Work offset in Wire EDM

[VC]

Hi, I like to wire cut multiple blocks on Wire EDM. How do I get G54, G55, G56? Do I have to modify the post? or Do I have to deal with Mastercam setting? I have been tried Misc. Value by putting 2,3,4. It only generated G54 so far. Please help me on this. Thank you very much.

[crazy^millman]

If it is like Mill you go to your T-plane button click and you see work offsets on the page there. I dont 54,55,56 I use 1,2,3 so I dont know if you put 1,2,3 or 54,55,66 I think it is 1,2,3 to make the post output 54,55,56 so just play and post a program and see what you get.

 

I hope that helps.

 

Crazy Millman

 

[ 09-28-2003, 07:41 PM: Message edited by: Millman^Crazy ]

[VC]

Hello, Millman, Thanks for your reply. Unfortunately, Mastercam wire doesn't have t/plane. I could not find anywhere in mastercam wire parameter showing the work offset. Right now, I just edit the program manually by putting G54, G55,G56 in the program. Any more help? Thanks.

[crazy^millman]

Sorry Vg I dont have wire cant be of any more help on that one.

 

Crazy Millman

[Lars Christensen]

Hi VC,

 

I forgot to check today if you can changes work offsets in wire.

 

But when I am runing multi parts in my wire then I am useing subs, many times I have different costumers in the machine at the same time.

 

I have made a main program that looks something like this:

G00 G54 x0. y0. z0.

G22 L1000 (calling sub-program)

G00 G55 x0. y0. z0.

G22 L1100

G00 G56 x0. y0. z0.

and so on.

This is just saved under a folder were I always can get it.

 

That way I am still writting my programs as normal, so if I get one job repeat, then I just run that program(forexamble program 1100).

 

Lars

sorry about the spelling

[Steve Landkamer]

VC,

It is Mastercam settings. I had the MPWFANUC post as my default and I set Misc. Integer #1 to 2 to invoke the Auto G54, G55 setting.

Then I had to go into the Origins/WCS button and set my new Start Position and Work Origin. Then I did get G55, G56 etc.

I hope this helps.

Steve

[CAM-mando]

Steves post above is for V9.1. If you are running V9.0 or lower the WCS options are not available and the stock MPFANUC.pst does not respect the mi1 value without modification.

 

Also in 9.1 if using the transform wirepath it will increment the G54,G55,G56 etc. if mi1 is set to 2.

 

Several improvements have been made in 9.1 regarding multi origins and start/cut/thread points.

 

CAM

 

[ 09-30-2003, 12:25 PM: Message edited by: CAMmando ]

[Steve Landkamer]

Ooops there is a different procedure in V8.1.1.

 

You still have to set mi1 to 2 then go into STCW and select a new XY location for the work origin.

Then the "Auto" G54, G55 etc. will work on the MPWFANUC post in V8.1.1.

 

I think that V9.0 should be the same as 8.1.1, I don't have 9.0 installed to be able to check that.

 

Steve

[Metric]

VC

I've been running wire with multi blocks setup.To get G54,G55 etc..On misc. Value you have to put 5,6,7..(Not 2,3,4..).Then you will get G54,G55..

 

[ 09-30-2003, 09:01 PM: Message edited by: Metric ]

[VC]

Hi all

 

Thank you all. Finally, I got G54, G55, G56 by using Steve's method. Steve, I just wonder why the work origin of multiple blocks must not be the same as the WCS(F9) value? So in order to get work offset, i have to put some value other than zero in work origin. Once again, thank you for your helps.

[Steve Landkamer]

VC,

Unfortunately I think it is the nature of the beast in Wire EDM. I belive the thinking was if someone was wanting to use a different workoffset number that offset location would have to be at a different XYZ location. It is assuming that if the offset XYZ location is the same you wouldn't want to use a different offset. I think that is why it says "Auto G54, G55" in Misc. Integer #1.

 

If what you are looking for is using G54, G55 etc. from the same XYZ location, you should be able to make it do it in the post.

 

Steve

[P_Scott]

VC,

 

Work offsets are post specific. That's why Steve's values and Metric's values are different than yours. To find out how the Work offsets are output for your machine, read the post processor you're using. It is typically near the top under Features. It may be easier to do a "Find" and look for G55 or Work Offsets in the post.

 

The WCS is designed to take any selected view and make it the TOP view for toolpaths/wirepaths in Mcam V9. It doesn't necessarily mean you need the Work Offset to match the WCS. They can be different. You can have multiple WO's on the same WCS. There is a document that was produced by Mastercam to explain the WCS in more detail, it's just not easy to read. I suggest getting some instruction from your reseller. They should offer a class which goes into greater detail with WO's and/or the WCS. HTH

 

[ 10-01-2003, 11:06 AM: Message edited by: Peter Scott ]