What's wrong here?

[CharlieM]

I have a very basic (3) axis Home Built Milling Machine.
I drive the stepper motors with K-Cam from a Desktop Computer.
K-Cam shows the out line of the part just fine, but when I put any diameter in ( G41 T001 ), it will only read the first 2 lines of code and stops!!?

I used this format on another, very simple, out line, and it seems to work, but here it don't !!?

I have ask this question on the Kellyware Forum, but no body responds?

Any help would be much appreciated.


[Tangs]
%
G90
M03
G17
G41 T001
G00 X0.44136 Y1.52635
G02 X.75154 Y1.59142 I1.48397 J-2.68099
G02 X2.23070 Y1.70326 I2.13091 J-6.81568
G01 X4.47936 Y1.70326
G01 X4.47936 Y1.45326
G01 X2.22936 Y1.45326
G03 X1.97936 Y1.20326 I2.22936 J1.20326
G01 X1.97936 Y.67052
G03 X2.22246 Y.42061 I2.22936 J.67052
G01 X4.07824 Y.36491
G03 X4.23909 Y.51678 I4.08290 J.52109
G01 X4.24348 Y.63493
G01 X4.66894 Y.62318
G01 X4.66453 Y.50424
G03 X4.81641 Y.34374 I4.82072 J.49993
G01 X5.58288 Y.32284
G01 X5.57598 Y.07294
G01 X2.25725 Y.16956
G03 X1.62836 Y.16293 I2.01989 J-7.25898
G03 X1.00620 Y.07372 I1.86606 J-3.71669
G01 X0.44136 Y1.52635
G40
M05
G00 X0 Y0
M30

[M250cnc]

I use Mach3

G41 is "Start cutter compensation left"

T001 is Tool 0001

This line "G02 X.75154 Y1.59142 I1.48397 J-2.68099"

You have to have the controller in the right IJ mode "Absolute or Incremental" for this to work correctly

If your using Cam the PP also has to be set so they are all reading from the same hymn sheet

Phil

[ger21]

Don't use KCAM, but try adding a leadin move before the G41, and also try calling the T1 before the G41. I think you also had a G3 instead of a G2.

Do you get an error? It seems to run fine in Mach3.

[Tangs]
%
G90
M03
G17
T1
G0 X0 Y0
G41
G00 X0.44136 Y1.52635
G02 X.75154 Y1.59142 I1.48397 J-2.68099
G02 X2.23070 Y1.70326 I2.13091 J-6.81568
G01 X4.47936 Y1.70326
G01 X4.47936 Y1.45326
G01 X2.22936 Y1.45326
G03 X1.97936 Y1.20326 I2.22936 J1.20326
G01 X1.97936 Y.67052
G03 X2.22246 Y.42061 I2.22936 J.67052
G01 X4.07824 Y.36491
G02 X4.23909 Y.51678 I4.08290 J.52109
G01 X4.24348 Y.63493
G01 X4.66894 Y.62318
G01 X4.66453 Y.50424
G03 X4.81641 Y.34374 I4.82072 J.49993
G01 X5.58288 Y.32284
G01 X5.57598 Y.07294
G01 X2.25725 Y.16956
G03 X1.62836 Y.16293 I2.01989 J-7.25898
G03 X1.00620 Y.07372 I1.86606 J-3.71669
G01 X0.44136 Y1.52635
G40
M05
G00 X0 Y0
M30

[ger21]

Also, what size is the tool? In Mach3, if the tool was larger than .1, it would'nt run correctly.

[CharlieM]

Ger21,
I re-wrote the program according to your suggestions. Nothing changes!

I did notice one thing, I would go a couple of lines father if I set the tool diameter at .100, same with the way you wrote and the way it was originally written.

That G03 move down in the program is correct, I'm climb milling and it's a counter clockwise move.

When I designed this part, I made sure that all inside radiuses were larger than .125, in order to use a .25 end mill.

You say it don't work with Master3 and a .25 Dai. end mill !

[ger21]

OK, I figured out that your code is written with Absolute IJ mode, and I was running it in Incremental IJ mode. Once I switched, it runs fine in Mach3, even with a 1/4" tool.

It's possible that it's a bug in KCAM, as it appears that comp is a newer feature in that software.