[RBCMan]

I am a new operator of a Unisign machine (model # unknown), which uses the Siemens programming language. I have a problem cutting a CCW radius with left-hand cutter compensation active. The problem arises when the machine reads ahead and give me a "wrong block" error message for the CCW radius. This is what I've programmed:

G58 x15 y-3.375
G0 X0 Y0
Z.2
G1 Z-.8
G41 X0 Y2
X-3
G3 X-4 Y1 J-1 (this is the line that give the machine the error)

I'm having a hard time determining whether the J is the correct radius variable, or should I use the I for the radius? This has stumped me for a long time, and I really would like to know once and for all how to use the I and J.

[HuFlungDung]

I and J are the X and Y coordinates of the arc center, so you need both values, typically correct to whatever tolerance the machine is capable of holding.

You also need to know whether the control expects those arc center coordinates to be incremental (relative to the arc endpoint), or whether they must be absolute coordinates, based on the work datum.

[RBCMan]

So for the arc that I've programmed, do I need to put both I and J in the line to let the machine know that the X and Y are changing, due to the 1" radius?
Or do I only need the I or J on the line to correspond to one axis?

I'm cutting out an 8"x4" rectangular pocket w/1" radius corner in the center of a hot-rolled steel plate.

Bear with me. I learned programming from a fellow employee who didn't have a good grasp on cutter compensation himself, and I haven't been able to take time to use scrap metal and test programming functions to see how they work.

[HuFlungDung]

The standard arc format is:
G02 XYIJ
or
G03 XYIJ
This formatting puts the machine into circular interpolation mode, and it knows how to move X and Y based on the arc center position that you have given it.

This is really nothing to do with tool radius compensation, though. A profile path is entered into the control as a normal full scale path when you use tool radius comp. This means, no offset is calculated into the profile by the programmer. Instead, the control requires the entry of the radius (or diameter) of the cutter in the appropriate address in the tool radius comp register. And furthermore, that comp address has to be called up when you turn on radius comp, otherwise, nothing is applied.

Then, the control is supposed to offset the cutter from the programmed path by the radius of the cutter. This is the essence of radius comp. You, as the programmer, need to be mindful that all the radii in the profile are at least large enough for the machine to create the offset without "going negative" on the radius, which is impossible.

This can be a complex subject and we've kind of jumped into the thick of it without proper introduction.

I'd recommend that you get this working first without the G41.

[RBCMan]

Since the G03 uses cutter comp. to calculate out the travel path, and I've already invoked g41 (LH comp.), would it be a good idea to subtract the mill's radius from the arc radius and use the new number for the I & J radius #?

Or should I just program the coordinates and adjust them for the mill's radius, thereby avoiding a conflict with the G03 and the G41?

Revised example based on first program:
G58 x15 y-3.375
G0 X0 Y0
Z.2
G1 Z-.8
y1.75
X-3
G3 X-3.75 Y1 J-.75

[HuFlungDung]

Reread what I wrote. A cutter comped program path is full scale, no offset. If you want to calculate all the offset path, then you don't use radius comp at all.

Using cutter comp means that the cutter will be left (or right) of the program coordinates by the radius of the tool.

Where is your call for the control to retrieve a value from the tool comp register?

[RBCMan]

I got a basic course on how to program, and everything else I've learned by trial and error, so I'm not as clear on the terminology.
I'm not quite sure what you mean by the "call for the control to retrieve a value from the tool comp register", but I do put: Txx Dxx M6 to get the tool and the tool information before running the rest of the program.

I understand what I was doing wrong, the G41 and G03 were conflicting due to cutter comp. on top of cutter comp, can't do both. Clears up the confusion perfectly.
Thank you very much for all your help and information. This is my first posting, and it's been wonderful. Thanks again.

[HuFlungDung]

G03 is not cutter comp, it is simply a command to execute a movement with circular interpolation, instead of linear interpolation. Lots of programed paths contain arc movements which are perfectly legal with cutter radius comp turned on.

Cutter radius comp means the control compensates for the actual diameter/radius of the current tool and has nothing to do with arc movement commands.

Your description Txx Dxx M6 does imply some kind of invocation of calling a "D" value from the cutter radius register.