Fanuc 5x, NO A-C Indexing

Anonymous · ‎08-24-2017

Need help to set up the generic Fanuc post processor.

Already try different modifications with notepad++, but can get it to code the indexing angles on A-C axis.

Here the output code:

N22 G54
N24 G68.2 X0. Y0. Z0. I90. J0. K90.
N26 G53.1
N28 M08
N32 G00 X1.3245 Y6.5313

But need to index the trunnion first, something like this:

G0 G54 G90 A-90. C180.
G68.2 X0. Y-25. Z-20. I180. J-90. K0
G53.1
G0 X0 Y0
G0 G43 H01 Z100.

Need help to get the A and C indexing angle to output by the Fanuc Post. (Doosan, DNM350/5x, Fanuc 31iB).

Any help would be greatly appreciated.

Thank you

bob.schultz · ‎08-30-2017

You can index the rotary axes prior to the G68.2 block by adding the following lines to the defineWorkPlane function.

      if (useMultiAxisFeatures) {
        if (_setWorkPlane) {
          abc = getWorkPlaneMachineABC(_section.workPlane);
          gMotionModal.reset();
          writeBlock(
            gMotionModal.format(0),
            conditional(machineConfiguration.isMachineCoordinate(0), "A" + abcFormat.format(abc.x)),
            conditional(machineConfiguration.isMachineCoordinate(1), "B" + abcFormat.format(abc.y)),
            conditional(machineConfiguration.isMachineCoordinate(2), "C" + abcFormat.format(abc.z))
          );
        }
        var eulerXYZ = _section.workPlane.getTransposed().eulerZYX_R;
        abc = new Vector(-eulerXYZ.x, -eulerXYZ.y, -eulerXYZ.z);
        cancelTransformation();

Bob Schultz
Sr. Post Processor Developer

Aadithya01 · ‎08-30-2017

Hey Bob ,

Just did the procedure which you had told to @Anonymous ... And now I my cnc output program is like the

(DRILL4)
N30 T4 M06
N35 S5000 M03
N40 G54
N45 G00 A90. C180.
N50 G68.2 X0. Y0. Z0. I90. J0. K0.
N55 G53.1
N60 M08
N70 G00 G43 X-59.881 Y-17.049 Z65.8 H04
N80 G00 Z55.8
N85 G98 G83 X-59.881 Y-17.049 Z29.05 R55.53 Q2. F1000.
N90 G80
N95 Z65.8

All I wanted was the A and C axis which is perfectly coming out right now . But now how to remove the G68.2 I J K line cause now I dont want that . Can you please tell me which part of the .cps program should I remove now

Laurens-3DTechDraw · ‎08-31-2017

@Aadithya01 wrote:

Hey Bob ,

Just did the procedure which you had told to @Anonymous ... And now I my cnc output program is like the

(DRILL4)
N30 T4 M06
N35 S5000 M03
N40 G54
N45 G00 A90. C180.
N50 G68.2 X0. Y0. Z0. I90. J0. K0.
N55 G53.1
N60 M08
N70 G00 G43 X-59.881 Y-17.049 Z65.8 H04
N80 G00 Z55.8
N85 G98 G83 X-59.881 Y-17.049 Z29.05 R55.53 Q2. F1000.
N90 G80
N95 Z65.8

All I wanted was the A and C axis which is perfectly coming out right now . But now how to remove the G68.2 I J K line cause now I dont want that . Can you please tell me which part of the .cps program should I remove now

Can we move this question to a new thread?

Because the Topic starter wants the G68.2.

And removing that means the machine has no multi-axis features which is much easier to set in the post.

Laurens Wijnschenk
3DTechDraw

AutoDesk CAM user & Post editor.
René for Legend.

Aadithya01 · ‎08-31-2017

Hey Laurens ,

You can move that post definitely to a new thread .. I have no problem with that..

Anonymous · ‎08-31-2017

Thank you, Bob.

Will try this ASAP, for what I can see from the other member comments it will work.

Thank you!.

bob.schultz · ‎08-31-2017

@Aadithya01 wrote:

Hey Bob ,

Just did the procedure which you had told to @Anonymous ... And now I my cnc output program is like the

(DRILL4)
N30 T4 M06
N35 S5000 M03
N40 G54
N45 G00 A90. C180.
N50 G68.2 X0. Y0. Z0. I90. J0. K0.
N55 G53.1
N60 M08
N70 G00 G43 X-59.881 Y-17.049 Z65.8 H04
N80 G00 Z55.8
N85 G98 G83 X-59.881 Y-17.049 Z29.05 R55.53 Q2. F1000.
N90 G80
N95 Z65.8

All I wanted was the A and C axis which is perfectly coming out right now . But now how to remove the G68.2 I J K line cause now I dont want that . Can you please tell me which part of the .cps program should I remove now

Your's is a much easier change. Just change the useMultiAxisFeatures variable to false where it is defined at the top of the post processor.

// fixed settings
var firstFeedParameter = 500;
var useMultiAxisFeatures = false;

Bob Schultz
Sr. Post Processor Developer

Anonymous · ‎09-04-2017

Bob,

Made some changes to the post.

