Tool Compensation Woes

[PBpaul]

Hello all. I hope some of you will help me with this. I’m using Mill9.1 on a Digital Tool router. It is PC controlled and tool compensation is handled within Mastercam. We’re cutting a pair of long (60”) curved splines in the general shape of a backwards “C”, nested about a half an inch apart, with a small endmill, .038 inches in diameter. I’m doing “Depth Cuts” for 3 trips on each contour and I have compensation set to the left, for a climb cut. When I go CCW from bottom to top along the first contour, which is the one to the left, the tool starts exactly where it is supposed to and runs CCW up to the top and ends exactly where it is supposed to. Then it picks up and moves to the other contour, starts exactly where it is supposed to and comes CW back down the bed. However, as it approaches the end of the contour, it becomes apparent that the bit is incorrectly coming down the centerline of the contour. The error is +.019 in “Y”. Now it picks up and moves to the start of the first contour to do the second depth cut and starts +.019 off in “Y”. When it gets back to the bottom of the second contour, the error is +.038 in “Y” and at the end of the third and final depth cut, the error is +.057 in “Y”. In other words, the error grows by .019 each trip.

When I backplot and do the math on the values of Y I’m reading on the Mastercam screen, tool compensation is perfect. Furthermore, I can run this same exact file but use a much larger bit, say a .76 inch diameter endmill and everything is perfect. Any thoughts would sure be appreciated. I’m going to do the SP2 update tomorrow in hopes that helps. If any additional information would be helpful, please let me know.

Thanks - PBPaul

[crazy^millman]

It sound liek to me that your table is traveling on you or the riser box if you are using one. If the code is right then it has got to be the Machine. I will also ask this do you have all G90 in the toolpath. if by chance you have a g91 then it would cuase this shift or by some chance you have a fixture offset call or a turn cutter comp on and off all of these could casue this. It could also be soemthing simple as if you are using a machine that neededs the head trimmed in alot it could possible be off. Just trying to throw things out there.

 

Good Luck and if you post the File up in FTP we can take a look and see if you missed something.

 

Crazy Millman

[PBpaul]

Crazy Millman:

I will go thru the NC file with a fine-toothed comb and see if see anything like that. Thanks for the suggestion. The machine has a fixed bed with a overhead gantry. We've tested it pretty thoroughly and I'm certain that is is not just losing position in X or Y. I suspect that it is doing exactly what my NC file is telling it to do!!!!!! As a matter of fact, I can run these same contours with the same tool but with compensation "Off" and it runs dead on the money right down the centerline, trip after trip.

Thanks- PBPaul

[crazy^millman]

Ok bring into Cimco edit and do the find for all G41 or G42 and see if has any. See what you come up with be intresting to see what the fix is.

 

Crazy Millman

[Müřlıń®]

quote:

---

I will also ask this do you have all G90 in the toolpath. if by chance you have a g91

---

Sounds like incremental is being turned on like Nutty...errr Crazy....errr dam what is that guys name.... Ummm ya what he said.....

 

The increment is exactly half your cutter....

 

 

Murlin

[crazy^millman]

Well Murin been called and answered to things I cant put up on here.

 

 

Crazy Nutty Millman

[PBpaul]

I'm writing from home......had to go nite-nite.

First thing at work this morning is to search for anything odd in the NC file. I do know that almost all moves in our files are G91. We start in G90 to move spindle to an absolute position to install a given tool. Then we change to G91 until finished with that tool. If another tool is needed within the same NC file, then we go back into G91 and move to that same absolute position to manually change the tool. Once the manual tool change is made, then we're back in G91.

PBPaul

[PBpaul]

OK, there are no G41's or G42's anywhere in the NC file. There is only one G90 and that is at the beginning when the spindle moves to a specific position to receive the first tool. Then it moves in XY to the location of the first plunge (still in G90), moves down to the Retract Height, and then it changes to G91 and stays incremental until the part is finished or else another tool is called for. In this instance, there is only one tool and so the file ends, still in G91. I'm doing the 9.1SP2 thing this morning. If the problem is still there, I'll send the drawing up to the FTP site and wait for more help.

