Earlier today, I was setting up a job I've run several times before. During verification, the first of the two G84's caused the mill to do something I've never seen before. It is probably best explained in this video: "http://www.youtube.com/watch?v=034I-YXibOc"]YouTube - Crazy G84
In the video, rapids were set at 25%. If they are at 5%, the 'bouncing' is less severe and slower; at 50%, it is more severe and faster. I didn't even want to try 100%.
I tracked the problem down to the "RAPID -> HS FEED" parameter. I changed it to "1" a while back to use interpolated rapids instead of dogleg rapids. When I changed "RAPID -> HS FEED" back to "0", the problem dissappeared.
My mill is a 2007 MiniMill, with a version 14.04C controller.
Here is the portion of code:
Has anyone else come across this problem before? Is there anything that Haas will do for an out-of-warranty machine with a bug? I would really like to use interpolated rapids because it allows me to take full advantage of my CAM software (ProNC) and minimizes one potential source for crashes.
For now, I will switch "RAPID -> HS FEED" off every time I want to use G84, but that is not a long term solution for me. If I forget to turn it off, G84 will cause a crash. If I forget to turn if on, the dogleg rapids could cause a crash. Damned if I do, damned if I don't...
Thanks in advance,
It is difficult to tell from a video but your spindle seemed to be running fairly slow; what was your rpm?
I have found that when something like 100 or 200 rpm is used for rigid tapping the spindle speed does not settle down. How this could interact with the feed I do not know but if you are going slow try speeding up and see what happens...several inches above the part.
An open mind is a virtue...so long as all the common sense has not leaked out.
Spindle speed is at 1500 rpm.
Looks to me like you didn't cancel the drill cycle (that I assume preceded the tapping cycle)..I see no G80..but I can't see the entire program..Just what I would guess..
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
On the line preceeding the toolchange, I have a G80.
Initially, I thought that I had somehow changed the G84 to a G83. Or even peck tapping. But if you watch the video closely, you can see the tool pecks down and then pecks up. Also, the depth that it goes to is not the Z-.35 that I commanded; it is more than that. When the rapids are set to 50%, it goes even deeper.
Lemme' ask you a stupid question: have you copied the program and deleted everything before and after that part, then tried it (tapping air)?
I'd approach it systematically. If deleting everything else fixes it, then the problem is elsewhere.
If not, I'd delete the second hole location and try it.
If that didn't work, I'd try changing the feed or RPM.
You'll eventually get to something that makes it not do that. At that point, you can work backward to a solution.
Could this be something between the retract plane and some retract setting elsewhere in the control? I'm not in front of my machine right now but I wonder if some really large retract distance in the settings might be conflicting with the retract plane in G84.
I too thought it might be a certain combination of parameters that was causing this behaviour, so I tried the following:
- faster/slower rpm
- faster/slower feed
- starting on the same tool
- starting with a tool change
- rapids at 5%, 25%, and 50% (not brave enough to try 100%)
- G84 as part of the main program
- G84 as part of short program (set speed, feed, then G84 X_ Y_ Z_ R_)
- G84 in MDI
- coolant on/off
- one hole/lots of holes (first hole is always bad, remaining are not)
- tool length offset/no tool length offset
- starting at retract plane/starting above retract plane
- and a few more that I can't recall off the top of my head
Unfortunately, the only thing that removed the problem was turning off "RAPID -> HS FEED".
I plan to call my HFO and/or Haas Help Desk on Monday.
Try turning setting 133 OFF. Haas told me this sometimes causes problems.
Repeat rigid tap is not on.
The Haas factory has confirmed that, on older controllers, interpolated rapids (i.e. RAPID -> HS FEED set to 1) can not be used with canned cycles (G81, G82, G83, etc.).
Only the newest control (software v16) can have interpolated rapids on all the time. Previous versions were just not designed to do so; the only commands that should be used are G00, G01, G02, and G03.