post for haas vf-2

[jprobst]

does anybody know where i could find some literature on how to customize my post processor for my haas vf-2?

[Guest]

In MX2 in the documentation there is a

 

post parameter.pdf

 

Welcome to the Forum

 

[Kannon]

whats wrong with your post..being a little more specific, you might find someone can help you here.

 

what do you want to change?

welcome to the forum

[jprobst]

i have mastercam x and a brand new vf-2, the post doesn't put in a g54 code, actually it did it once(very strange), and it has some extra things in there i don't need, also at the end of the program i would like it to return to the middle of the table, i write it in now but its a time waster, and in the beginning of the program it gives me some things i don't need

[Guest]

Well, the lack of the G54 that was but now is not in the post is likely an error occurred when updating the post.

 

I would look in the tool change section of the post, ptl_chg and look for pwcs, make sure it is stilll there and there is no error preventing it from outputting.

 

On the end of the program how do you want your coode to center the table to look?

 

It will go into the peof section of the post.

 

What extra stuff is in that you don't want in?

[jprobst]

It gives me this at the beginning-

/ G91 G28 Z0.

/ G28 X0. Y0.

/ G92 X10. Y10. Z10.

 

don't need it, and the way i want it at the end is this-

G00G49Z.25

G00G91G28Z0.0

G00G90G53X-12.0Y0.0A0.0

M30

%

 

by the way thank you for the welcome to the forum

[crazy^millman]

Check that the post does not use a Mr1 to control this if it does you need to go to the CD and fix it there and all should be good.

 

HTH welcome to the Forum.

[Guest]

in the peof section before the M30

 

plces this

 

code:

---

pbld, n$, , sg00, sg90, "G53", "X-12.0", "Y0.0", "A0.", e$ 

 

pbld, n$, "M30", e$

---

Also on the update if you renamed your file at the bottom of the post there may be 2 cntl defs being referenced.

 

You can delete the one that you do not use.

[jprobst]

this is what it says for the g54

pwcs #G54+ coordinate setting at toolchange

if mi1$ > one,

[

sav_frc_wcs = force_wcs

if sub_level$, force_wcs = zero

if workofs$ <> prv_workofs$ | (force_wcs & toolchng),

[

if workofs$ < 6,

[

g_wcs = workofs$ + 54

]

else,

[

g_wcs = workofs$ + 104

]

if workofs$ >= 0 & workofs$ <= 25, *g_wcs

else, "ERROR - Invalid Work Coordinate System", e$

]

force_wcs = sav_frc_wcs

!workofs$

]

this right?

[Guest]

yes it is,

 

Is your mi1$ variable set to 2?

[jprobst]

no it is set to one, should it be set to 2?

[Guest]

code:

---

 if mi1$ > one,

---

Well, this means if it is greater than one, everything below takes place.

 

So I would say yes

[chris m]

Yes, it should be two. I put this in all of my mill posts:

 

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

# Start of File and Toolchange Setup

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

psof0 #Start of file for tool zero

psof

 

psof #Start of file for non-zero tool number

mi1=2 # Force G5X WOFS output (cdm) <======

 

so that I don't have to sweat this

 

C

[Surface]

To join the consensus, your output is a result of Mi1. There is a check-box in the Miscellaneous Values page (automatically set to post values). You could set the operation defaults to have that checked.

[cadcam]

James What Version are you using?

 

[ 01-18-2007, 11:00 AM: Message edited by: Cadcam From Cad/Cam Consulting ]

[cadcam]

Sorry James you said Mastercam X

[Midwest]

Have you tried the mpmaster post for the Haas.

 

 

HTH

 

 

[jprobst]

i got the bottom of the program to do what i want, but i just can't seem to get the g54 in there, maybe i'm doing it wrong,

[cadcam]

James I called and left my # so I may be able to help you.