[GTOGuy]

Using MC X, when I post to a generic 4 axis post I use for my PCNC 1100, I get the G54 code output near the beginning and a G28 at the end of the NC file that I don't want. Here are the examples of the strings in the file.

"G00 G90 G54 X.77 Y-.588 S1200 M03"
"G28 Y0."

Anyone know how to configure MC so it does not do this

[ataxy]

why dont you want a g54

[cob]

try this
on mastercam say you are doing a toolpath operation like (drill toolpath)
you sellected your holes, then on your (toolpath parameters page) at the bottom there is a box called (Misc values) you select that box and on the top
box where it says (work coordinates) make sure there is a number 0 (zero)
try that see how that works

[GTOGuy]

Tried the misc values box setting. It was already on 0

[GTOGuy]

ataxy,

I am setting the parts up to the work coord system (i.e. corner of the vise, center of my rotary head, etc) and don't want the program to override that WCS when it runs as it will if the G54 is in the code

[jeffrey001]

I think it must be set to -1, 0 is for G54, 1 = G55 2 = G56 and 3 = G57

[GTOGuy]

The -1 didn't do it either unfortunately.

[psychomill]

Any value 0 or less will output a G54 for most posts. You need to edit the post in order to not output any WCS values.

I am setting the parts up to the work coord system (i.e. corner of the vise, center of my rotary head, etc) and don't want the program to override that WCS when it runs as it will if the G54 is in the code

What work coord system are you talking about? Are you saying you're not using any work offset at the machine? Are you positioning based on machine coordinates (G53 for many)....?

[Superman]

Do a back-up copy of your post

open the post using a text editor and find

force_wcs : yes$ #Force WCS output at every toolchange?
change to
force_wcs : no$ #Force WCS output at every toolchange?

Test on multiple operations that it works correctly

Also
Misc Values MI#9 may also "lock onto 1st WCS" your post may/may not use this

[oldjohn]

I did it like this:
#force_wcs : no$ #Force WCS output at every toolchange?

[Andre' B]

On every control I have seen G54 was the default work offset meaning that even if you do not put a G54 in your program you are still using the G54 offset unless you have a G55 ... etc..

[psychomill]

That's a parameter setting for most machines. Most factories will set as a system default to G54 however it can be changed to default to nothing or G53. There are actually several variations to the parameters and some controls even have this default control for AUTO operation status.

But, for most cases I've seen, you still have to call G54 in order to use G54 even if the machine defaults to G54. Therefore, you can move around and machine all over the place without ever using G54. A bit crazy IMO but I've seen it done....

[GTOGuy]

I ended up having to comment it out as suggested like this:
"#force_wcs : no$"

Same to supress the G28 I set the sg28 value to "" rather than the "G28"

Thanks everyone for the replys

For those asking why I needed to do this, I generally make 1 or 2 parts rather than a long production run and I generally set the part up in a specific coordinate system when setting up the machine (i.e. G55 - corner of vise or G56 - center of rotary head) and I don't want the program to override my plans by telling the machine to use a G54 when I have set it up in a G55. I learned this the hard way when it crashed my tool the 1st time.

Pat

[psychomill]

So if I'm following you right.... You actually already have "preset" coordinates in your machine then? So G55 is always the corner of vise or G56 is always center of rotary head , etc, etc? If so, then I see what you're doing...

[GTOGuy]

That is correct.