[rfarleman]

I have been trying to program wire radius compensation (G41 or G42) on a Sodick A280 machine for a circle and I keep getting the message "Offset approach is impossible with arc instruction." Radius comp works for a rectangle but I can't do a circle. I know that you have to make a right angle when you begin cutting. I am cutting in from the edge of the part on the center line of the circle and then start the arc. I thought that would make the required right angle approach. I can cut a circle without comp just fine but I must be missing some instruction for compensation. Do I need to define G54 and/or G92 in a certain way?

[sodickappsguy]

can you post the code you are using? What diameter hole are you trying to program? Are you trying to use I,J or R? What offset are you using?

[rfarleman]

The hole diam is .130 inch and the edge of the hole is .050 inch from the edge of the part. The code I used is as folows:

G90
G54
G92X0.0Y0.0
G41H007
G01X0.100
G03X0.100Y0.000I.065J0.0
G40X0.0Y0.0
M02

I have noticed in the Sodick manual for the G41 & 42 command for the "H" value, in one place it says H007 = .007 inch and in another place H07 = .007 inch, which one is correct.

[TheBigJW]

The G41 needs to be on the same line as the G01.

John

[sodickappsguy]

Ok here is what i would use to make the hole. This assumes a few things. I assume that the start hole is in the center and not .05 from center. The condition number and H offset is just random numbers. Always refer to what your power settings manual says to use. The Condition number does not have to be on the same line and the first cut neither does the H value. The machine will use the last C and H called up in the program. both C and H can be three digits or one. (ex H007 and H7 is the same thing) Most people stick with 3 digits to make the code clean.

Some other helpful bits for you G00 X0. Y0. can be shorten to XY. The machine will assume if you dont give a G code at the start of the program (G01,G02,G03) that the code is G00. If you dont give a value for the direction the machine assumes 0. also you can use R for programming arcs. R programming will let the machine figure the I,J for you. An example of this is G02 X0. Y.065 R.065. The machine knows the end of the arc and will figure the radius based on the R value. Your program had a few mistakes in it.


It would be a good habit to break the arc in half or quarters. Sometimes the machine will have a brain fart cause if you give it a position that it is already at it will skip the line of code.

The G40 line needs a G1 in it. Cutter comp lines must always have movement (rapid is not acceptible)
program assumes start from center.
G92X0.0Y0.0
C100 H001
G41 G01 X0.065 Y0.
G03 X0. Y0.065 I-.065.0 J0
G03 X-.065 Y0. I0. J-.065
G03 X0. Y-0.065 I.065 J0.
G03 X.065 Y0.I0 J.065
G40 G01 X0.0Y0.0
M02

If you Pm your email address i can send you a EX21 control training manual. Your control will program similar to this control.

[rfarleman]

I used your code and the program runs great. I just made several cuts with different comp values and the hole came out exactly to size.

Thanks!!!

[sodickappsguy]

Glad to hear it. I just emailed you the training manual for the ex21. I didnt see your email when i checked it late last night. One other thing that i can show you is you can cut a radius with a G01 command. The example is below. The big thing is you MUST HAVE CUTTER COMP TURNED ON. I am doing the code long hand to keep it clear but you can short hand it and get the same result. The example below will cut a one inch square with .05 corner radius.

LONG HAND
C001 H001
G00 X0. Y0.
G41 G01 Y-.5
G01 X.5 R.05
G01 Y.5 R.05
G01 X-.5 R.05
G01 Y-.5 R.05
G01 X0.
G40 G01 Y0.
M02

SHORT HAND.
C1 H1
G0 XY
G41 G1 Y-.5
X.5 R.05
Y.5 R.05
X-.5 R.05
Y-.5 R.05
X
G40 G1 Y
M2