Haas 4 axis - controller displays rapid on a feed move - CNCzone.com-The Largest Machinist Community on the net!

jimcooptcam77 · #1 02-15-2011, 01:45 PM

I am having some surface finish problems when cutting with simultaneous 4 axis. I noticed that when there is a lot of rotary motion in my program the controller flashes between feed and rapid on the display, but each line of code has a given feed rate, there is no G00 call.

Anyone have any ideas on this?

KenFoulks · #2 02-15-2011, 03:16 PM

Are you using inverse time?

jimcooptcam77 · #3 02-15-2011, 03:20 PM

Yes, G93. But even when turning that off, it still shows the same thing.

thanks for the reply,

Jim

KenFoulks · #4 02-15-2011, 03:24 PM

Is HSM enabled?

jimcooptcam77 · #5 02-15-2011, 03:33 PM

Yes

thanks,

Jim

ToyMaker94566 · #6 02-15-2011, 07:59 PM

Did you tell the control what diameter you are working at so the feed can be correctly calculated? I believe the diameter call out is the next parameter below "4th axis enable"....

jimcooptcam77 · #7 02-16-2011, 08:01 AM

Yes, the diameter has been set.

As a result of another error, i had to restart the control. The rapid/feed display seems to be solved by the reboot. I am still having finishing problems, but that doesn't seem to be related.

thanks for all the posts in reply!
Jim

Wizzard of H · #8 02-16-2011, 12:09 PM

What you are seeing is an efect of mixing linear and rotary motion with high speed machining option. it is not a problem. It just indicates that the rotary axes had to slow down when getting near the end of a stroke to insure machine stays accurate.

jimcooptcam77 · #9 02-17-2011, 02:46 PM

That's very interesting. I'm doing some tests that show just that. The rotary is ahead of the linear axis on each move, but I'm starting to think it is a problem.

Anyone found a way to tune the rotary axis to the linear?

Wizzard of H · #10 02-17-2011, 03:33 PM

Check that parameters 786, 787, 788, and 789 are all the same value. If you have them, they are probably set to 64 but they all need to be the same.

jimcooptcam77 · #11 02-18-2011, 09:38 AM

Wizard of H - cannot thank you enough....and Haas should thank you too. Seems they've shipped their version 17.03 software machines with the linear FIR's set to 64 and the Rotary FIR's set to 0. Linear and Rotary axis are tracking much better now with both set to 64.

thanks so much,

Jim

Thread Tools	Search this Thread
Show Printable Version Email this Page	Search this Thread: Advanced Search
Display Modes
Linear Mode Switch to Hybrid Mode Switch to Threaded Mode

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Okuma mill feed rate jumps to rapid feed	easyguy97	Okuma	6	12-20-2009 04:14 AM
Rapid move axis control	mattpatt	SolidCam	3	08-15-2008 09:51 AM
Haas rapid move ?	binzer	Haas Mills	2	06-28-2007 07:11 PM
Crash during Z rapid move	AndyB	Fadal	1	03-07-2007 08:48 AM
Axis move during feed hold	1ctoolfool	Haas Mills	3	09-12-2006 10:12 AM

Currently Active Users Viewing This Thread: 1 (0 members and 1 guests)