Multiple work offsets

[normand]

Hi all,

 

I've had a search through the forum and can't quite find what I'm after. It's probably there but maybe I need a little guidance still. I currently have a HAAS VF-1 and are just about to upgrade to a VF-3 so we can machine multi parts,,, And that's where my question starts. We machine mostly the same 2 op parts. About 20 different parts. 1 vise for op 1 the other a machined softjaw for op 2. You get the picture.

For the VF-3 I have 4 new chick vises (double) and each vise will do 1 complete part. What I'd like to do is have the flexibility to machine part A on vise 1 and 2 and Part B on Vise 3 and 4 (for example). Is there a simple solution to this??

 

I'm thinking that I could import all toolpath operations to 1 file? Or is there a better way to work with work offsets.

 

Thanks,,

[ATG]

Just import the operations for both part a and part b in one program. Then you can use transform tool path to off set for vise 1,2,3,4

 

Offset G54,G55,G56,G57

[robh]

We do mostly the same kind of 2 op work.Our op1 is done on the rear jaw of all the vises and op 2 is done on the front just flipping the part forward into the pocket machined in the soft jaw.Not enough offsets G54-G59 unless you have G54.1P01-P48 or more,newer machines do have multiple offsets like this.If you don't,once you define where your vises are you could do it with only two ie. all op1 G54 and all op2 G55 but that makes it hard to do any fine tuning to any one set of jaws. Don't know if that's what you're looking for or not.HTH

Regards

robh

[Josh T™]

Wouldn't using WCS take care of this? I just got finished with a 3 operation/setup program using multiple WCS and it ran great.

 

HTH

Josh

[Justin Beebe at Folsom Tool]

They way I do this is to first make a layout with solids that shows my parts in the vises. Then from the view manager I do the following

 

1. Copy the top view and name it G54

2. Assign work offset 0 to the new view G54. 3. Select an origin for the new view G54

 

1. Recopy the top view and name it G55

2. Assign work offset 1 to the new view G55. 3. Select an origin for the new view G55

 

Then I program each part being careful to select the proper view before creating each operation. Mastercam will automatically output the correct fixture offset codes.

 

There is a great example of this method in the older WCS tutorial.

[Justin Beebe at Folsom Tool]

This is a repost because my last post looked confusing.

 

They way I do this is to first make a layout

with solids that shows my parts in the vises. Then from the view manager I do the following

 

1. Copy the top view and name it G54

2. Assign work offset 0 to the new view G54 3. Select an origin for the new view G54

 

1. Recopy the top view and name it G55

2. Assign work offset 1 to the new view G55 3. Select an origin for the new view G55

 

Then I program each part being careful to select the proper view before creating each operation. Mastercam will automatically output the correct fixture offset codes.

 

There is a great example of this method in the older WCS tutorial.

[Justin Beebe at Folsom Tool]

It did it again

[MotorCityMinion]

G10 and subs would work good also.

[normand]

Thanks heaps for all your replies,

I'm trying hard to educate myself right now, I have been programing parts for a couple of years and never used multi offsets, wcs, transform or toolpath import. I guess I just go stuck on what was working.

I have a bunch of parts programmed already and what I'd really like to do is import each part onto a different work offset post the code and have toolpaths run 54 55 56 57 before changing to the next tool (I hope that made sense).

I think my solution is somewhere in your answers and the MC help.