G-Post

[ptc-766123]

Hello Everyone,

I am trying to out put a tool change sequence for a Yasnac MX-3
controller. Basically I need to output the line " G28 G49 Z0.0 M05 "
before I grab the next tool. I have looked at tool change seq. under
machine codes but I see no option to insert this line. Do I need to write
a FIL routine to accomplish this?

Thanks in advance,




Kevin Uttley
CAM Programmer
Centerline (Windsor) Ltd.
Automation Components Division
655 Morton Dr.
Windsor, Ontario
N9J 3T9
(519) 734-8330 x 259

[AustinN.C.,Inc.]

> Hello Everyone,
>
> I am trying to out put a tool change sequence for a Yasnac MX-3
> controller. Basically I need to output the line " G28 G49 Z0.0 M05 "
> before I grab the next tool. I have looked at tool change seq. under
> machine codes but I see no option to insert this line. Do I need to write
> a FIL routine to accomplish this?
>
> Thanks in advance,
>
> Kevin Uttley

The correct answer is YES!

Try this FIL example:

CIMFIL/ON,LOADTL
XX=POSTF(20) $$ SAVE THE LOADTL RECORD
INSERT/'G28 G49 Z0.0 M05$' $$ OUTPUT YOUR STUFF
XX=POSTF(21) $$ RELOAD THE LOADTL RECORD
XX=POSTF(13) $$ EXECUTE THE LOADTL RECORD
CIMFIL/OFF

You need to make sure your settings under Machine Codes -> Tool Change ->
Tool Change Coordinates that the Z coordiante for tool change is a
positive number like "30". Maybe a bigger number if you have a large
amount of Z travel. Also make sure you have the post set to "Do Not
Output" a positioning block.

Fred

[byron.taylor]

Can a G-post used in GOELAN or MasterCam be converted to Pro-Man?