problem with mill volume sequence that will cause my cnc machine to crash.
Good morning guys,
I ran into this problem last month and finally narrowed it down to the culprit. I was programming a huge compression mold and used a mill volume sequence with a mill window. Usually when I am machining a pocket I would just use scan_type=type_spiral and the program would be fine. This time I had a big 2" inserted cutter and on a previous job I was plugging the middle of the tool when the toolpath would start with a small circle in the middle of the mill window. So I started to play around with the scan type to help with the plugging issue. I found the spiral_maintain_cut_direction to work much better on the play path and thru vericut. So I used it on the program and it was working fine on the machine until 1" into the part the CNC code programmed a large radius that violated the mill window and basically sent the tool 200" ipm into the material 1" deep. Also mowed off the boss feature inside the cavity the sight was not pretty. Blew up the spindle head. I thought it was a machine problem at first because playpath and vericut did not show that move. So got the machine repaired and rerun slowly at that area of the code and then saw the problem. The code was telling the tool to wipe out the boss and go outside the window at the 1" deep depth. Ran the program thru another backplotter and saw the problem again. Next thing was maybe it was the post but talked to the post builder and even used the default 4 axis posts from Gpost and I would still get bad code. We analyze the .ncl and .acl file and see the bad data from ProE. Turned it into PTC but so far no resolution to the problem. So now I am really leery to try other functions in ProMAN. I wanted to see if anybody else out there has used that scan type option and not run into any problems.
Oh I am on WF4.0 M180
Great Plains Mfg.
108 W. 2nd Street
Assaria, KS. 67416
785-667-7763 ext. 3477
This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.
I have seen this before. My work around has been to put code in point to point in the configuration. Do not use circular interp it has always caused me grief. Especially when going around a full circular boss. If you are running full DNC point to point should not be an issue. I believe it has something to do with the way the kernel does the math on the full circle. Pro/e is famous for this even in part mode. I have seen it in patterning features in a circle, get just past the 180 degree point or approach 360 degree and boom your pattern fails in a number of different fashions. Never had a problem with code from point to point every move just a G1 xyz. Stay away from G01, G02, G41, G42 unless you can really check your code. Note this method is for roughing of large volumes of material when your program may become very large. Sometimes it makes good sense to use those codes when you are just doing a simple 2D profile on a part, a few hundred lines of code vs 10K lines of code on a large volume rough.
Another option if you have to use circular interp is to break your volume into two volumes. Half on each side of the boss. OR Don't let your volume go completely around the boss leave a little sliver out so the circle is not continuous.
The Haas machines I use have a feature that will allow dry run of code and you can watch it on the screen. Sometimes you could see where it would cut badly and other times it would show an error for machine overtravel. Either way it was not 100% that you were not going to scrap or break something but it was a quick check.