Multiple Work Offsets

[9 1/2]

Hey Gang,

Just finishing up my last year in school and learning tons. Asked my instructor how to post multiple work offsets and he didn't really know.


anywho,....... what I want is to build the part and have it posted for 3 vice (54 55 56) Currently I copy all the needed operations into a new tool path group and select planes, then 1 (for 55) 2 or 3 etc etc for all three offsets.

This produces the correct posting but each part is completed one at a time. No good. It needs to post each opp once for each offset (ie: spot drill at 54 55 then 56 then drill 54 55 56 etc etc) eliminating excessive tool changes.

To copy each operation three times for each off set and change the planes individually seems cumbersome and ripe for an error.

Gibbs cam has an input field for "Number of vice" which in turn posts offsets for each opp for each vice...........
Any help out there? I'd be greatly indebted to you all AND a rock star in class!!

Owen

[thebowman]

Owen,

"This produces the correct posting but each part is completed one at a time. No good. It needs to post each opp once for each offset (ie: spot drill at 54 55 then 56 then drill 54 55 56 etc etc) eliminating excessive tool changes."

Take a look at Transform Toolpath.

On the first page on the bottom left of the Transform Toolpath dialog you will see where you can choose:

Group NCI Output By:

1. Operation Order

2. Operation Type

From what you described that you want to do you need to use: Operation Type.

From The Mastercam On-Line Help:

"Operation type-> Groups the transformed operations by the operation type. For example, if you selected a pocket and a contour operation, all transformations of the pocket operation would be executed together, as would all transformations of the contour operation (pocket, pocket, contour, contour, etc.)"


"To copy each operation three times for each off set and change the planes individually seems cumbersome and ripe for an error."

I agree that it's "cumbersome and ripe for an error". It's also not associative.

Take a look at the first page of the Transform Toolpath dialog box. On the bottom right you will see:

Work Offset Numbering

0 = G54
1 = G55
2 = G56

etc.

[9 1/2]

Thank you so much!
I had to experiment with the options contained within the Transform tool path dialogue but finially got it sorted out.

Monday I'll put this to the class, I'm assuming my instructor either didn't understand what I was asking or wanted me to dig a bit on my own. Well I hope asking here would be considered "digging"

Peace.
owen

[psychomill]

Also,...

if you have a post that supports sub programming for multiples, you can have a single file/single part program and output for as many vices as you need.

Just another option....

[9 1/2]

Thanks physco but, I don't believe this post does or if it does I don't know how or where to sellect that option.
The Gibbs post we use has that option. I take a look again and see if I've over looked some thing.

[thebowman]

Originally Posted by 9 1/2 Thank you so much! I had to experiment with the options contained within the Transform tool path dialogue but finially got it sorted out. Monday I'll put this to the class, I'm assuming my instructor either didn't understand what I was asking or wanted me to dig a bit on my own. Well I hope asking here would be considered "digging" Peace. owen

You're quite welcome.

One important thing I forgot to mention is on the first page and listed as:

Method:

Toolplane

Coordinate

Make sure you understand why you would choose Toolplane vs. Coordinate.


Finally, a few pieces of advice if I may based on my 2 years of real world experience using Transform toolpath to make parts with.

1. Experiment with all the options in Transform Toolpath to see what they do.

2. Tranform Toolpath is an area of Mastercam that I feel is often very buggy especially Transform Mirror where my advise to you is to *always* 100 precent check what Transform Mirror gives you as it often does some strange things on its own like reversing chains where it shouldn't.

I have found that often in Mastercam when I don't get what I know I should be getting I close Mastercam and restart it. It's truly amazing to me how many problems this solves. This applies to all versions of Mastercam I've used... X2, X2MR2 SP1, X3, X3MU1, X4.