Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Adding optional stop to my post


ToddF
 Share

Recommended Posts

I would like to have the code for optional stop post out in my programs.  I thought there used to be a place you could turn that on in the control definition, but I dont see it.  I dont know much about modifying my post to do that.  Any help would be great.

Link to comment
Share on other sites

This has been built into almost every Post that is available for Mastercam.

The "switch" is used inside the Post as others have mentioned, to enable the Optional Stop after every Operation. (Actual Tool Change) 

If you want to control where the Op Stop is output (you only want it on some Ops, but not on others), then you can use the Canned Text function (every Op has Canned Text), to output the M01 where you need it.

Link to comment
Share on other sites

The post that I am using is a Generic Fanuc 3X Mill.pst.   I can see in the beginning of the post the prog_stop    : 1     #Program stop at toolchange: 0=None, 1=M01, 2 = M00.  

I would like to have M01 post out before every tool change and am not sure where in the post to make that happen.  I can attach a copy of my post if that would help?

Link to comment
Share on other sites
34 minutes ago, ToddF said:

I would like to have M01 post out before every tool change and am not sure where in the post to make that happen.  I can attach a copy of my post if that would help?

Is it posting an M01 at all? 

Look for this -

#Cantext string definitions (spaces must be padded here)
sm00         : "M00"
sm01         : "M01"

Make sure that sm01 has the "M01" between the quotes.

Then look for -

#region Tool change / stage tool
ptlchg$          #Tool change

see if you have this line and that it is not commented out

      if prog_stop = 1, pbld, n$, *sm01, e$

 

10 hours ago, Colin Gilchrist said:

The "switch"

LOL.  oops.. I meant "switch". 

  • Thanks 1
Link to comment
Share on other sites

#Cantext string definitions (spaces must be padded here)
sm00         : "M00"
sm01         : "M01"  (This line wasn't in there)

 

#region Tool change / stage tool
ptlchg$          #Tool change

      if prog_stop = 1, pbld, n$, *sm01, e$  (The *sm01 wasn't in there either)

  • Like 1
Link to comment
Share on other sites

might be jimmying this thread but how do you get it to post an M0 at the end of a tool, was just screwing around after reading this thread and couldnt figure it out. read the help file but wasnt much help. can you add text like after a tool, check inserts. how is it controlled? say you want to add an M0 before tapping to add oil or "lube me up" as i always put.

Link to comment
Share on other sites
11 hours ago, Grimes said:

might be jimmying this thread but how do you get it to post an M0 at the end of a tool, was just screwing around after reading this thread and couldnt figure it out. read the help file but wasnt much help. can you add text like after a tool, check inserts. how is it controlled? say you want to add an M0 before tapping to add oil or "lube me up" as i always put.

 

Just look for the M06 call and put an M00 after that:

t$, " M06", e$

"M00", e$

Link to comment
Share on other sites
On 10/18/2018 at 5:50 AM, jlw™ said:

You can always to a manual data entry between ops.  You can use canned text for a lot of that and  you can use toolpath editor to put it basically any where you want.

explain this more jlw

 

On 10/18/2018 at 8:43 AM, Mark VIII said:

 

Just look for the M06 call and put an M00 after that:

t$, " M06", e$

"M00", e$

ya i could probably change that just on the tapping cycle, but what if you dont want it all the time?

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...