Here what we have so far:

(2D CONTOUR1)
N30 T3 M06
(2 FLUTE FLAT ENDMILL)
N35 S5000 M03
N40 G54
N45 G00 A-90. C0.
N50 M08
N60 G00 X0.929 Y-8.4
N65 G43 Z1.2495 H03
N70 G01 Z-0.2505 F20.
N75 G03 X0.9173 Y-8.3923 I-0.0117 J-0.005 F40.
N80 G01 X-1.0827
N85 G03 X-1.0944 Y-8.4 J-0.0127
N90 G01 Z0.9995
N95 G00 Z1.1995
N105 G28 G91 Z0.
N110 G90

(SWARF1)
N120 G00 X0.9258 Y-8.4036
N125 G43.4 Z0.9814 H03
N130 G00 A-91.12 C-2.763
N135 X0.9407 Y-8.3976 Z0.6716
N140 G01 Z0.4997 F20.
N145 Z0.3278
N150 Z0.1559
N155 Z-0.016
N160 Z-0.1879
N165 Z-0.3597
N170 X0.939 Y-8.3917 Z-0.4299 A-91.577 C-2.566 F40.
N175 X0.938 Y-8.3888 Z-0.4613 A-91.774 C-2.406

The contour works that way, don't need the G68.2.

The problem is the Swarf the bottom Z is Z-.250 but toolpath goes way below to around Z-.680.

On machine simulation works, but the post will do the wrong Z values.

Need help to solve this, I think my postprocessor is almost ready.

Thank you

Laurens-3DTechDraw · ‎09-04-2017

@Anonymous wrote:

Bob,

Made some changes to the post.

Here what we have so far:

(2D CONTOUR1)
N30 T3 M06
(2 FLUTE FLAT ENDMILL)
N35 S5000 M03
N40 G54
N45 G00 A-90. C0.
N50 M08
N60 G00 X0.929 Y-8.4
N65 G43 Z1.2495 H03
N70 G01 Z-0.2505 F20.
N75 G03 X0.9173 Y-8.3923 I-0.0117 J-0.005 F40.
N80 G01 X-1.0827
N85 G03 X-1.0944 Y-8.4 J-0.0127
N90 G01 Z0.9995
N95 G00 Z1.1995
N105 G28 G91 Z0.
N110 G90

(SWARF1)
N120 G00 X0.9258 Y-8.4036
N125 G43.4 Z0.9814 H03
N130 G00 A-91.12 C-2.763
N135 X0.9407 Y-8.3976 Z0.6716
N140 G01 Z0.4997 F20.
N145 Z0.3278
N150 Z0.1559
N155 Z-0.016
N160 Z-0.1879
N165 Z-0.3597
N170 X0.939 Y-8.3917 Z-0.4299 A-91.577 C-2.566 F40.
N175 X0.938 Y-8.3888 Z-0.4613 A-91.774 C-2.406

The contour works that way, don't need the G68.2.

The problem is the Swarf the bottom Z is Z-.250 but toolpath goes way below to around Z-.680.

On machine simulation works, but the post will do the wrong Z values.

Need help to solve this, I think my postprocessor is almost ready.

Thank you

Without G68.2 you will need to program from the A and C axis center of rotation.

With G68.2 you can put your work offset anywhere you want.

Laurens Wijnschenk
3DTechDraw

AutoDesk CAM user & Post editor.
René for Legend.

bob.schultz · ‎09-05-2017

@Anonymous wrote:

Bob,

Made some changes to the post.

Here what we have so far:

(2D CONTOUR1)
N30 T3 M06
(2 FLUTE FLAT ENDMILL)
N35 S5000 M03
N40 G54
N45 G00 A-90. C0.
N50 M08
N60 G00 X0.929 Y-8.4
N65 G43 Z1.2495 H03
N70 G01 Z-0.2505 F20.
N75 G03 X0.9173 Y-8.3923 I-0.0117 J-0.005 F40.
N80 G01 X-1.0827
N85 G03 X-1.0944 Y-8.4 J-0.0127
N90 G01 Z0.9995
N95 G00 Z1.1995
N105 G28 G91 Z0.
N110 G90

(SWARF1)
N120 G00 X0.9258 Y-8.4036
N125 G43.4 Z0.9814 H03
N130 G00 A-91.12 C-2.763
N135 X0.9407 Y-8.3976 Z0.6716
N140 G01 Z0.4997 F20.
N145 Z0.3278
N150 Z0.1559
N155 Z-0.016
N160 Z-0.1879
N165 Z-0.3597
N170 X0.939 Y-8.3917 Z-0.4299 A-91.577 C-2.566 F40.
N175 X0.938 Y-8.3888 Z-0.4613 A-91.774 C-2.406

The contour works that way, don't need the G68.2.

The problem is the Swarf the bottom Z is Z-.250 but toolpath goes way below to around Z-.680.

On machine simulation works, but the post will do the wrong Z values.

Need help to solve this, I think my postprocessor is almost ready.

Thank you

Hello Antonio,

It looks as if you are not using TCP on the control, in this case make sure you set the post processor to modify the output points for the table rotation.

function onOpen() {
...
optimizeMachineAngles2(1); // disable TCP mode
...
function getWorkPlaneMachineABC(workPlane) {
...
var tcp = false;

and like @Laurens-3DTechDraw mentioned, the origin (0, 0) must be programmed at the table center.

Bob Schultz
Sr. Post Processor Developer

Community

Fanuc 5x, NO A-C Indexing

Fanuc 5x, NO A-C Indexing

Fanuc 5x, NO A-C Indexing