Rotary post question

[MIKE_B]

Hi all!

 

I need to have my post put out an M11 to tell my indexer to rotate. Can anyone tell me how or where in my post I need to put this?

Here is a sample program. I need the M11 after the G80's

 

Thanks

Mike

 

 

N110 T1 M6

N120 G0 G90 G54 X-1.7507 Y1.19 S2500 M3

N130 G43 H1 Z4.

N140 G98 G81 Z2.315 R2.475 F10.

N150 Y0.

N160 Y-1.19

N170 X-4.2507

N180 Y0.

N190 Y1.19

N200 X-6.7505

N210 Y0.

N220 Y-1.19

N230 X-9.25

N240 Y0.

N250 Y1.19

N260 G80

( 90° )

N270 G0 G55 X-9.25 Y-1.19

N280 Z4.

N290 G98 G81 Z2.315 R2.475 F10.

N300 Y0.

N310 Y1.19

N320 X-6.7505

N330 Y0.

N340 Y-1.19

N350 X-4.2507

N360 Y0.

N370 Y1.19

N380 X-1.7507

N390 Y0.

N400 Y-1.19

N410 G80

( 180° )

N420 G0 G56 X-1.7507 Y-1.19

N430 Z4.

N440 G98 G81 Z2.315 R2.475 F10.

N450 Y0.

N460 Y1.19

N470 X-4.2507

N480 Y0.

N490 Y-1.19

N500 X-6.7505

N510 Y0.

N520 Y1.19

N530 X-9.25

N540 Y0.

N550 Y-1.19

N560 G80

( 270° )

N570 G0 G57 X-9.25 Y-1.19

N580 Z4.

N590 G98 G81 Z2.315 R2.475 F10.

N600 Y0.

N610 Y1.19

N620 X-6.7505

N630 Y0.

N640 Y-1.19

N650 X-4.2507

N660 Y0.

N670 Y1.19

N680 X-1.7507

N690 Y0.

N700 Y-1.19

N710 G80

N720 M5

N730 G91 G28 Z0.

N740 G28 Y0.

N750 G90

N760 T1 M06

N770 M30

%

[Guest]

Mike,

 

Where is the address for the axis.

 

I don't see and A90. or even B90.

 

What tells the program what axis IS going to move

[Guest]

Here's something you could do, assuming this a "Hardinge" type indexer.

 

set up something like this in the pcanceldc$

section of your post.

 

code:

---

if mr1$ = 1, pbld, n$, "M11", e$

---

Place that after the G80 line in the pcanceldc$ section and set

 

code:

---

[misc reals]

1. "M11 Output 0=no, 1=yes"

---

Something like that should work for you

 

Then whenever you create a drill cycle and you know you're going to want to rotate, go onto the Misc Ints page set mr1 to 1 and after it reads the G80 it will output an M11

[MIKE_B]

John

 

It is a haas indexer with its own control that

I have to program by hand. All I need my main program to do is send signal (M11) for it to index. I was thinking something in the canned text parameters could do this could do this??

[Guest]

Canned text will get it into the program certainly, positioning it using canned can be a PITA if you need it in certain spots.

 

The example above will give to you where you need and only when you want it.

 

If you're not sure where to plug it in email me I'll get in place for you, then you can try it and see if it works for you

[MIKE_B]

Thanks Joun I'll give it a shot and let you know.

[Bruce Gibson]

mike,

change the "lock codes" in the rotary setting in your post from a 0 to a 1

[MIKE_B]

John

 

Thanks alot that was exactly what I needed!

 

Saved me alot of editing

[Guest]

Glad I could help

 

 

Won't work for him Bruce. His axis movement is being generated outside of MC by a seprate indexer the M11 for him is simply a trigger.

[Bruce Gibson]

ok

[PeterM]

M11 is no doubt a miscellanius code, typically m21 or m20. I think that the new mp master post has a switch to output this. check it out. Peter

[MIKE_B]

John

 

After getting a little deeper in my program I noticed I need the M11 after the clearance plane.

 

This is what I get now:

G80

M11

G0 Z4.

 

This is what I need

G80

G0 Z4.

