Tech Tip, Multiple Parts using Transformed OPS.

[Dave.L]

Greetings Members,

 

Based on another post and member requests, I have created 3 sample files to demonstrate multiple part tool paths using transform operations. I have uploaded these files to the FTP (X4 files sub-directory) and they are as follows:

 

Transform OPS-sample-1.MCX

 

In this example, 4 parts are on the table and the program will process 1 part complete and then move to the next (process complete) and so on. This is not an efficient method but sometimes users may want to do this for many reasons (low quantity run and easy maintenance)

 

Transform OPS-sample-2.MCX

 

In this example, the same 4 parts are on the table and the program will be processed by tool order, still jumping from part to part based on the tool. Better, but still not the most efficient.

 

Transform OPS-sample-3.MCX

 

In this example, the same 4 parts are on the table and the program will be processed by tool order and operation order. Each tool will process all ops it’s used on for each part before moving to the next part. This is the most efficient tool path for cycle time.

 

Please realize a few things: 1) It’s late. 2) These are sample dummy files for the purpose of this topic only. 3) All examples have incrementing work offsets for each part location. Example, Part 1 G54, Part 2 G55, etc. If you have questions, please post them and I will answer.

 

I hope this helps.

 

BTW, I am well aware many members already know how to do this. This thread is for those who do not. Please feel free to add to this thread to help.

[Fred @ Slate Industries]

Dave

What about the Tool Z offset's ?

Thats my hang up, touching all tools off the G54 work piece and then only touching the "Gauge tool" off every work piece and plugging that # in?

 

Spoiled by probes and lasers and Hurco touch screens "Z offset / all tools"

 

Thanks Dave!

[Dave.L]

quote:

---

Thats my hang up, touching all tools off the G54 work piece and then only touching the "Gauge tool" off every work piece and plugging that # in?

---

Tony,

 

That is your issue -old school approach. I long term buddy of mine has an old Fadel and he does not understand tool lengths.

 

The tool should be touched off in a way the control stores tool length independent of the workoffset. Then, the workoffset can be set using any tool in the mag or automatically without the tool (for known workoffsets).

 

I hope that helps you.

 

EDIT: BTW, these examples are setup to post out different workoffsets per part location.

[Dave.L]

One more note: If you are jumping from different workoffsets at different Z values, you need to be carefull and add clearance or retract (reference) postions.

 

Tony, maybe this is what you were asking?

[jhjr]

I'm not sure if this adds anything but I'll say it anyway. Say you want to create 40 of the same parts out of 1 piece of stock using 1 work offset. You can use transforming to machine all parts after the first part with a similar method. Do your 1 first path then transform it. You can even kinda of nest your parts this way if you don't have that option using transform mirror, rotate etc. You can subprogram using inc so your code isn't a mile long. This can be very handy. Thought I'd add a little more about transforming for those who don't know much about it.

[Thee Rickster ™]

I have only used transform a few times and here is what I had done.

 

No sub programs just 1 transformed group of paths.

 

Back in Jan i turned a 6 insert fixture into a

36 mold insert program to maximize efficiency in

changing inserts. Now the entire (36per)cor/cav sets

are Machined over night. They are doweled to the

fixture plate and the z level pick up are the same

and the locations are equally spaced grid pattern.

 

I used your #3 method without using the g54,g55...

locations. transformed the path 5 across (in x)

and 5 down (in y).

 

It turned my file size from 50 meg to 430meg.

It takes about 10min to open the file now.

and take a little patience to do a simple E.C.

but the path is Awesome.

 

Thanks for the tips.

 

Cheers

Rick

[Dave.L]

I created the samples for a few reasons:

 

1) I have received an incredible amount of help from this forum and I wanted to return the favor. I have no formal MC training and much of what I have learned came thru this forum.

 

2) I get the impression that even some of the seasoned MC users have not used this toolpath much or even at all.

 

3) Transform tool paths can be applied so many ways. We would probably need about 20 examples to fully illustrate all the possible scenarios. I mostly use this for multiple parts. But as you all can see from the replies, there are many other uses.

[MACHINEMASTERG]

i relize this is about using transform to get multiple parts but we use the MPSUBREP pst.

We programe and machine the 1st pc make any adjustments to the master cam file then repost with this pst and you get multi pcs in a subrep easy to edit not alot of code and you get efficent code ...i think not alot of users know of this post but it works great ...hth

[Dave.L]

Greg,

 

But how do you order your operations?

 

With transformed OPS you have many options to choose.

[John @ Walter Klassen FX]

We do a fair amount of mirrored parts, transform mirror saves me a lot of time.

[MACHINEMASTERG]

Dave with the mpsubrep pst it DOES each operation for each of the multi parts then moves on to the next op it does NOT do 1 complete part and then another .

[Dave.L]

Greg, take a look at my example 3 on the FTP (backplot it). You will see how this is a benifit for cycle time.

[JasonM]

I'm trying to get either method #2 or #3 to work, but for some reason I am not getting a new work offset # when it attempts to machine the other piece? I have a feeling I am missing something? I have copied the Transfrom Toolpath Parameters menus identically.

 

Thanks

[Dave.L]

Jason,

 

Email me your file and I can look at it tommorrow.

[JasonM]

Thanks Dave, I sent you an email.

 

I just tried posting one of your samples, and I do not get G55, G56 etc.. on them either?

[Dave.L]

Jason,

 

It's a post issue. I just posted your file with my post and it works fine.

[JasonM]

That's what I thought.

 

Thanks for your help, I will contact my vendor.

 

Your examples were still quite helpful!