Changing Post

[Smitty]

Could Someone Tell me how to change the post

so my tool change is not to the extreme right of the table travel.We are using v8

and MP Fan as our post.

[Dave Eno]

On some controllers (like ours) the tool change position is set in the control.

How do you set tool change position in your programs (if you do)?

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

Dave Eno

Auburn Vacuum Forming Co., Inc.

[email protected]

[Allan Brown]

You are most likely referring to the these lines in your NC files:

G91 G28 Z0

G28 X0 Y0

You could either have post edited to remove the G28 X0 Y0, or you could adjust the G28 'Reference Point' on you control.

[Smitty]

Thanks Dave Thomson for your reply.

I would like to chamge it in the post,any

idea on how to change the post.

[Smitty]

Thanks Dave Eno,We are editing the post now

we do this by changing the G28 x0,y0,to G00.

What I would like to do is change the post so I don't have to do this.The post would do

this for me.I just don't know where in the post to do this.Any Ideas.

[Allan Brown]

Change lines like these:

pfbld, n, *sg28ref, "X0.", "Y0.", e

pbld, n, *sg28ref, "X0.", "Y0.", protretinc, e

to:

pfbld, n, *sg00, "X0.", "Y0.", e

pbld, n, *sg00, "X0.", "Y0.", protretinc, e

or:

pfbld, n, "G00", "X0.", "Y0.", e

pbld, n, "G00", "X0.", "Y0.", protretinc, e

[PBoulanger]

Hi Smitty;

Nice to hear from another Easterner!!!

An option you may be interested in is to use the 2nd reference return point on your Fanuc controller, the G30. Depending on the model of controller there are parameters that can be used to offset the return position of each axis from the hardwired G28 location. If you want your table to go to the left at a toolchange for example, you need to put a value in the x-axis parameter for the 2nd reference return point. Just remember to make it negative, in mm * 1000 and that it doesn't exceed the travel limits of your machine. You can then modify your post file to have it spit out G30's instead of G28's where required.

If your interested I can supply you with the parameters involved. Just drop me a line at [email protected]