getting the XYZ (A table) machine profile to load

[jwhalin]

Last September I bit the bullet and bought a 3 year subscription to Fusion 360 when the free version was "adjusted". Mainly, so I could continue to import my old SolidWorks files and also for the A axis rotary table control. This week, I had a need to use the rotary table to make a large flange and bolt pattern that would not fit on the teensy 5" x 11" x-y table of my mini-mill. I went to the "Machine Library" and selected "Autodesk Generic 4-axis (A Table)" and tried to drag it onto the "local" tab.  This is what it returned; "Cannot perform copy on invalid machine asset!" I have no idea what this means or how to load the profile to control MACH3. I could use a push in the right direction. Thanks, Jeff

[engineguy]

@jwhalin 

You do not need to have a Machine Configuration to do 4th axis job, don`t "set" a machine in your Setup, just use the correct Post Processor, a sample PP for Mach3 that works with an A axis set in either the X or Y axis, selectable by the user.

Sample PP attached.

[jwhalin]

Thanks for the help.. I'll give it a try. Jeff

[jwhalin]

Following your suggestion, I deleted the Generic XYZ profile from the “machine Library” and specified the new “post processor” file you provided (Thanks again BTW).

Test;

I modeled  a 6 inch diameter disk .5 inch thick and patterned (5) .375” holes on a 5.5 inch bolt circle and a .5 inch center hole.

Next I opened the “manufacturing” window and defined a drilling “setup” with the center hole as the WCS and “Z” up and selected one hole. (When I select all the holes it just moves XY and drills.)

Then the wheels came off my wagon… Clearly, I’m clueless as to the proper way to address the fourth axis.

I don’t see any command where I can tell the “A” axis to rotate 72 degrees and duplicate the drill cycle “n” times.

(If I were writing the gcode I would just add G1 A72 F25 between the drill code and add 72 (144, 216…) degrees to the next drill cycle. )

If I click on the “multi-Axis” icon it wants to start a 7 day free trial.

[engineguy]

@jwhalin 

Just upload the file, much easier to see what has been done. Are the holes on the face of the plate or are they drilled around the circumferance ??

How is your 4th axis fixed on your CNC machine, does it rotate around the X or Y axis or are you trying to do this with the 4th axis sitting horizontal on the bed ??

[jwhalin]

The rotary table is parallel to the table with its rotation around the "Z" axis. What I want to do is move the table to a hole location on one axis ( say X) and index the table to locate and drill the remaining holes around the perimeter by rotation vs XY. I'm not trying to do any fancy 4 axis interpolation. 

[engineguy]

@jwhalin 

Jeff, that is what I thought you were after.

If you have a paid for subscription you should have the "Rotary" function available to you, I don`t have that so not able to show how to do what you want using it.

The really rough/painful/simplistic way is to use the "Manual NC" and Create a "Pass Through" of the code to make the move as you have already worked out, something like this :-

G01 G91 A72 F25

G0 G90

Code snippet below

(DRILL1)
N5 M5
N6 T10 M6
(10MM SUS DRILL JOBBER)
N7 S5000 M3
N8 G54
N9 M8
N10 G0 X60. Y0.
N11 G43 Z15. H10
N12 Z5.
N13 G98 G81 X60. Y0. Z-12. R5. F1000.
N14 G80
N15 Z15.
N16 G01 G91 A72 F25
N17 G0 G90

(DRILL1 2)
N18 G0 X60. Y0.
N19 Z15.
N20 Z5.
N21 G81 X60. Y0. Z-12. R5. F1000.
N22 G80
N23 Z15.
N24 G01 G91 A72 F25
N25 G0 G90

As there is a G01 G91 (Incremental) move then it will need a G90 to get back to Absolute otherwise all your Height moves will be at the F25, as it is Incremental you only need to input the 72 because you are telling it to move 72 degrees, not "go to 72 degrees"

See attached Code file and example file using the Pass through. Just a PITN suggestion that will work if all else fails 🙂

Apologies, that`s all I have 😞

[Anonymous]

If the post was setup correctly would tool orientation work?

Jason