Indexing help

[Threept82]

Hi guys.

I am modifying a program for a shorter cycle time.

it is in a indexing form not a full rotary. When I post I get a "ctable" alarm and need to say OK about 300 times.(not kidding).

When it does post out it only post the indexing in whole numbers. I am using about 8 rotation locations of which one of them is at A202.5

 

The post outputs A202 goes to a location ,outputs A203. posts the next line then outputs A202 and so on and so on.

 

Any help will be great

Thanks

[Threept82]

No rotary Gurus out there?

[JayM]

It sounds like your A axis in the Machine Definition is configured for positioning with the angle set to 1 degrees.

[cadcam]

What Machine Def are you using and how did set the planes?

Can you share the file?

[Jayson Kramer]

Ya what Cadcam said.

[Guest]

Have you tried changing your indexing value in the machine def to something like .1

 

The default is I believe 5 degrees

[Threept82]

I am using Mastercam X

I do not see an indexing option in the machine def and I am using the standard generic 4 axis mill def.

[Guest]

in the properties of the Rotary axis component

 

VMC A Axis, right click properties, Fixed Continuous Interposition, place a smaller value in that box

[Threept82]

John, worked awesome.

 

Was wondering if you ever saw output like this?

 

All seems to post good except for when it works on this angle.

Then it posts out as shown until the end of the tool. (Which is the longest of the program)

 

 

N9326 T9 M6

N9328 M11

N9330 A203

N9332 M10

N9334 G0 G90 X-2.028 Y.8037 S2800 M3

N9336 G43 H9 Z6. M8

N9338 M11

N9340 A203

N9342 M10

N9344 Z.87

N9346 M11

N9348 A203

N9350 M10

N9352 G1 Z.414 F12.

N9354 M11

N9356 A203

N9358 M10

N9360 Y.7737 F6.

N9362 M11

N9364 A203

N9366 M10

N9368 Y.7151 Z.4942

N9370 M11

N9372 A203

N9374 M10

N9376 Y.667 Z.5499

N9378 M11

N9380 A203

N9382 M10

N9384 Y.614 Z.6017

N9386 M11

N9388 A203

N9390 M10

N9392 Y.5566 Z.6491

N9394 M11

N9396 A203

[Guest]

Is the toolpath something different on this position?

 

Check your toolpath settings, see if you have rotary enabled, if you do, try disabling it

[Threept82]

it was not enabled. I enabled it and posted the same either way.

[Guest]

If you want to send a z2g my way I'll take a peek and see if anything jumps out. My thought is it's toolpath related because everything else posts OK but beyond that, tough to say

[Threept82]

using your S4A email?

[htm01]

using your S4A email?

S4A is now cimquest but JP's not there anymore

[Guest]

I can always be contacted at

 

jmparis65 at gmail dot com

[Threept82]

File sent.

and thanks

[Guest]

Ken,

 

This is the end of your tool 9 as I post it in X7, looks like you're on X3 which I don't have

 

N2542 Z.87

N2544 G1 Z.414 F12.

N2546 Y.7737 F6.

N2548 Y.7151 Z.4942

N2550 Y.667 Z.5499

N2552 Y.614 Z.6017

N2554 Y.5566 Z.6491

N2556 Y.4955 Z.6915

N2558 Y.4312 Z.7284

N2560 Y.3646 Z.7596

N2562 Y.2963 Z.7849

N2564 X-.6788 Y.2681 Z.7935

N2566 X-.6813 Y.2398 Z.8012

N2568 X-.6887 Y.1904 Z.8121

N2570 X-.6985 Y.1452 Z.8196

N2572 X-.7103 Y.1018 Z.8245

N2574 X-.7234 Y.0604 Z.8272

N2576 X-.7365 Y.0235 Z.8279

N2578 X-.7488 Y-.0085 Z.8273

N2580 X-.7602 Y-.0363 Z.8259

N2582 X-.7708 Y-.0608 Z.8238

N2584 X-.7808 Y-.0829 Z.8214

N2586 X-.7903 Y-.103 Z.8187

N2588 X-.7993 Y-.1213 Z.8158

N2590 X-.8078 Y-.1379 Z.8129

N2592 X-.8158 Y-.153 Z.8099

N2594 X-.8233 Y-.1667 Z.807

N2596 X-.8305 Y-.1792 Z.8041

N2598 X-.8441 Y-.2009 Z.7987

N2600 X-.857 Y-.2189 Z.7938

N2602 X-.8701 Y-.2327 Z.7897

N2604 X-.8767 Y-.2375 Z.7882

N2606 X-.8835 Y-.2406 Z.7872

N2608 X-.89 Y-.2416 Z.7869

N2610 X-.8967 Y-.2406 Z.7872

N2612 X-.9032 Y-.2376 Z.7882

N2614 X-.9094 Y-.2331 Z.7895

N2616 X-.9211 Y-.2211 Z.7931

N2618 X-.9328 Y-.2056 Z.7975

N2620 X-.945 Y-.1867 Z.8023

N2622 X-.9581 Y-.1643 Z.8075

N2624 X-.9651 Y-.1514 Z.8103

N2626 X-.9725 Y-.1374 Z.813

N2628 X-.9804 Y-.122 Z.8157

N2630 X-.9887 Y-.105 Z.8184

N2632 X-.9975 Y-.0864 Z.821

N2634 X-1.0069 Y-.066 Z.8233

N2636 X-1.0168 Y-.0434 Z.8253

N2638 X-1.0272 Y-.0185 Z.8269

N2640 X-1.0307 Y-.0099 Z.8273

N2642 X-1.0382 Y.0094 Z.8278

N2644 X-1.05 Y.0413

N2646 X-1.0624 Y.078 Z.8263

N2648 X-1.0747 Y.1193 Z.8228

N2650 X-1.0859 Y.1638 Z.8168

N2652 X-1.0945 Y.2087 Z.8084

N2654 X-1.0999 Y.2519 Z.798

N2656 X-1.102 Y.2963 Z.7849

N2658 Y.3646 Z.7596

N2660 Y.4312 Z.7284

N2662 Y.4955 Z.6915

N2664 Y.5566 Z.6491

N2666 Y.614 Z.6017

N2668 Y.667 Z.5499

N2670 Y.7151 Z.4942

N2672 Y.7737 Z.414

N2674 Y.8037

N2676 G0 Z6.

N2678 M5

N2680 G91 G28 Z0. M9

N2682 G28 X0. Y0.

N2684 A0

N2686 M30

%

 

[Colin Gilchrist]

This is a 5X post, correct? If so, disable 'brk_mv_head'. (set it to '0')

 

That variable is causing large rotations (moves between tool planes) to be broken into multiple moves.

 

The breaking of the moves is fine, it usually prevents crashes when repositioning, but the constant Unlock, Move, Lock, Unlock, Move, Lock is a pain.

 

We have a project to revise the locking/unlocking logic during these break moves, so that it Unlocks once, makes all the required broken reposition moves, and then locks the rotaries.

[Guest]

Colin, no vintage Fanuc 4 ax

[Guest]

OK, it is an original V10 Generic Fanuc 4 axis post

 

Something is amiss, I updated it to X7 and it still posts good code on my end.......

 

In my position, there isn't much more I can do.....

[Threept82]

This is "X" (oldie) and it its the generic fanuc 4 axis

[John Summers]

If the index position can go to .5 degrees, change the FS format statement of the indexer -- for instance: FS 6 1.15(ltn...)

The last number 5 is the fractional format of the previous position (the 'tenths' position). This can be a 5 or a 2 (2 tenths of the previous place).

In this case the indexer FMT statement will refer to FS 6.