[cwhettinger]

Hi everyone,

Long time lurker, first time poster.

I am new to CNC, so bear with me. I have read a lot of posts regarding the error I'm having, but when it is out of the context of my part I lose understanding of what to do.

Mill: Tormach PCNC 1100 (Mach3)
Cam: Camworks

Problem:
I am receiving "tool radius not less than arc radius" in the message window of Mach3. Here is a photo of my part:

Attachment 259762

I am receiving error when the tool tries to cut the 2D contour (perimeter) path of the part, oriented as in the photo above. When the path is wrapping around the "top" of the crown points (N23), it gives me the error.

Here is my gcode:

%
O1 ( PROP-.75LEADIN )
(CWPOST: TORMACH PCNC1100 BLC TAMPA)
( 12-6-2014 )


(T22 = 1/2 EM HSS 2FL 5/8 LOC)
(T77 = 1/8 CRB 2FL BM 1  LOC)


(CW OPER= CONTOUR MILL8)
(1/2 EM HSS 2FL 5/8 LOC)
N1 G00 G90 G40 G98
N2 G43 M06 T22 H22
N3 M08
N4 G00 G90 G54 X2.7248 Y.1237 S3162 M03
N5 Z.1
N6 G01 Z-.6228 F5.6
N7 G01 G41 D72 X2.2869 Y-.1175 F3.
N8 G03 X1.9283 Y-.5658 I.3618 J-.6569
N9 G01 X1.8498 Y-.8369 F11.24
N10 X1.844 Y-.8506
N11 G02 X1.4369 Y-1.079 I-.351 J.1486
N12 G01 X1.4302 Y-1.078
N13 X1.4236 Y-1.0766
N14 G03 X.9063 Y-1.0201 I-.5624 J-2.7528
N15 X.389 Y-1.0766 I.0451 J-2.8093
N16 G01 X.3824 Y-1.078
N17 X.3757 Y-1.079
N18 G02 X-.0314 Y-.8506 I-.0561 J.377
N19 G01 X-.0372 Y-.8369
N20 X-.2 Y-.2748
N21 Y-.2393
N22 G02 X.4131 Y.0588 I.3791 J0
N23 G03 X.5996 Y.0752 I.0834 J.1198
N24 G01 X.6018 Y.0774
N25 X.604 Y.0795
N26 G02 X1.2086 I.3023 J-.3188
N27 G01 X1.2108 Y.0774
N28 X1.213 Y.0752
N29 G03 X1.3995 Y.0588 I.103 J.1034
N30 G02 X2.0126 Y-.2393 I.2341 J-.2981
N31 G01 Y-.2748
N32 X1.9283 Y-.5658
N33 G03 X1.9918 Y-1.1363 I.7204 J-.2087 F3.
N34 G01 G40 X2.233 Y-1.5743
N35 G00 Z.1
N36 Z1.
N37 M09
N38 M05

(rest of gcode omitted)

What I've tried:
I have tried the following based on advice in other threads:
1.) To test, I changed the tool diameter in the Tormach tool table to .001 to see if it worked in an air cut test. It still gave the error.
2.) I changed the gcode from having a lead-in to a simple z plunge. It still gave the error.

We have limited tooling, so we are using a .5" cutter due to the length of cut we are trying to do.

What is confusing to me is that the path is on the left side of the cut throughout the part. The "crown" points are separated by a .4" radius arc - which should have no problem handling the .5" end mill radius of .25".

If anyone can help explain what the error is here, as well as give any advice as to solutions, I'd appreciate it.

Thanks to this community for answering hundreds of other questions for me!

[SCzEngrgGroup]

My guess is the problem is this line:

N7 G01 G41 D72 X2.2869 Y-.1175 F3.

This is the line that turns on the tool radius compensation, but though you are using tool 22, it is specifying, in the "D" word, to use the radius of tool 72. I would guess if you edit the "D72" to "D22", it will run correctly. This is likely an error in the Camworks POST.

Regards,
Ray L.

[cwhettinger]

I would guess if you edit the "D72" to "D22", it will run correctly. This is likely an error in the Camworks POST.

Ray you were exactly right. The D word wasn't getting set to the correct tool.

We had a compounding of errors - not only was the cam assigning the wrong tool number to the D word, which then looked up a much larger cutter diameter, but it ALSO was already planning an offset path. This double offset made our arcs too small for the .5" cutter.

To fix this, we zero'd out our machine tool file's diameter field and plan to only use the CAM values for this.

Thank you so much for your help!!!