1994 VF3 over-travel or position problem?

Hi all,

I ran a few dozen 6061 parts on a new to me 1994 vf3 last week and I was having trouble with the x or y axes over traveling on higher feed rates. I had a trapezoid shaped pocket with acute angles in the corners and roughed it out with a 3/4 end mill, then cleaned up the corners with a 1/2, first by taking .2 doc climb cuts at 125 ipm just in the corners, then finishing it with the 1/2, .005 cleanup full depth (1.6in). By feed holding after each op i narrowed the problem to the corners during the .2 doc cuts, it would leave .025 or so deep gouges at the end of travel. When I single blocked through it was fine, and changing the feed to 40ipm fixed it.

I thought it might be cutter deflection, but it was at the end of travel where the tool was cutting air and it did the same thing cutting polyurethane foam.

Also, backlash measures under .0005 with an indicator, although I measured it in a relatively unscientific way without any load.

I searched the forums a bunch and there was talk of a parameter for maximum corner rounding but I think my machine does not have that, all I can find are servo parameters that I am hesitant to mess with.

All other tool path seemed ok, I ran the 3/4 at 80-100 ipm. Also, I re made the tool path in sprut cam with circular lead in and lead out and it still left a big mark at the end with high feed rates ( well higher, anything over 40).

One thing I noticed was a little groaning/ buzzing of I think the x while stationary. Loading the axis a bit by pushing on the table quiets things. Seems to just be dithering a bit between encoder counts, probably not a big deal.

I've gotten some feedback on other forums basically saying that old Haas machines just can't cut accurately above 75ipm. Anybody with a 94' vintage machine have a good idea of how fast I can run the feed and expect +/-.005?

Ideas? Thanks!

Are you doing straight line cuts in the corners? If so, you could program an arc in the corners, and it might cut smoother. If that leaves too much stock for your finisher you could use your 1/2" rougher and plunge each corner to leave less stock for the finisher.

Two of the machines in our shop are early 90's Haas's, and we can cut +/-.002 on them without a whole lot of trouble. Never really had any problems on them. I wouldn't run a rougher any faster than 60-80 ipms and would finish any faster than 30-40 ips on one though.

Hi Brian,

Thanks for the post. I am running a small arc in the corners, about .05r or so. I am plunging in with the 1/2, leaving .01 stock. I improved things a lot by messing with the accel and timing parameters for X and Y, they were set quite low and the combination sets a threshold where over a certain feedrate the control treats things as a rapid move. Once I set these parameters things were way better, while it did not cut perfect corners on the roughing passes at 100IPM, the .010 stock I left was plenty to clean up the error with a finish pass. This is totally acceptable to me, and probably will not push the parameters further. Once I have a little time I will put the actual parameters I am using up here and see if anyone knows any down side to having them set to where I do.

Also, the program is attached.

Thanks,
Dustin

So I called Haas and they do not have a servo tuning procedure. I have been studying the manual and in the parameter description section parameter 113 "X acc/dec t const" there is a description of how this works with parameter 7 "acceleration" to define the maximum accurate feedrate. The numbers in this explanation did not match the numbers in the control, and if I plugged the numbers from the control into the equation I came up with 66.4ipm as the maximum accurate profiling feedrate. With the numbers in the example you get 159ipm.

Parameter in control-
7- 1,000,000
113- 375
21- 1,000,000
114- 375

Set to-
7- 1,200,000
113- 750
21- 1,200,000
114- 750

So I hit the e-stop and reset these parameters for X and Y. With these parameters the part cuts great at 100ipm. The corners are not perfect on the roughing passes but the .010 stock I leave before the finish is plenty to clean it up, and it is WAY better.

Also, I ran the program at feedrates just above and just below the cutoff of 66.4ipm (with the old parameters) and you can see the difference with it just cutting air, it decelerates slightly as it gets to the corners and sounds smooth with the feed below, and if you go above it does not do this and and there is more vibration and "drumming" of the sheet metal.

I thought this might be related to setting 44 "min F in radius CC" after talking to a haas engineer but is acts the same regardless of whether or not cutter comp is on. The Haas guy said that this slows the feed in every g02-g03 move with cutter comp on but reading the manual it seems only to slow it down on certain approaches, not sure what it does. The program runs the same with cutter comp on or off.

Basically I am happy with how it is running now, I can program 100ipm without worrying about gouging things. But it would be great to know more about how these parameters and settings work, anybody have details?

Thanks