consistent on the angle test and at low feed, then it's the interpolation on the control or the CAM output
If the marks go away at lower feeds and stay the same at an angle then it's the loop (low level motor control)
If the marks are different at an angle then it's mechanical

If it's the interpolation then maybe changing arc standards will work, but that sounds dubious to me, too. If you divvy your code into 0.003" line segments then run it at low feed it'd be a good comparison.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

As always, I agree with Bob

I've seen this pop up as a control issue. If this is what it is, and you run the program slowly, these artifacts should disappear.

This was one of the reasons why we decided to stay with FADAL's at PRS - the mid priced CNC routers all seemed to do this. The FADAL was the best buy in terms of $/feed rate while maintaining carve accuracy.

Trev

_________________
http://www.PeakeGuitars.com

OFF TOPIC SOME: Andy, FYI ,Mach3 also has a plasma setting in the general config. I have used with this function many many times to smooth out the arcs even better than Incremental IJK and or absolute IJK, constant velocity mode . Just for fun sometime try a test in air in cutting arcs with plasma on and with plasma off added to your normal settings. Mach 3 has an algorithm that smooths the interpolated segments further to keep a plasma cutter from stopping and blowing out and causing a jagged cut. It's an interesting test to say the least. I use it on most carves now.

MK

_________________
I'm outside looking in, just farther from the window than most.

Probably even better $ / IPM now...I sold mine for 9K with ten tool holders. You need to have a tech, though, now that the company's gone.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

check setting 85 "contour tolerance" in your control. default is .05 which is too much for those who want good finishes. decrease by half and try again. don't go down to 0 or you will choke the machine servos.

use r values for arc generation. your x5 post should default to 180 degrees and this is fine. i, j, k, are unnecessary in the haas control unless you are doing helical interpolation and are using sub routines which i generally mdi anyway.

I find that IJK is usually the best. When Writing G code by hand the R makes the process a little simpler especially when figuring geometry with a calculator.

That said I tend to use IJK when possible. If using software I see absolutely no reason for using an R. You have an expensive computer and program there that is designed for doing this sort of geometry why would you let it "cut corners"?

Also like mentioned above if it's a control issue slowing it down will help it move more fluently in and out of the arcs preventing the machine from having to slow to figure its next move.

Hope that is helpful.

By the way is it an old haas? I know on my '95 and '97 model vf0 machines they can have some issues with that running through a lot of code really fast. The control gets overworked. Though on my '04 '07 '10 '12 models I have no issues with control lag at all. So if it's an old machine you may want to use IJK and simplify the code as much as possible. Go in and take out any repetitive codes that are uneccesary. CAM programs have a tendency to be quite redundant and activate codes that are already active and not needed which can bog down controls on old machines.

I've had some issues with Mach3 getting lost when running I, J K code.

My 95 Fadal wont work with any form of arc. Everything has to be line segments. I e gone through all of the machine settings and they are correct so I'm thinking it could be a setting in the DNC software but haven't had time to chase it down. Thanks for sharing the information. Sorry to derail.

Which control is on it? It could be your post if it's newer than an 88HS -4, that's what was in my '94 and it handled arcs fine.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

Anyway...it hasn't been until today that I actually got a chance to revisit this issue.

I first checked out parameter 85 and found that the default was .025" so I left that alone. The machine is a 2008 Haas TM-3.

Running with I.J.K code completely resolved the issue. Nice, smooth arcs now.

I'll just run around the edge and finish with a 3/4" four flute emdmill and I think I'll be able to start finish sanding at 400.

Thanks for your help guys!!

_________________
I read Emerson on the can. A foolish consistency is the hobgoblin of little minds...true...but a consistent reading of Emerson has its uses nevertheless.

StuMusic

Hmmmmmmmmm Ive never seen an issue like that on a model that new! Kinda makes me worry. You may want to contact your local HFO and see if they have any ideas about it. But then again if IJK work you may just want to not worry about it. Glad you got her figured out. Make some chips!