Machsupport Forum
G-Code, CAD, and CAM => G-Code, CAD, and CAM discussions => Topic started by: bartk on January 23, 2007, 09:13:06 AM
-
I am trying to do cutter compensation on a fairly simple shape, but Mach 3 complains about the end radius of the arc not matching the start radius.
The GCode below works fine if I remove the G41. Any suggestions?
G41 P0.09
N1 G00 X0. Y0. Z0.1
N2 X1.7 Y1.5
N3 G01 Z-0.375 F15.
N4 G02 Y1.25 I0. J-0.125 F20.
N5 G01 X1.2
N6 G03 X1.075 Y1.125 I0. J-0.125
N7 G01 Y0.875
N8 G03 X1.2 Y0.75 I0.125 J0.
N9 G01 X1.7
N10 G02 Y0.5 I0. J-0.125
N11 G01 X1.1211
N12 G03 X1.0327 Y0.4634 I0. J-0.125
N13 G01 X0.7479 Y0.1785
N14 G02 X0.5711 Y0.3553 I-0.0884 J0.0884
N15 G01 X0.7518 Y0.536
N16 G03 X0.825 Y0.7128 I-0.1768 J0.1768
N17 G01 Y1.2872
N18 G03 X0.7518 Y1.464 I-0.25 J0.
N19 G01 X0.5711 Y1.6447
N20 G02 X0.7479 Y1.8215 I0.0884 J0.0884
N21 G01 X1.0327 Y1.5366
N22 G03 X1.1211 Y1.5 I0.0884 J0.0884
N23 G01 X1.7
N24 G00 Z0.1
-
Are you set to incremental I,J mode in config, I think you need to be.
Graham.
-
Yes, I do have IJ set to incremental (tried other settings to, without much luck)
-
Are you cutting inside the shape or outside.
Looking at the code you don't have a lead in or out. Will you post me more detail and a DXF file and I will look into it in more detail.
Graham.
-
Here's the dxf (from BobCad V20)
Trying to cut on the outside (so G41 P0.0625 for a CW toolpath)
-
Try this program.
Graham.
O0001 (SHAPE)
G20 G40 G00 G80 G17
N1 (.0625 end mill)
G00 G90 X1.708 Y1.203
Z.1
G01 Z-0.375 F15.
G41 P.0625 X1.739 Y1.211 F20.
G03 X1.7 Y1.25 R0.039
G01 X1.2
G03 X1.075 Y1.125 R0.125
G01 Y0.875
G03 X1.2 Y0.75 R0.125
G01 X1.7
G02 X1.825 Y0.625 R0.125
X1.7 Y0.5 R0.125
G01 X1.121
G03 X1.033 Y0.463 R0.125
G01 X0.748 Y0.179
G02 X0.571 Y0.355 R0.125
G01 X0.752 Y0.536
G03 X0.825 Y0.713 R0.25
G01 Y1.287
G03 X0.752 Y1.464 R0.25
G01 X0.571 Y1.645
G02 Y1.821 R0.125
X0.748 R0.125
G01 X1.033 Y1.537
G03 X1.121 Y1.5 R0.125
G01 X1.7
G02 X1.825 Y1.375 R0.125
X1.7 Y1.25 R0.125
G03 X1.661 Y1.211 R0.039
G01 G40 X1.692 Y1.203
G00 Z1.
M30
-
I tried it, but Mach 3 now complains about the radius of the arc being smaller than the cutter after compensation. I think the problem is the lead in path.
Meanwhile I have generated a different toolpath with the offset function in BobCad. This function essentially creates the compensated toolpath.
Of course that means deciding upon a tool while doing the CAM, but it worked like a charm.
Thanks for your help!
Bart
-
This should work now.
Graham.
O0001 (SHAPE)
G20 G40 G00 G80 G17
N1 (.0625 end mill)
G00 G90 X1.681 Y1.094
Z.1
G01 Z-0.35F15.
G41 P.0625 X1.754 Y1.155 F20.
G03 X1.7 Y1.25 R0.063
G01 X1.2
G03 X1.075 Y1.125 R0.125
G01 Y0.875
G03 X1.2 Y0.75 R0.125
G01 X1.7
G02 X1.825 Y0.625 R0.125
X1.7 Y0.5 R0.125
G01 X1.121
G03 X1.033 Y0.463 R0.125
G01 X0.748 Y0.179
G02 X0.571 Y0.355 R0.125
G01 X0.752 Y0.536
G03 X0.825 Y0.713 R0.25
G01 Y1.287
G03 X0.752 Y1.464 R0.25
G01 X0.571 Y1.645
G02 Y1.821 R0.125
X0.748 R0.125
G01 X1.033 Y1.537
G03 X1.121 Y1.5 R0.125
G01 X1.7
G02 X1.825 Y1.375 R0.125
X1.7 Y1.25 R0.125
G03 X1.638 Y1.181 R0.063
G01 G40 X1.678 Y1.094
G00 Z1.
M30
-
I have a problem with compensation also. I just upgraded my mini mill 2 with new steppers and controller as well as Mach3. my g codes are created by a program I have used for years, (Minitech cnc) My templates come out 1 mm smaller all the way around. I use a 1 mm bit. I don't see any compensation in the Mach 3 program. I cut outside sometimes and inside others. I sure could use some help. Thanks joe
-
Hi Joe,
post a dxf file and I will have a look at it.
Graham.
-
I didn"t realize that compensation happened with the dxf file, but thought machine software did. Here is a dxf that we use. we always compensate to the outside oh the line. Thanks Joe
-
I have had a look at the dxf file and all looks ok.
Is the DXF file to size or do you scale it up/down?
Will Mach run off in the same place each time? If so where.
Is the profile size wrong from the start or part way through?
Dose it make one right and then one wrong?
What size cutter are you using and to what depth.
Graham.
-
Graham, I realized today that the Mach3 that I have has tool length compensation on the main screen, and put in my tool dia 1/16, ran the program and it worked great. I tried to run several other programs, and sometimes good, sometimes crazy off track. Reload instead of rewind seems to take care of that problem. When you tell machine to home, x and y seems to work, but z just goes up till out of travel.I am new to this software and any advise that you can give will be appreciated. The software that worked the old controller was very simple and you can see it @ www.minitech.com/software/download/programs.htm. I purchased this mill 6 yrs ago from Minitech, and had it upgraded because of board failure, and the Minitech people did not know how to compensate for tool dia.!!!!!
-
Hi Jrich,
I have sent you a PM.
Brett