How To Set Up Work Offset

[EPettus]

Fairly new user of V8 MasterCam Mill, I can not find info in my supplied books how to set up 2 or more work offset in one program. I know I want it to output G54, G55, etc., but where or what is the area I need to go to change from one to other work offset in the software. Any help would be appreciated.

[Fred from Université de Sherbrooke]

In the tool parameters page of your operation, there's T/C plane button. Click on it and you'll see Work offset. If you put 0, you'll have G54. If you put 1, you'll have G55 (G54+1).

[B Whale]

I'm a mastercam new user,i try to follow Fred to do that ,but i still can't get G55 when i changed it to 1 in the work offset of tool parameters page

......tell me more Fred........

[EPettus]

I did this also and I am getting the correct geometry, but I also am getting G54 output from the post. I have reviewed the post and do not find anything that just jumps out at me. FRED or anyone if you let us know more. Thank for the help.

 

[ 10-24-2002, 03:23 PM: Message edited by: EPettus ]

[Finecut]

Come on guys, WHAT Post are you using ????

THen we can all look at it as see where the problem is !!!!!!!!!!!!

 

Finecut

[P_Scott]

EPettus,

 

Check to see that the Misc. Int. value is correct for a G54 offset series output. You can find this value in the "Misc. Values" button in any toolpath's parameter page of the operation. This, combined with the correct value as FRED suggested will produce what you are looking for. All this information is listed at the top of a Mastercam post processor, usually just after the header of the post where it will have additional notes to describe how you would set up for multiple work offsets. Read the post you are using before just plugging in numbers in value fields and hoping you'll get the output you need. HTH

[B Whale]

I have tried to change the setting in the tool parameters page with the post of MPFAN.pst .........work coordinates[0-1=G92, 2=G54's] to 2 in Misc values, and change Work offset to 1-5 (to get G55 -G59) in T/C plane.thanks Fred and Peter Scott , i have got it .

but i have another problem in the post that i always use, that is : MPOSP.pst ,as i can't get the result follow above setting.

Please tell me how to change the post. below is the top part of MPOSP.pst example:

 

************************************************* # Post Name : MPOSP

# Product : MILL

# Machine Name : OKUMA MILL

# Control Name : OKUMA OSP5020M

# Description : OKUMA MILL

# Associated Post : NONE

# Mill/Turn : NO

# 4-axis/Axis subs. : YES

# 5-axis : NO

# Subprograms : YES

# Executable : MP 9.0

#

# WARNING: THIS POST IS GENERIC AND IS INTENDED FOR MODIFICATION TO

# THE MACHINE TOOL REQUIREMENTS AND PERSONAL PREFERENCE.

#

# ------------------------------------------------

 

# Revision log:

 

#-------------------------------------------------

 

# Programmers Note:

# CNC 05/03/01 - Initial post update (re-write) for V8.1, rjm

# CNC 01/09/02 - Initial post update for V9.0, rjm

#

# ------------------------------------------------

# Features:

# ------------------------------------------------

# This post supports Generic OKUMA OSP-5020M code output for 3 axis milling.

# It is designed to support the features of Mastercam Mill V8.

#

# Following Misc. Integers are used:

#

# mi1 - Work coordinate system

# 0 = G30 reference return is generated and G92 with the

# X, Y and Z home positions at file head.

# 1 = G30 reference return is generated and G92 with the

# X, Y and Z home positions at each tool.

# 2 = Fixture Offsets of H1, H2...H50 based on Mastercam settings.

#

# mi2 - Absolute or Incremental positioning at top level (Main Program)

# 0 = absolute

# 1 = incremental

#

# mi3 - Select for G30 reference point return at each toolchange.

# 1 = G30 output requested.

#

**************************************************

 

I prefer to use MPOSP post as it without the sequence number and with R in G2 ,G3 when i save my nc file. MPFAN post with sequence number and IJ in G2,G3.

 

 

tell me what post should i use if i need it with: G54 to G59, R in G2 G3, no seq number , feed in F#.

 

thank you.

[heeler]

If you contact your reseller, they can change the MPfan post to do that really easy. I know that our mpfan post has been modified to put out the R and use only 180 deg or less arcs. Your reseller can many times suggest other real improvements to your post.

 

HTH

[cadcam]

I wonder if he has lookied at the MPmaster post from this site.

I do not know the Machine he is running.

[B Whale]

great! mpmaster.pst is the one that i looking for .

thanks Jay.

[EPettus]

I am using MPCENT6.pst which is a modified version of MPFAN.pst as I am told.

 

Work offset problem, I believe I have got it now. Sometimes I require a swift kick to the head to see what I need to do.

 

Many Thanks to Fred, Peter Scott, and All Forum Users.