[Steven74]

Hello Everyone,
I am somewhat new to cnc programming and could really use some expertise to solve this problem. Any help is much appreciated. Im taking over the programming of our cnc machines because the person who use to do it is no longer around so I don't know what kind of mess I inherited.

The machine is a Monarch 150 with a Fanuc series 16 controller. Here's what I got. Keep in mind that this program worked in the past and that the tool offsets were accidently erased.

The program uses a 1" mill to rough out a pocket that is 1.75 wide and 1.12 deep in a mild steel block. Then the program is set up to use a 3/4" HSS mill. Here is the SUB program:

%
O2011(SQUARE HOLE -Y)
(1" MILL)
G40
G91
G1Z-.125
G1G41D7X.3725Y-.8725
G3X.5Y.5R.5
G1Y.75
G3X-.5Y.5R.5
G1X-.75
G3X-.5Y-.5R.5
G1Y-.75
G3X.5Y-.5R.5
G1X.75
G1Y.8725X-.3725
G40G90
M99
%

Cutter D offset is .500 with no other offset for that cutter except for the height. The Over travel occurs at the 4th G03. The cutter then goes back to the center without going to the last position G1Y.8725X-.3725 which leaves stock that I dont want.
I tried to use a 3/4" carb insert mill with the correct offsets thinking that the previous programmer forgot to change the reqiured tool in the program. The overtravel in the 4th corner went away but then the cutter would still leave the unwanted material. I then tried these changes:
%
O2011(SQUARE HOLE -Y)
(3/4" CARB INSERT MILL)
G40
G91
G1Z-.125
G1G41D7X.3725Y-.8725
G3X.5Y.5R.5
G1Y.75
G3X-.5Y.5R.5
G1X-.75
G3X-.5Y-.5R.5
G1Y-.75
G3X.5Y-.5R.5
G1X.75
G3X.5Y.5R.5
G1Y.3725X-.8725
G40G90
M99
%

I wanted to move the cutter across by repeating the first corner again with the 3/4" mill but then got the CRC error on this side instead of the other.
I experimented with the wear offset to move the cutter where I needed it to be so that my hole was at 1.74" but still got the CRC error on the last Radius. Any ideas?

[beege]

Hello Everyone,
I am somewhat new to cnc programming and could really use some expertise to solve this problem. Any help is much appreciated. Im taking over the programming of our cnc machines because the person who use to do it is no longer around so I don't know what kind of mess I inherited.

The machine is a Monarch 150 with a Fanuc series 16 controller. Here's what I got. Keep in mind that this program worked in the past and that the tool offsets were accidently erased.

The program uses a 1" mill to rough out a pocket that is 1.75 wide and 1.12 deep in a mild steel block. Then the program is set up to use a 3/4" HSS mill. Here is the SUB program:

%
O2011(SQUARE HOLE -Y)
(1" MILL)
G40
G91
G1Z-.125
G1G41D7X.3725Y-.8725
G3X.5Y.5R.5
G1Y.75
G3X-.5Y.5R.5
G1X-.75
G3X-.5Y-.5R.5
G1Y-.75
G3X.5Y-.5R.5
G1X.75
G1Y.8725X-.3725
G40G90
M99
%

Cutter D offset is .500 with no other offset for that cutter except for the height. The Over travel occurs at the 4th G03. The cutter then goes back to the center without going to the last position G1Y.8725X-.3725 which leaves stock that I dont want.
I tried to use a 3/4" carb insert mill with the correct offsets thinking that the previous programmer forgot to change the reqiured tool in the program. The overtravel in the 4th corner went away but then the cutter would still leave the unwanted material. I then tried these changes:
%
O2011(SQUARE HOLE -Y)
(3/4" CARB INSERT MILL)
G40
G91
G1Z-.125
G1G41D7X.3725Y-.8725
G3X.5Y.5R.5
G1Y.75
G3X-.5Y.5R.5
G1X-.75
G3X-.5Y-.5R.5
G1Y-.75
G3X.5Y-.5R.5
G1X.75
G3X.5Y.5R.5
G1Y.3725X-.8725
G40G90
M99
%

I wanted to move the cutter across by repeating the first corner again with the 3/4" mill but then got the CRC error on this side instead of the other.
I experimented with the wear offset to move the cutter where I needed it to be so that my hole was at 1.74" but still got the CRC error on the last Radius. Any ideas?

Try moving the G40 to the previous G1 line. You have comp turning on in the linear move before the first arc, and it should turn off on the move after the last arc...

