[aadrew10]

Hi,

I'm making 4 small parts at a time. They are the same parts. I will use 3 tools. I do not want to do a single part with three tools and then switch to the next part. I want to use tool 1 on each part, then switch to tool 2, use it on each part, and finish the parts with tool 3. This will save quite a bit of tool changes and time. In the past I have done this by copying each individual operation, and changing each individual offset within that operation. This takes quite a bit of time when there are 20 operations with 4 different offsets. 20 x 4 = 80 individual work offset changes. Also, if I need to make a change on an operation, I have to make that change on all 4 of the operations. Is there a better way to do this? I'm using X3.

I want to be able to tell the machine to run all the operations on tool 1, 4 times on G54, 55, 56, 57. Then switch to tool 2, 3 ....

Thanks,

- Andrew

[mactec54]

aadrew10

I don't use MC but there are many ways to do this,One simple way is if you have the 4 parts drawn in MC, Then select the first tool & do all 4 parts at the same, Then the next tool Etc , you only need to use one work offset ( G54 ) for all tool operations

The parts then are just simple X & Y movements apart, no separate offsets needed

[Mike Mattera]

You dont need to draw 4 parts.

Program the first toolpath.
Go to Toolpath - Transformation. Pick the op and select Translate. In the lower right set it to increment the WCS starting at 0 and adding 1 for each Op.

Dont give it any value for the Translation distance.
You just want 4 parts, programmed from 0,0, each with it's own fixture offset.

Mike Mattera

[Superman]

Program the first toolpath.
Go to Toolpath - Transformation. Pick the op and select Translate. In the lower right set it to increment the WCS starting at 0 and adding 1 for each Op.
Dont give it any value for the Translation distance.
You just want 4 parts, programmed from 0,0, each with it's own fixture offset.

You may have to set the tramsform by toolplane ( upper left section )
In the lower left section, execute the op by toolgroup ( upper check box )- this lets mastercam output code to spot all parts, drill all parts, tap all parts in that order
--if you want more ops to occur on one part before moving to the next ( with the same tool ), make it a seperate tramsform.

if necessary, "Ghost" the ops to avoid double machining the 1st part.

[mactec54]

Mike Mattera

That is correct, you don't have to draw 4 parts, this was just an easy way for aadrew10to see a picture of how to do it, as I said there are many ways to do it,why make it compicated if he is trying to figure out how to do it in MC

It's also better to see all the parts on your computer being cut, then you know everything is working when you put the program in your machine

[Superman]

I don't use MC

We won't hold that against you...

That is correct, you don't have to draw 4 parts, this was just an easy way for aadrew10to see a picture of how to do it, as I said there are many ways to do it,why make it compicated if he is trying to figure out how to do it in MC

It's also better to see all the parts on your computer being cut, then you know everything is working when you put the program in your machine

Transform method is the simplest, your method is so open to having errors, it's not funny.
Try modifying a depth , profile, or any other item on all ops and then try to place stock and verify and then backtrack one that you missed

using transform is a direct copy of the 1 operation, modify it, and you've modified all across the board

PS the transform feature does display on-screen

another method, is to copy the view and give the new view another work offset number so when you copy the operation, all you have to change is the T & C planes.... the toolpath will display in the identical loation as the original view

To see it pitched out on-screen, change the origin points and regen
( this is good if you want to have a fixed single origin, common to all parts , but also you are locking in the pitch. )

[mactec54]

Superman

Quote
your method is so open to having errors, it's not funny.


This is ok if you are efficient in using MC, your way will work, as for saying my method is open to error's is total BS

[neurosis]

Mike and Supermans suggestion "is" the easiest way whether you are efficient with mastercam or not. In fact, if you are not efficient with mastercam it is even easier yet than the way you suggested.

As for your suggestion being open to error, I dont know that I agree with that unless you are not paying attention to what you are doing.

Transform will also allow him to make any needed changes to a single tool path instead of having to make a change for every drawn part on the screen. Make the one change and all of the transformed tool paths will follow.

