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:

I can't believe I need to ask this.... Manual tool change


jaydenn
 Share

Recommended Posts

I added this at psof
	  pbld, n$, "G90 G00 Z15.", e$
	  pbld, n$, "G00 Y-10.", e$ 
	  pbld, n$,"M00", "(LOAD", *t$, ")", e$ 
          pcan
	  ptoolcomment
          pbld, n$,"("*t$, sm06, ")"e$   
=>
N3 G90 G00 Z15.
N4 G00 Y-10.
N5 M00 (LOAD T7 )
( 7/32  DRILL .2187 OSG  .5LOC .7CLR | TOOL - 7 | DIA. OFF. - 7 | LEN. - 7 | TOOL DIA. - .2187 )
N6 ( T7 M6 ) 

and this at pretract$

          pbld, n$, sccomp, *sm05, psub_end_mny, e$
          pbld, n$, "G90 G00 Z15.", e$ #sgabsinc, sgcode, *sg28ref, "Z0.", scoolant, e$
	  pbld, n$, "G00 Y-10.", e$ 

and this at ptlchg$

 

  
	  pbld, n$,"M00", "(LOAD", *t$, ")", e$ 
          pcan
	  ptoolcomment
          result = newfs(15, feed)  #Reset the output format for 'feed'
          pbld, n$,"("*t$, sm06, ")"e$ 

 

=>

N16 G90 G00 Z15.
N17 G00 Y-10.
( WEAR COMP FOR THIS TOOL D3 = .000 )
N18 M00 (LOAD T3 )
( 1/4 FLAT ENDMILL .75LOC 1.CLR | TOOL - 3 | DIA. OFF. - 3 | LEN. - 3 | TOOL DIA. - .25 )
N19 ( T3 M6 )

 

Too easy thanks to this forum and Colin's post classes.  Machines without tool changers are more rare than 5x machines.  Therefore post support is not a freebe.  

  • Like 1
Link to comment
Share on other sites

IMO, if there is a reason to do a manual tool change, IE large tool or special attachment, the logic to remove the tool should be done in the TC macro in the control. This is the only way to make sure nothing bad happens.

Here's how we do it:

TC macro checks the length and diameter to see if beyond limits of tool magazine. Or, tool is flagged as manual tool change only via macro variable (or tool table if available).

IF yes to either one of these, tc to empty pocket and move to operator position and prompt operator to put in tool (M00). When finished, move to operator and prompt removal (M00). Check tool presence signal in I/O to make sure spindle is empty and carry on.

 

No post mods and no chance of programmer or operator missing something.

 

MIke

  • Like 8
Link to comment
Share on other sites
16 minutes ago, GoetzInd said:

IMO, if there is a reason to do a manual tool change, IE large tool or special attachment, the logic to remove the tool should be done in the TC macro in the control. This is the only way to make sure nothing bad happens.

Here's how we do it:

TC macro checks the length and diameter to see if beyond limits of tool magazine. Or, tool is flagged as manual tool change only via macro variable (or tool table if available).

IF yes to either one of these, tc to empty pocket and move to operator position and prompt operator to put in tool (M00). When finished, move to operator and prompt removal (M00). Check tool presence signal in I/O to make sure spindle is empty and carry on.

 

No post mods and no chance of programmer or operator missing something.

 

MIke

Awesome tip Mike. 

  • Like 2
Link to comment
Share on other sites

If you have Heidenhain , in many cases , if your tool number exceeds the number of physical pockets ,  the machine will empty the spindle  and comes close to you asking for a tool.

Done , easy ...

 

Gracjan

Link to comment
Share on other sites
18 hours ago, jaydenn said:

Looks like I've upset the fanbois... Sorry I ever mentioned that Mastercam may in some way be flawed! Long live Mast3rcam!

My most humble apologies.

:P

Actually, you're just making yourself look like an asswhole. ;)

  • Thanks 1
  • Like 3
  • Haha 4
Link to comment
Share on other sites
On 5/31/2018 at 11:32 AM, jaydenn said:

Looks like I've upset the fanbois... Sorry I ever mentioned that Mastercam may in some way be flawed! Long live Mast3rcam!

My most humble apologies.

:P

Wow, Do you actually expect to get help from people with an attitude like that?

 

Feel free to ask anyone at CNC if they consider me a fanboy, I can guarantee the answer would always be no. But even with that I can honestly say your thoughts on Mastercam are flawed. The lack of a dedicated radio button in every path to do some obscure function that you have multiple other ways to accomplish already is not a flaw. What you are trying to do is a simple task, you are just choosing to make it more difficult on yourself. Manual entry being the easiest. You complain that it would be bad if you forgot to add that though. Well that is all on you. This is a trade where attention to detail is key. You had two people offer to edit your post for you and yet you keep complaining about not having time. Seems to me you just want to complain and nothing will stop your temper tantrum unless you get exactly what you want before you want it. A poor craftsman blames the tools for his failures.  

 

  • Like 9
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...