[dwneumann]

I am pulling my hair out trying to get 4-axis working and am asking for help from anyone who is using MadCam 4-axis with Mach3 successfully.

I am trying to mill the attached model (zip file): it is basically a squashed cylinder with a gouge scooped out of it. Madcam produces a roughing toolpath that looks correct in the viewport and in the simulator, but the Gcode produced by the Mach_3_Inch_4-axis post processor causes A axis moves that crash the cutter into the stock.

I don't know whether this is a MadCam problem, a post processor problem or a Mach3 problem, but I have painstakingly tried every combination of postprocessor options (the resulting G code files are identical regardless of whether *ANGLE_OUTPUT* is set to CONTINUOUS, ABSOLUTE, or unset), and I have tried every combination of Mach3 options Ang-Short-Rot-on-G0 and Rot-360-Rollover without success. Attached image #1 shows how the toolpath looks in Rhino and attached image #2 shows how it looks in Mach3 with Ang-Short-Rot-on-G0=OFF and Rot-360-Rollover=OFF. You can see that in Rhino the toolpaths to scoop out the the gouge are nice smooth Z-level contours, but in Mach3 the toolpaths are interrupted by 360 degree rotations of the table with the cutter below the surface of the stock. (the G gcode file produced by MadCam is also attached.)

I cut the Gcode down to find the exact cause of the crashes and discovered that during post MadCam flips the sign of A axis coordinates from positive to negative and vice versa at A=180 degrees, so that instead of a path that goes A=178, 179, 180, 181, 182... it generates a path of A=178, 179, 180, -179, -178... So any move that crosses A=180 degrees generates a 360 rotation of the table without raising the cutter to safe Z.

Can someone with a working 4-axis setup please tell me what combination of MadCam, Mach_3_Inch_4-axis post processor and Mach3 settings will result in no 360 degree "circular" rapids or feed moves below the surface of the stock with the attached model?

Thanks. I have been struggling with this for way too long.
-- Dean
(just a hobbyist trying to create some art)

[JOM]

Dean,

This is due to the angular coordinates of the output code is set to absolute.
There are two ways to change this.

1) Run the simulator and CLICK on the options button. Change the "5-axis angles" from absolute to continuous.

2) It is possible to edit the post processor and add * ANGLE_OUTPUT * to the post processor. (see example below)
:
* CUTTER_REFERENCE *
TIP
* TOOLPATH_OUTPUT *
TRANSFORM
* ANGLE_OUTPUT *
CONTINUOUS <== Set the angle output to continuous
* RAPID *
G00 "x" "y" "Z" "a"
* END_SECTION *
:

Joakim

[dwneumann]

thank you Joakim!
Setting * ANGLE_OUTPUT * to CONTINUOUS does not appear to work for me however setting the "5-axis angles" to "continuous" on the simulator options dialog does fix the problem. I am milling continuous 4-axis (hooray!)
Best regards,
Dean