Tool change position

[RichE]

Could someone tell me how to set my tool change position in mastercam. I know that I found the path to set the tool change location once but I'll be darned if I can find it again. I'm running V8 on a Bridgeport cnc mill and it would be nice to have it complete tool changes at -2,0,0 .

 

Thanks

[JAMMAN]

Welcome to the forum, RichE.

Wow, I'm up to learn something from this thread. Till 1 minute ago I would have bet money that tool change position was handled by the controller, because every one I've ever worked with was.

[gcode]

Rich

On the Tool parameters page of every operation is a box labeled Home Postion.

When I enabled the Home Position Box and used post MPBOSS10 (from the installation disc)

Mastercam output moves to home.

In the NC Settings of the Screen/Config pages

you can set a defualt home postion.

I think that if you check the Home box in the first operation of a program Mastercam will output Home moves for every tool change.

If this isn't working for you, you are probably using a post that doesn't support the Home Position feature.

[ 12-23-2001: Message edited by: gcode ]

[Guest CNC Apps Guy 1]

Well, there are a couple of different ways you can deal with it.

[*]1) "Hard Coded" In the Post

[*]With the Home Position Switch

Option 1 will require you to into the post and in psof and ptlchg, the line before the tool change command you'll need to put someting like pbld, n, "X-2." ,"Y0.", "Z0.", e

Option 2 will require you to set the Home Position in Screen Configure, NC Settings and Home Position. Then click the Home Postion switch in your toolpaths, or go to Screen COnfigure, NC Settings, Operation Defaults and set all the toolpaths to turn on the Home Position switch. You'll also need to go into the post and at psof and ptlchg and add the line pbld, n, *xh, *yh, *zh, e

Hope that helps.

[RichE]

Thanks, everyone! I just needed a little mind jog. I went to screen-configure-nc settings and set the home position for -2.0,0,0. I then checked it under setup sheet-test fields and it looks like the tool change position is now set properly. Again thanks

[Reece L Gibson]

I think there is a "M25" you can put in the program and it acts like a G30 on a Fanuc.

(You set this position in advance and store it in the control)