Problems With G02 G03 Using I And J

[Jim Estes]

I have been programming with Bobcad V20 for a while now, and before that I used V17. I have always had a problem with pocketing. Sometimes when I am pocketing I get erroneous output of I and J. Whenever I select all the code and then do a geometry from nc function, I get very larges radii for my toolpath. If I were to use these programs, the cutter would ruin the work. Seems I only have this problem sometimes, but when I do get this error I dont know how to get rid of it, I usually just use a different size cutter or redraw the pocket and do something different.

Do you think this might have something to do with the accuracy setting in the enviroment?

This is really starting to bug me. Here is a sample of the code. When I do a geomtry from nc on this I get a huge circle around the very small hole that I am trying to cut. The hole is a 0.156" diameter hole and I am pocketing with a 0.125" cutter. and stepping 0.005" and leaving no stock.

G00X-10.Y8.Z0.05
X7.4492Y1.196
G01X7.4492Y1.196Z-1.F2.0
G00X7.4492Y1.196
G01X7.4542Y1.196
G03X7.4542Y1.196I7.4487J1.196
G01X7.4592Y1.196
G03X7.4592Y1.196I7.4487J1.196
G01X7.4642Y1.196
G03X7.4642Y1.196I7.4487J1.196

Any ideas about what is causing this?

Jim

[mrainey]

It looks like I and J are being output as the absolute coordinates of the arc centers. Apparently your machine control needs them to be defined in some other way, such as signed incremental distance from start of arc to center point, or ?.

[HuFlungDung]

I concur with Mrainey. Check in your NC setup pages, there is a setting for the type of arc center coordinates.

This problem should not 'come and go' if you choose the same machine post each time you insert a new nc object....if you don't crash the program, in which event settings may not be written to disk properly.

Hint: if editing in Bobcad, use 'undo' (in the nc editor) to get rid of the code you don't want. This works a little better than just highlighting and deleting.

If I recall, I think that performing 'geometry from nc' uses your current post settings, so make sure that whatever post you used to post the code, is the same one used to regenerate the toolpath from the nc code. Just a precaution to take if nothing else seems to work correctly.

[Jim Estes]

Whatever it was, is got a whole lot worse. After a bit of playing around with it, going back and using old programs to compare to, I concluded that my PC must have had some proplems because all my programs were not working right, I had to re-install the setup for my machine and now it's working properly. I don't know what happened, but just out of the blue I started getting that error. After reinstalling the setup and redoing the macros I am back to where I was with this. Thanks for the replies.


BTW, my machine uses I and J absolute numbers. The numbers look like they were right, but the "geometry creation" portion of Bobcad must have gotten confused. Here is a sample of the output now.

G00X0.Y0.Z0.05
X7.4492Y1.196
G01X7.4492Y1.196Z-1.F2.0
G03X7.4491Y1.1959I7.4487J1.196F10.0
G01X7.4542Y1.196
G03X7.4542Y1.1959I7.4487J1.196
G01X7.4592Y1.196
G03X7.4592Y1.1959I7.4487J1.196
G01X7.4642Y1.196
G03X7.4642Y1.1959I7.4487J1.196

Jim

[tjones]

I did find an error in the pocketing that may be related to what you are seeing.

If you have set in the NC to 'show only changed x,y coordinates' then you will get a sporatic error of i,j output with no xy coordinates. You will get a full circle when you run or simulate the code. Uncheck these in the NC menu setpu>driver window.

Also I think you should check if your machine requires i,j to be increamental instead of absolute. Also you may wish to check that the area you are trying to pocket has enough room for the endmill you are using. Check that you have cutter comp turned off because that could cause the tool to make a large move when reversing directions like it does in pocketing.

[bdrmachine]

This sounds like the same sort of trouble I had with Vector. I beleive they are based on the same program code. I switched to a different cam package and have solved most of my problems.

[Jim Estes]

I have had problems with programs that were written by other people, using other cam programs, and they didn't have the post set to output I and J as absolute numbers. My machine requires absolute I and J numbers. This problem was something entirely different. It looked like the same thing, but I think that the problem was actually with whatever portion of BobCad does the backplotting. After the first program, I tried several old programs that I new were good programs, and when I backplotted them using the "geometry from NC" option, I got the same sort of crazy loops. I re-installed the setup that I got from the BobCad site, and then re-did my program start and end stuff and it seems to be working just fine again. It seemed like what used to happen to Windows 98, it would "degrade" over time, and I would have to re-install every once in a while to get all the code back to normal.

Jim