M11

 

Any suggestions?

Thanks

Mike

[Guest]

I'm winging I don't have time to test it so try this

 

move that added line fromt teh pcanceldc$ to the end of the pdrlcommonb section.

 

If that does not work the other thing you could try is to insert that added line of code in right after the pdrlcommonb line in all of your drill cycle callouts.

[MIKE_B]

Thanks I'll give it a shot

[PeterM]

This is the code I mentioned in the latest MPMASTER post

 

 

use_rotmcode : 1 #Output M-Code for Axis direction (sindx_mc)

#0 = Signed direction (only valid when rot_type = 1)

#1 = M-Code for direction

 

This is the output result

 

CONTOUR....)

(OVERALL MAX - Z.1)

(OVERALL MIN - Z-.0525)

G00 G17 G20 G40 G80 G90

N1 T1 M06 ( 1/2 FLAT ENDMILL)

(MAX - Z.1)

(MIN - Z-.0122)

G00 G90 G55 X-.19 Y.4012 M22 A-15. S955 M03

G43 H1 Z.1 T2

G01 Z-.0122 F50.

G41 D1 X-.47 F5.

Y-.1512

G40 X-.19

G00 Z.1

M05

 

 

note the M22

It should be a piece of cake to change the output to be M11(A___)

 

 

_____________________

Peter Martin

mcam 3... - x - mill level 3

Senior Programmer/Milling Supervisor

Preci Mfg.

400 Weaver St. Winooski VT 05468

email [email protected]

[Paul Decelles]

I would recommend looking at pindex, pcout and pfcout in your post. It appears to me that someone modified one of these postblocks to output the angle as a comment rather than as an "A" or "B" position. You will want to add the "M11" to whichever postblock is outputting this information so that it properly appears anytime the angle changes. Check the initialization of the variable index towards the top of the post. If it is set to 0 then you most likely need to look in pcout and pfcout. If it is set to 1 then you need to look in pindex (note: the setting of index is determined by the rotary axis definition in the MD when using the new Generic Fanuc 4X post).

[Guest]

quote:

---

It appears to me that someone modified one of these postblocks to output the angle as a comment rather than as an "A" or "B" position.

---

Paul, he is not outputting an angle with his post, those are added comments. He has a programmable indexer hooked up to his machine. He does not need the anlge output. He is looking to generate a simple M11 to trigger his programmed indexer to rotate.

 

Does not need to output angular info as it is programmed in his indexer

[Paul Decelles]

Ok, let me get this straight... He is already hand editing every NC file to put in the (ANG)? If that is an acceptable solution, why not simply hand type M11 (ANG)?

Wouldn't life be easier if the post did what I said? Output the angles as M11 (ANG) right in pindex?

Adding the M11 output to pcanceldc$ means that he is going to get an M11 at the end of every drill cycle he posts whether he needs it or not. That ought to work great the next time he programs a drill cycle that doesn't have any rotation. Oh wait, he can always go in and hand edit every single NC file he posts from now on to remove the M11's he does not need... Somehow I think most of you would find this unacceptable.

I programmed Haas and SMW indexers that worked exactly like this before I left the shop and came over to the software side of things. The posts I used then were modified to not only do what I said above, they also spit out a seperate file containing a list of the angle moves to make it easier to program the indexer control (which is done by hand).

[Guest]

Mike_B would have to answer that Paul.

 

I do know from talking to him thru email that he programs his indexer seperate from Mastercam and uses MC to program his drill cycles, thus he needs and M11 only to tell his indexer to rotate.

[Paul Decelles]

I can see hand editing a single NC file for a couple of rotations but eventually a job will pop up requiring a lot of hand editing - and that's when human error comes into play and machines crash.

[Guest]

Paul,

 

That's the point, his rotations do not come out of Mastercam. Those (ang) you see are notes so he knows where he is in the program, not actual rotations.

[MIKE_B]

Paul

 

John's suggestion worked great. But you are correct there were a few M11's I did have to go in and delete because I did not want it to rotate when I had a tool change. I want the next tool to work at the last rotation. I'm a little busy today but I will take a look at what you suggested

 

Thanks

Mike