indexing

[KMartin]

Hi Everyone - I would really appreciate some help ith this part that needs to be done asap .

I'm using a Vertical machine and holding the part in the 4th axis . I have made the toolpath

and I need to index the A axis . Would I be able to use a sub program to index . I haven't

had much experience with sub programs . Any help would be appreciated .The part is in the

X5 directory under part 44 .

 

Thanks in advance .

[Manuel0822]

What control are you working with? If it is a Fanuc or a Haas, you could use the subprogram as you wish, you can post your program and save as O0002 for an example, then at the and of your posted program, add a line reading "G0 G91 A6." as it seems like you have a 6 deg spacing.

 

Check this example:

 

%

O0002(GROOVE MACHINING INDEX SUBPROGRAM)

G0 G90 X-3.3845Y-4.4787

Z0.

G1G41D20X-2.885Y-4.456F20.

X-3.0162Y-1.5704

G3X-3.1161Y-1.4749R.1

X-3.1206Y-1.475R.1

G1G40X-3.3704Y-1.4864

G0X-3.3705Y-4.478

G1G41D20X-2.871Y-4.4553

X-3.0022Y-1.5697

G3X-3.1021Y-1.4743R.1

X-3.1066Y-1.4744R.1

G1G40X-3.3564Y-1.4857

(*************************************)

(PROGRAM CUT FOR LENGTH)

(*************************************)

G1G41D20X-2.6872Y-4.447

X-2.8184Y-1.5614

G3X-2.9183Y-1.4659R.1

X-2.9228Y-1.466R.1

G1G40X-3.1726Y-1.4774

G0X-3.1847Y-4.4696

G1G41D20X-2.6852Y-4.4469

X-2.8164Y-1.5613

G3X-2.9163Y-1.4658R.1

X-2.9208Y-1.4659R.1

G1G40X-3.1706Y-1.4773

G0 X-3.3845Y-4.4787

(*************************************)

(ADD INDEX HERE)

(*************************************)

G0 G91 A6.

G90

(*************************************)

(*************************************)

M99

%

 

So you load this subprogram on the controller and then make another empty program that calls YOUR SUBPROGRAM AS SHOWN:

 

%

O0001(0299D354)

(DATE=DD-MM-YY - 13-09-11 TIME=HH:MM - 19:00)

(MCX FILE - C:\USERS\MANUEL\DOWNLOADS\PART 44.MCX-5)

(T20|COLLET -60 DEGREE FLYCUTTER|H20|D20|WEAR COMP|TOOL DIA. - 4.305|XY STOCK TO LEAVE - .01|Z STOCK TO LEAVE - 0.)

G20

G0G17G40G49G80G90

(SINGLE TOOTH)

T20M6

G0G90G54X-3.3845Y-4.4787A0.S2500M3

G43H20Z3.

Z0.

(*************************************)

(CALL SUBPROGRAM HERE)

(*************************************)

(SUBPROGRAM WILL LOOP 60 TIMES TO MAKE 60 CUTS)

M98 P0002 L60

(*************************************)

G0Z3.

M5

G91G28Z0.

G28X0.Y0.

M30

%

 

Now before you run any of this make sure you have enough clearance with your tool before the indexing. Also you may want to run Air on the Looping as without testing it I could make a mistake on the count.

 

Hope it helps.

[KMartin]

Manuel0822 Thanks for the help . Much appreciated .Buy the way I'm running a Hasss .

[neurosis]

Manuel0822 has given probably the most practical method. I wouldnt hesitate to use it!

 

However,

 

Im lazy and dont like to hand write any code if I do not have to. I like to just post and go. That way if I need to make changes to the program for any reason in the future I can just make the changes, re-post, and go!

 

I put a file on the ftp called PART 44transform.MCX-5.

 

I had to select a different Machine Def that supports a rotary axis. If you look at the file you will see what ive done. I used your tool path and transformed/rotated it around the Left Side Rotation view. Its tricky to get Mastercam to post a transform/rotate operation without posting a new fixture offset for every rotation. I had to change the work offset number in the view manager for TOP to 0 rather than -1.

[Manuel0822]

Yep, That's the the nicest way of doing it.

 

Calling a subprogram will work just fine specially if you don't work as much experience using rotary axis paths or transform as Neurosis shows. It will also work just fine if you don't have a full 4th axis machine,let's say you have one of the old times Haas Indexers with a control box outside the machine, you would then just change your "G0 G91 A6."" line for whatever M code controls the outside box.

 

Anyways Neurosis Methods is the way I would go, easiest to update, verify & no messing around counting loops

[K2csq7]

Kevin, I would be careful using transform, there have been a few complaints here on the forum recently.

On the other hand I still use it fairly often ... A forum search for transform showed 80 results, here are the two I recognize.

 

bit by transform

 

transform bug

 

I don't know if you will be using the same methods, Just an FYI.

[neurosis]

Keith,

 

That first link that you posted, I probably should have followed up on once I got the final response from QC but I wasnt sure what to say since I was given a very basic explanation. It was not an issue with the transformed operation. It was an issue with the Optirough tool path. I am not sure what the problem was that caused the gouging but they said that they tested in X6 and the issue appeared to be fixed. I wish that I could give more information but that was all that was given to me.

 

I have had several issues with Transform operations but never with something that is this simple. This particular part would be very easy to double check the program to make sure things looked correct.

[K2csq7]

Good to hear. I didn't have the time to look into his file, just wanted to throw it out there.

I use transform for subs frequently, but only simple stuff (easy to double check) as well.

[KMartin]

Thanks everyone for the help .I just ended up using

a sub program . The parts were in high demand - as usual .

Next time I will try the transform .

 

Thanks again .