X3 post problem for rookies on horizontal

[left coast lefty]

Using the generic 4axis Fanuc HMC post, G54 is forced to G55, G56, and so on in transform rotate toolpaths. We have looked all over but cannot find anything. Does anyone know how to set the machine or control definitions to deal with this? The toolpath looks good. We just want it to stay on G54.

[Dan@home]

Try Settings/Machine Def manager then click on the little telivision icon (Edit the control def)/Work System, in the drop down for (Tplane during automatic work offset number creation:) select None. I am working with X4 so yours might be a little different.

 

PS, you can stop the alarm you get when are using the same offset # for more than one view. Play with some of the settings on this page.

[Justin Beebe at Folsom Tool]

left coast,

 

I'm not using X3 but I beleive this info will apply to X3. There are a few ways to control this. If you set mi9 to 1 your toolpaths will lock onto the first WCS so you will always get G54. If you want to change your post so you do not have to use mi9 do the following. Keep in mind the post shown below is an old V9 mpmaster post but the same method worked for X2. Your post may look a little different.

 

To universally lock on to G54, in psof change:

 

code:

--------------------------------------------------------------------------------

 

sav_mi9 = mi9 sav_workofs = workofs

 

--------------------------------------------------------------------------------

 

to:

 

 

code:

--------------------------------------------------------------------------------

 

sav_mi9 = 1 sav_workofs = 0

 

--------------------------------------------------------------------------------

 

Once you make this change you will only be able to post G54.

 

 

I also reccomend doing the following so you get a B output if your first toolpath is B0.

 

For the forced B, search for these lines in pheader:

 

 

code:

--------------------------------------------------------------------------------

 

sav_rot_on_x = rot_on_x rot_on_x = 0

 

--------------------------------------------------------------------------------

 

change to:

 

 

code:

--------------------------------------------------------------------------------

 

sav_rot_on_x = rot_on_x rot_on_x = 1

 

Hope this helps and that this info is not outdated. As always back up your post before making changes

[MIL-TFP-41]

In your WCS view manager there is a column for work offset. Make sure it is set to "0" on all of the planes you are using. The 0 will output G54. My guess is right now it is either blank or set to -1. Once you do this you will likely get an warning message "Same work offset used on multiple views" when you post. To get rid of that....

 

http://www.emastercam.com/cgi-bin/ultimate...ic;f=2;t=000048

[Dan@home]

JMC forgot that part about the 0,s

[Trevor Bailey]

or get the mpmaster_horizontal set up. that way you can LOCK ON First WCS using the mics value.

[left coast lefty]

Many thanks to all. I will try these tomorrow morning at the shop. I have the demo version here at home, but it's not quite the same.

[Jayson Kramer]

Well now I get the answer lefty. I had posted to find what version you were using on the other forum to answer your question.

 

Here is a picture of my WCS View Manager for a project I did in X3 on a EC500 Haas. using a Chick tomb system. 8 parts loaded and one offset from center of rotation.

 

[Guest CNC Apps Guy 1]

On the WCS;

0=G54

1=G55

~

5=G59

6=G54.1P1

and so on and so forth.

 

Putting 55 like Jay said puts you at G54.1P150.

[left coast lefty]

Thanks guys. I'll check it out tomorrow. I never got an alarm, just unwanted Gcode.

[Jayson Kramer]

James on the MPmaster configured for the Haas I get 154 P50 not the 54.1 P150 just so you know.

 

quick posting sample:

 

(PROGRAM - TEST.NC)

(HAAS 3/4-AXIS HORIZONTAL)

(MACHINE GROUP-1)

(MASTERCAM - X4)

(MCX FILE - T)

(MATERIAL - ALUMINUM INCH - 2024)

(DATE - JUN-22-2009)

(TIME - 5:02 AM)

(T1 - 1/2 FLAT ENDMILL - H1 - D1 - D0.5000")

G00 G17 G20 G40 G80 G90

G91 G28 Z0.

N1 T1 M06 ( 1/2 FLAT ENDMILL)

G00 G17 G90 G154 P50 X-.1 Y-.5578 S1069 M03

G43 H1 Z5.

Z4.1

G94 G01 Z3.5 F6.42

[Guest CNC Apps Guy 1]

Haas... my bad.

 

It's still the same issue regardless of how Haas Extended Work Offsets work though. He incorrectly addressed the Work Offsets in the WCS. Intead of 0, he put 54. instead of 1 he put 55, so on and so forth. Unless there's some math in his post to comp for it, you can't do that.

 

Just to clarify YOU brought up Haas, not us Jay. He said FANUC

[Jayson Kramer]

James good point it looks like I put G55 in there being the offset. but it was what was needed by the post to put offset 154 P50 to force out.

 

And I have been Clarified Sir.

[Guest CNC Apps Guy 1]

Nuthin' but love for ya Jay, nuthin but love...

 

Just bustin' yer ballz a bit.

[left coast lefty]

Thanks again guys! It worked putting "0" in the Woff#'s in the View Manager. Also, under Transform Operation Parameters, Types and Methods, Work Offset Numbering, selecting "assign new" and then zeros will affect the outcome. Still working on the various combinations. Sometimes we actually want to force G55, G56 etc. for some applications.

[Jayson Kramer]

Lefty what city in Cali are you in?

[left coast lefty]

San Leandro.