Need Help!- Program runs the wrong way....

[bgrdtruk]

I have a Program that I'm running on a vmc with a Yeong chin MXP-200i control (came with 21I books). The program was produced in cad/cam and verified ok then it was sent to the machine.(cf card)
It ran half way through the program then made a complete loop(shouldn't have) and kept going like nothing was wrong.
I verified the program in another cad system and it checked ok... I then had another vmc (OI-MD control) draw the program in it's graphics and it looks fine.......

My question is is there a setting for arc tol. that would cause one machine to machine the wrong way around a G03 and the other to cut correctly ???????

[sinha_nsit]

Yes.

Try radius method. It would always work.

[bgrdtruk]

Thanks for the reply.

The cam software outputs I J K and it has worked fine up till now(we have run hundreds of programs this way) but there is something just a little off about this and I can't put my finger on it.

I'd like to hear any more ideas about this weird motion.

Thanks
Steve

[christinandavid]

Had this happen when doing a 180deg arc using R method, with cutter comp active. I altered the CAM program R+, R-, and IJ method at the machine to no avail - it happened using all methods. Ended up changing it to G1s with a ,R to round the corners that worked. I have a sneaking suspicion it was something to do with the cutter compensation...

DP

[bgrdtruk]

Thanks for the reply.

The cutter comp. was not active for this program.

This is just driving me nuts because now we have to dry run all the programs for this machine to make sure we don't trash any more parts.

AAAARRRRRRRHHHHHHHHH LOL

Thanks Guys

Steve

[drdos]

This happens when your radius is too small. The controller mis-interpenetrates the radius and sends the tool in the opposite direction. Make sure your radius isn't so tight.

[sinha_nsit]

Post the part of the program where you get unexpected movement.
In IJK method center must be correctly specified within a tolerance which may have different settings on different machines. So, the same program may behave differently on different machine.

[bgrdtruk]

Thanks for the replies.

Here is the section of code we were using:

G01 X7.2754 Y-.8438
G02 X7.3372 Y-.784 I1.9184 J-1.9184
X7.4039 Y-.7301 I.3974 J-.4235
X7.4776 Y-.686 I.3636 J-.5248
X7.5564 Y-.6518 I.3161 J-.6203
X7.6407 Y-.6281 I.2321 J-.6633
X7.7274 Y-.6159 I.1275 J-.5929
X7.7995 Y-.6135 I.0721 J-1.0691
X7.815 Y-.6136 I0. J-1.0715 (the problem occurred in this area)
G03 X7.9027 Y-.6143 I.0877 J6.0563 F93.16
G01 X8.078 F97.

I have posted the whole nc file for those who want to see the whole path. the area in the file is marked with a N3333 to N3334.

I understand what path the control is following (the wrong direction vrs. programed path) but my worry is that there is a setting in this control that allows the control to "adjust" for a programing error and cause this problem.

I'd like to figure this issue out so I can set the cad/cam and all the controllers the same to prevent this issue in the future.

Thanks for all the help.

Steve

[sinha_nsit]

The program looks ok. There is an error of 0,0001 inch in radius calculation.
Possibly, floating point error is causing problem. Try larger path segments in your CAM software.