Boss drive works, now controller problems

[jderou]

Well the drive system works great now, transistors fixed the z-axis. Now for the next problem. Using MDI, G0 and G1 work fine, G2 and G3 don't. When I try to enter G2 or G3, it either doesn't do anything or just moves in one direction. It worked one time for me, no luck since. I pulled out the XDI, ERS, etc. boards, they were all partially coated in a fudge-like substance (old oil-based cutting fluid? The whole machine was covered in it when I got it). I cleaned this off best I could, but it didn't help. The format I am entering the code is:
G2X0Y0X-2Y0F100
Maybe it is related but also when I have the selectors both set on TNO and push the button, nothing happens (supposed to increment tool number).
With the RS232 hooked up, I can download ok, but it usually won't run (even G1 and G0).
Is it the pull-out boards that do all of the control work?
Aaargh, if it isn't one thing its something else. I spent most of today troubleshooting the spindle (wouldn't come on all of the sudden) turned out to be something wrong with the brake interlock.
Thanks for any help!

[HuFlungDung]

If the machine is using standard ISO code format, the structure of your arc movements should be:
G X Y I J F
where I = the X value of the arc center, and J = the Y value of the arc center.
There are two possible systems that the arc center can be calculated on: absolute arc center coordinates or incremental arc center coordinates. Machintek could likely tell you which way it should be for this controller.

The arc center coordinates have to be accurately calculated, or your machine may alarm, or it may take a funky "corrective action" to get to the final coordinates in XY that you specified in your G02/G03.

[machintek]

A G2 or G3 is a circular move. It needs a R value or an I & J to create an arc. It assumes you are at the start point and the G2/G3 line is the end point. As a matter of good programming, I usually would include decimal points in my values, EXCEPT feedrates which do not have any. A F100 is actually a feedrate of 10 IPM. The use of an R is easier but I have seen machines fit an arc between points. The I J defines the center of the arc and is more accurate. If you want to mill a hole, look into the G79 command. Very slick.

George

[jderou]

Well my spindle died again last night so I can't experiment with this yet. A bit of investigating shows I only have 2v between lines 2 & 3 (for the spindle latching), I am assuming this should be 24v. Other than this I have good continuity all the way to the spindle contactor.

[jderou]

Got the spindle working again, still having problems with circular int. though. It's like it doesn't recognize G2 and G3. If I have a couple lines like this:
G0 X0.000 Y2.000 Z-2.000
G3 X0.000 Y-2.000 R2.000 F200
G3 X0.000 Y2.000 R2.000
It carries the G3 lines out as if they were G1, it moves straight to Y-2 and Y2. Is it possible for the thing to 'forget'?

[machintek]

Research multi quadrant. There is a G code to do this. On later machines the control booted with this enabled.

George

[HuFlungDung]

If this is an old machine, it may not recognise R. Better to stick with I and J. You need to know whether the arc center coordinates, I and J, need to be incremental (relative to the current position), or absolute, depending on whether your machine is currently in G91 or G90 mode.

[jderou]

G75!! Thank You, Thank You, Thank You!! I was starting to really worry about this thing but I found G75 and that did it.
Now to make stuff!