Thanks to everyone on this thread- PBPaul

[PBpaul]

I'm still stuck.

I've uploaded PBPaul.zip to cadcam's FTP site and placed it in MC9_files folder

 

It contains my drawing

It contains my .pst and the .txt that goes with it

It contains 2 NC files as examples

It contains a brief txt file re-explaining problem

 

I would greatly appreciate any suggestions.

I'm running Mill9sp2

 

Thanks- PBPaul

[Müřlıń®]

Your splines are messed up man. look in file murlin on ftp.

 

 

Murlin

[PBpaul]

Murlin:

How so? I have a copy of your file downloaded. What am I looking for?

Thanks- PBpaul

[Todd Patterson]

PBPaul,

 

I think there is a problem with your splines. I broke the splines to arcs, then reselected the geometry, regenerated the toolpath, and the comp looks like its working.

[PBpaul]

I really do appreciate the help but I'm still not understanding where I went wrong. Our customer sent us an Autocad drawing of an opening that we are surrounding with a wooden arch. We drew new splines (also in Autocad) to clean up waves and errors in the original and then did offsets for inside of trim, outside of trim, and so forth. Then this was brought into Mastercam and we did all the toolpaths and posted and promptly ruined the maple blank, which represented a whole lot of work down the drain. We then discovered that as long as we didn't ask Mastercam to provide tool compensation, it ran fine. We also discovered that as long as the tool is pretty large, as when cutting out the perimeter of the arch with a .76 dia endmill, that runs perfectly.

Should it be standard practice to convert splines to arcs before trying to cut? If ever there was a vanilla spline, this is what we thought we were drawing!

Thanks again. I'm still all ears!- PBPaul

[Müřlıń®]

Paul your splines were wigged out. You could see that there was a mistake in the top half. I cut off the half that was not correct and mirrored.

 

If comp isnt working, then you need to redo the geometry in arcs and lines.

 

Edit////

 

 

OK I converted your splines to arcs by Modify/Break/Splines to arcs and regened.

Try that. Look at murlin2 on ftp.

 

 

Edit////

 

 

Murlin

 

[ 10-03-2003, 01:49 PM: Message edited by: Murlin ]

[crazy^millman]

PBPaul I have found that when using Autocad splines they come into several program as garbbley gook. I found it always better to redo the arcs, splines, and other geometry when bringing them in. It seems like it should work and if you just look at it seems ok but upon futher investagation on very complex curves and shapes from Autocad it just seems to be that way. I think you have done everything in the right track just soemtimes you come across those thing you just huhhhhhhhh. Well I did look at your file but do not have 8.1.1 here so seem like my Buddy Muriln was steering you in the right direction.

 

Crazy Millman

[PBpaul]

Thanks- I will try to machine the files you uploaded and see what happens. Strange thing is, as long as I have comp turned off, all these contours machine perfectly. With comp on, CCW splines do fine but not CW. I may be able to get around the issue with Autocad but we also do/plan to do a lot of importing from Rhino to machine surfaces with very small cutters and so that's another reason why my red flags are up.

PBPaul

[crazy^millman]

Well bpauls with no cutter comp it will always do better. I think the reason for this is like doing a buch of broken lines. I do my text engraving this way to create toolpath that do what I want. It works great and goes in the direction I want and does good this way. If i do it with cuttercomp it will always seem to sometimes do a reverse or go on the wrong side things like that cuased by the geometry being broken just slighty.

 

I think you are on the right track and I wish you luck.

 

Crazy Millman

[Müřlıń®]

OK Paul, I re-read your posts and think I have a solution to your problem.

 

In order to get the cutter comp to work correctly on your cuts, you must chain each spline one at a time and you can cut with CC on the left or right.

 

When I pulled up your splines, they had what looked like an error on the top half and I assumed that was your problem. NOT

 

 

Somehow when you chain all 4 of them at once to cut them, the CC wigs out.

 

 

Murlin