HTH

[Steven74]

Thanks for the advise. I'll try it and see what happens.

[angelw]

Hello Everyone,
I am somewhat new to cnc programming and could really use some expertise to solve this problem. Any help is much appreciated. Im taking over the programming of our cnc machines because the person who use to do it is no longer around so I don't know what kind of mess I inherited.

The machine is a Monarch 150 with a Fanuc series 16 controller. Here's what I got. Keep in mind that this program worked in the past and that the tool offsets were accidently erased.

The program uses a 1" mill to rough out a pocket that is 1.75 wide and 1.12 deep in a mild steel block. Then the program is set up to use a 3/4" HSS mill. Here is the SUB program:

%
O2011(SQUARE HOLE -Y)
(1" MILL)
G40
G91
G1Z-.125
G1G41D7X.3725Y-.8725
G3X.5Y.5R.5
G1Y.75
G3X-.5Y.5R.5
G1X-.75
G3X-.5Y-.5R.5
G1Y-.75
G3X.5Y-.5R.5
G1X.75
G1Y.8725X-.3725
G40G90
M99
%

Cutter D offset is .500 with no other offset for that cutter except for the height. The Over travel occurs at the 4th G03. The cutter then goes back to the center without going to the last position G1Y.8725X-.3725 which leaves stock that I dont want.
I tried to use a 3/4" carb insert mill with the correct offsets thinking that the previous programmer forgot to change the reqiured tool in the program. The overtravel in the 4th corner went away but then the cutter would still leave the unwanted material. I then tried these changes:
%
O2011(SQUARE HOLE -Y)
(3/4" CARB INSERT MILL)
G40
G91
G1Z-.125
G1G41D7X.3725Y-.8725
G3X.5Y.5R.5
G1Y.75
G3X-.5Y.5R.5
G1X-.75
G3X-.5Y-.5R.5
G1Y-.75
G3X.5Y-.5R.5
G1X.75
G3X.5Y.5R.5
G1Y.3725X-.8725
G40G90
M99
%

I wanted to move the cutter across by repeating the first corner again with the 3/4" mill but then got the CRC error on this side instead of the other.
I experimented with the wear offset to move the cutter where I needed it to be so that my hole was at 1.74" but still got the CRC error on the last Radius. Any ideas?

Hi Steven,
In both examples the cutter starts and finishes not quite in the centre of the pocket; its off by 0.0025 in both the X and Y axes, not that that would cause the problem you're encountering.

I can't see your program working if using a 0.5 cutter radius compensation value for D7, when the corner radii are 0.5. Normally this would result in a Cotter Radius Compensation Error if the CRC equaled any concave radius in the profile, but would work if the CRC value was set to 0.4999.

If a 1.0" cutter is used to rough the pocket, there is no scope to being able to offset the cutter to leave a finishing allowance. Normally you could set a larger than actual cutter radius (greater than 0.5) so that a finish allowance is left. Doing so with a 0.5 corner radius will result in an alarm being raised.

Try the following program to rough with if you're hell bent on using the 1.0" cutter, and 0.5 corner radii in the pocket. Using a 0.510" CRC offset value for D will result in a 0.010" finishing allowance on all sides.


O2011(SQUARE HOLE -Y)
(T07 1" MILL - ROUGH PROFILE)
G40
G91
G01 Z-0.125
G41 G01 X0.0 Y-0.875 D07
G01 X0.857 Y0.0
G01 X0.0 Y1.750
G01 X-1.750 Y0.0
G01 X0.0 Y-1.750
G01 X0.875 Y0.0
G40 X0.0 Y0.875
G90
M99

Then use the following sub program to finish with, using a 0.375" CRC offset value (or thereabouts) to result in the correct pocket size.
%
O2012(SQUARE HOLE -Y)
(T08 3/4" CARB INSERT MILL - FINISH PROFILE)
G40
G90
G01 Z-1.120
G41 G91 G01 X0.375 Y-.875 D08
G03 X0.5 Y0 .5 R0.5
G01 Y0.75
G03 X-0.5 Y0.5 R0.5
G01 X-0.75
G03 X-0.50 Y-0.5 R0.5
G01 Y-0.75
G03 X0.5 Y-0.5 R0.5
G01 X0.75
G40 G01 X- 0.375 Y0.875
G40G90
M99
%

Regards,

Bill

[Steven74]

Thanks for your help.

[Steven74]

Thanks again for everyones help. The program is now running again.