Superman

Quote
your method is so open to having errors, it's not funny.


This is ok if you are efficient in using MC, your way will work, as for saying my method is open to error's is total BS

[mactec54]

Superman
Quote
We won't hold that against you...

I don't use MC for a good reason,There are other software that is much better to use, We own & do have MC ,& my 9 year old uses it when different companys, want him to do there programs in MC

But mostly he programs in the other software that we have, because it is better to use

[mactec54]

aadrew10

This is also how your program could look, this was done with one part drawing, one tool, for 4 parts, & I did not have to tranform anything

[TheBigJW]

Superman
Quote
We won't hold that against you...

I don't use MC for a good reason,There are other software that is much better to use, We own & do have MC ,& my 9 year old uses it when different companys, want him to do there programs in MC

But mostly he programs in the other software that we have, because it is better to use

What is the other software? I know there must be a better and easier than MC. Please do tell.

John

[Mike Mattera]

Transforming the toolpath is one operation. It's not harder than making 3 more copies of the geometry. Not to mention that each will have different coordinated, unless he established 3 more WCS' zero points. All of which is more work. The "Copy" method totally defeats the reason for having associative toolpaths.

So what I'm getting here is...
1) A 9 year old can use Mastercam and make money doing it.
2) Dad should have asked the 9 year old how to help this guy.
3) Someone's not understanding or taking full advantage of associative toolpaths.

Thebigjw: Google Search "Cadcam" or "CAM" systems. You will get a full list of companies that you can contact for demonstrations. Good luck in your search for a new CAM system. If your not happy with Mastercam I strongly encourage you to buy a new package that will suit your needs better. Because if you think that Mastercam service, software and maintenance sucks, just wait till you've tried the competition.

[neurosis]

aadrew10

This is also how your program could look, this was done with one part drawing, one tool, for 4 parts, & I did not have to tranform anything

You can get similar code in mastercam using only one set of geometry and transform. You can also get each position to post using only one fixture offset or separate for each part location using transform. You have the option of using sub programs or not using transform.

Again. Transform is very fast and easy to use. You do not have to be efficient with mastercam to use it. I dont know that a 9 year old could do it though..

[aadrew10]

Thanks for all the input guys. I figured out Mike's method on my own yesterday and it makes what i'm trying to do quite easy. Mastercam has so many features and options and it's pretty easy to figure them out on your own. Super program.

If I had logged back into here I would have seen the answers given and would have saved a bit of time.

Thanks again guys,

- Andrew

[mactec54]

Mike Mattera

If you read my post,You would see that we do have MC & on maintenance, & I don't have a problem to do the transform operation,without the help of my 9 year old, We also have Gibbs cam my favorite & is what I use all the time now,it also has the Best customer service

I only keep the MC going because, Julien my son, uses it for paying customers, He also uses Gibbs,Solidworks & Aspire, we have other software that he would like to use, but I think he has enough that he is doing, learning 5axes now

[mactec54]

aadrew10

Glad you figured it out,& how to do it in your MC, it sometimes is the best way to learn, different things, as you will then remember them for next time

[colton_m]

Wow, this just made my life a whole lot easier!

One question to add though.

Using mikes method, how could I limit the number of work offsets it posts?

Right now I am working with a facing operation and would like it to occur on two parts. I got the transformation to work (with no translation distance, as discussed). However my code is comming out like this:

(Facing)
G54...
(Facing)
G55...
(Facing)
G56...
(Facing)
G57...

Under work offset numbering my start is 0 and my increment is 1.

Only problem is I only need G54 and G55 (Two parts). How can I hold MC back from posting G56 and G57?

And on a side note what about G58 and G59? What if I wanted 6 parts instead of two... or four?

Thanks,
Colton.

[aadrew10]

Go to your transform parameters, click the translate tab, set your # of Y movements to 0, set your # of X movements to the desired number of work offsets. The default is 2 and 2, which makes 4 parts, that's why you're getting 4.

[colton_m]

Hehe it works just kick-ass now.
The answer is always right in front of you isn't it

Thanks again.