Tool change position

[Threept82]

Hi guys. (Mill-9.1)

Is there a trick to having the machine go to

the ref. or home position for tool changes without

having to hard wire it in the post.

I only need to do this when set up is to high,

not often. Thanks.

[Threept82]

?

[Fralex_francois]

I already done that at school on fadal but it was on the machine not in the post it's supose to be a setting for zero return to change... check on this maybe

[Threept82]

I have no idea what you just said.

[Jack Mitchell]

G91 G30 XYZ

 

This will take you to a secondary machine zero position. Sometimes these values are pre-set-able in parameters.

 

Just another thought on this topic.

 

Regards, Jack

[Fralex_francois]

Instead of sending your machine to your regular home machine, you send it to a substitute home machine that you can set in your machine but I don't know what parameter you have to change.

 

p.s. what is your machine???

[Threept82]

I can do it long hand but I thought there was a

switch in Mastercam

(turn on to go to home at tool changes)

(turn off not to.) if I check the box in Home

position isnt mastercam suppost to code that on.

no matter which post i use, it still does not

go there. I hope i'm making sense, because noe i'm

[Guest CNC Apps Guy 1]

You could use an open Misc. Int. Create a postblock like below

 

pmoveout

pbld, n, "G0", "G91", "G28", "Z0.", e

pbld, n, "G0", "G90", "G28", "X0.", "Y0.", e

!mi5

 

Then at the Toolchange

 

pcan

if mi5=1, pmoveout

if stagetool >= zero, pbld, n, *t, "M6", e

pindex

 

HTH

[jeff]

Or just create a macro on your machine, so every time it reads an M06 it goes to a certain position.

[fboike]

Just click ref point in tool parameters page

tell it where you want it to go for tool change.

I use it for tall setups too.

[Threept82]

Thats what i needed. Thanks

[kinglouie V]

After an exhaustive search I've found this old posting of yours to affect a tool change position. I'm having trouble finding the appropriate place for this text as pcan in my post is referencing 'canned text'. Would you have any suggestions for

this? I have already designated a place for the misc. integer so where can I put this language to be effective?

 

 

pmoveout

pbld, n, "G0", "G91", "G28", "Z0.", e

pbld, n, "G0", "G90", "G28", "X0.", "Y0.", e

!mi5

 

 

pcan

if mi5=1, pmoveout

if stagetool >= zero, pbld, n, *t, "M6", e

pindex

[Tim Johnson]

You can put the postblock almost anywhere. How about after Toolchange setup;

code:

---

#Toolchange setup

 

pmoveout

pbld, n, "G0", "G91", "G28", "Z0.", e

pbld, n, "G0", "G90", "G28", "X0.", "Y0.", e

!mi5

 

pspindchng #Spindle speed change

if prv_spdir2 <> spdir2 & prv_speed <> zero, pbld, n, *sm05, e

if prv_speed <> speed | prv_spdir2 <> spdir2,

[

if speed, pbld, n, *speed, pspindle2, pgear, e

]

!speed, !spdir2

---

The second part would go in the toolchange area, ptlchg_com in my post;

code:

---

ptlchg_com      #Tool change common blocks

pcom_moveb

c_mmlt #Multiple tool subprogram call

pcan

if plane < 0, plane = 0

if mi5=1, pmoveout #<<<<<<<<<<<<<< Here's where I would try it

if stagetool >= zero,

[

pbld, "G91", "G30", "X0", "Y0", "Z0", e

pbld, "M06", *t, ptoolcomm, e

]

macrocount = macrocount + 10

35, no_spc, "930=", macrocount, e

---

Note: This was pulled from my mpmaster.pst

 

HTH

 

Tim

[kinglouie V]

Thanks Tim,

I'll work on it.

 

[kinglouie V]

Works nicely now!

thanks again!