Changing G54 to G55 in MC

[deanj]

How do i change my G54-G59 settings in mastercam V8? thanks,JMD

[Scott Bond]

Hi

on the first page of operations, click on mis.values. Read the top let box put a 3 in it,and try it.

[TheePres]

Scott,

How could I do this in mass to 200+ operations?

[Steve Biehl - Cimquest Inc]

select the ops to change, right click and select Options-Edit common parameters.

[Jim Evans from CNC Software]

JMD,

 

What Scott suggested will only work if your post uses the MISC Values for work offsets. If your post uses the work offsets inside Mastercam, then you need to edit the work offset field under the T/C Planes dialog box.

 

Edit your post and search for the variable WORKOFS, if you find it, then the post is probably using the Mastercam Work Offset Field and Scott's solution will not work. If your post is using the Misc Values for the work offset value, then do exaclt what Scott and Steve have suggested.

[david b]

i found thst if u dont put any G54-G59 the machine will default to G54 and if u want G55-G59

in a program that u only have to do it the first tool path only the G55-G59 will stay modal until program end or you call a new G54-G59.

[rottncf]

Toolpaths--Operations--T/C plane checked

Tool Plane/ Construction Plane--Tool plane checked

Work offset checked

-1 = tplane is off--defaults to G54

0 = tplane is on G54 + 0 = G54

1 = " " " " + 1 = G55

2 = " " " " + 2 = G56

3 = " " " " + 3 = G57

4 = " " " " + 4 = G58

5 = " " " " + 5 = G59

6 = " " " " + 6 = G54P1

7 = " " " " + 7 = G54P2

...= " " " " + . = G54P...

 

I have my post customized to output the "P" offsets, so your post may not output the same.

 

The only thing I can't figure out is how to force the tool to a new clearance plane between offsets (I want my tools to rapid up +2.00 before moving over to the next wfo).

 

Hope this helps.

 

Les.

[vulan]

quote:

---

Toolpaths--Operations--T/C plane checked

Tool Plane/ Construction Plane--Tool plane checked

Work offset checked

-1 = tplane is off--defaults to G54

---

mine :

-1 = tplane is off--defaults to G53 ???

mc9 sp1 ,win 2000

[Jim Evans from CNC Software]

A value of -1 in the work offset field should be written to the NCI file (1016 line parameter # 9) as a zero. -1 should never be written to the NCI file.

 

If this file wasn't created in V9sp1, try doing a regen to see if this problem goes away.

 

As far as -1, this does not mean OFF to Mastercam. A value of -1 tells Mastercam to automatically set the value as need. So if there is a change in tool plane or tool origin, then a new WCS value will be generated. If you don't want Mastercam to do this, then always set the work offset to 0 (G54).

 

I hope this helps!

[deanj]

Thanks for all the help guys. I know this reply is kind of late, I was actually was on vacation for the last 10 days, but it was great to come back and find all this useful info. I finally got the damn thing working.

 

Thanks again, JMD