Cutter Compensation Problem

I have a problem with the cutter compensation on EMC2.
I’m trying to cut ¼” dowel pin holes using circular interpolation and cutter comp.
I have read all of the information on G41 and G42 and the rules for cutter radius VS programmed radius.
On the Tooling page it asks for “length” and “DIAMETER” for each tool.
I should be able to mill a ¼” hole using any endmill that has a smaller “Radius” than .125.
Using the program below EMC2 will only allow me to use a cutter that is 1/8” diameter or smaller.
The program reacts as though it is seeing the “Diameter” amount on the tooling page as a “Radius” amount. The radius of the 1/8” endmill is .0625. If I put .130 in for the cutter diameter I get a “arc move in concave corner cannot be reached by the tool without gouging alarm”. I should be able to make a .125 radius move with a .065 radius cutter.
Something is wrong here. Is there a parameter setting in the software that can be changed? Any help would be greatly appreciated.
SAMPLE PROGRAM
%
(tool 1 ENDMILL D.125 C0. L1.5)
G17 G20 G40 G49 G80 G90 G00 G94 X0 Y0 Z0
(MSG, " Change to .125 ENDMILL )
(MSG, " Spindle Speed 2383")
(M0)
G43 G90 H1
G1 Z.1 F5
(M0)
(Begin FEATURE PROFILE)
X0 Y0. Z-.25 F13.3476
G42 D1 Y.125 F25.
G2 X.125 Y0. I0. J-.125
X-.125 Y0. I-.125 J0.
X.125 Y0. I.125 J0.
X0 Y-.125 I-.125 J0.
G1 G40 Y0.
G0 Z.1
G00 G49 Z0
G90 G00 G40 G80 X0.0 Y0.0 Z0.0
M2
%

John,
You did mean "you can NOT turn on cutter comp with a move that is less than the radius of the tool" correct?
My cutter is .125 dia, on the Tooling page I am telling it that it is a .130 dia. The G42 line of code is moving .125 which is .060 larger than the radius of the tool. The next move is a radius move of .125 also. as soon as I increase the diameter from .125 to .130 I get the gouging error. That shouldn't happen. I mill 1/4" holes with cutter comp using a 3/16" cutter in my shop all the time, without any errors. This is a .125 dia. cutter milling a .250 hole. Increasing the diameter by .005 should not result in an alarm.

thanks for the tip on M2 and %. I will take care of it.

JT,
I played around with a few different types and sizes of lead ins and lead outs for cutter comp. I programmed a 1” x 1” square pocket with ¼” rad. Corners, and I used a .450 arc as a lead in for cutter comp so I could test a few ideas.
Here is the 1” square program and what I have discovered:

%
( tool 1 ENDMILL ROUGH D.25 C0. L2.5)
(SQUARE CUTTER COMP TEST.NC)
G17 G20 G40 G49 G80 G90 G00 G94 X0 Y0 Z0
(MSG, " Change to .25 ENDMILL ROUGH")
(MSG, " Spindle Speed 1191")
(M0)
G43 G90 H1
G1 Z.1 F5
(M0)
(Begin FEATURE PROFILE)
X0. Y.05 Z-.25 F6.6738
G41 D1 X.45 F13.3476
G3 X0. Y.5 I-.45 J0.
G1 X-.25
G3 X-.5 Y.25 I0. J-.25
G1 Y-.25
G3 X-.25 Y-.5 I.25 J0.
G1 X.25
G3 X.5 Y-.25 I0. J.25
G1 Y.25
G3 X.25 Y.5 I-.25 J0.
G1 X0.
G3 X-.45 Y.05 I0. J-.45
G1 G40 X0.
G0 Z.1
G49 Z0.0
G90 G00 G40 G80 X0.0 Y0.0 Z0.0
M2

1. I ran this pocket profile program with the cutter Diameter set at .100. It ran fine and it offset to the inside of the pocket by .050. So, it is reading the Diameter amount on the tool page and offsetting correctly.
2. I increased the diameter several times up to .450 on the tool page, and it ran fine each time.
3. When I changed the diameter to .460 on the tool page, I get the gouge error. I should be able to cut this pocket with a cutter diameter of .499 or less without any error. The .450 radius lead in is still larger than the .230 radius of the cutter.
4. I changed my lead in to a “tapered line” instead of an arc. The program ran without errors until my cutter diameter was set at .500. This is how it should be.
Summary:
I believe the problem is in the software. As soon as my diameter setting on the tooling page is equal to the programmed radius of the lead in, I get an error.
I can use a different lead in on larger shapes to avoid this problem. However, on small holes I really don’t have any other choice except for the arc lead in.
I’m sure that this is a software glitch. Can this problem be passed onto the Linux programmers to be fixed? Is there already a fix that I am not aware of? Please help.

Thank you,
Karl

I tried that too. I tried a 1" radius lead in above the part to the side wall contact area for a 1/4" hole. Then feed down in the z axis to final depth (this would leave a witness mark which is not desired). As soon as it read the next move which was a .125 radius, it gave me the error. If I change the cutter diameter to .124 or .123, it runs fine.

FYI to other users.
The best solution to my cutter comp problem with smal holes would be G12 or G13 (which EMC2 does not offer at this time). This is a true circular interpulation G code. It does a circular lead in to a starting point, then cuts the entier circle and goes past the starting point, then circles back into the center of the hole.
The best option that I found was a While / Endwhile Subroutine (wiki.linuxcnc.org/cgi-bin/wiki.pl?G12-13).
This will work with a little extra programming.
However, I still believe there is a glitch in the software. It should not give an error until your cutter radius is larger than any programmed radius on the part.
Happy Programming,
Karl

Can you do a G2/3 spiral down with cutter comp?