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:

Dumb Question: How to remove Opt Stop at tool change?


Recommended Posts

Hey All,

For Background I'm running Mastercam 2018 and posting to a Haas VF3-SS. I'm running multiple variations on a program which has 14 tool changes in it. The Haas machine automatically looks ahead to pre-load the next tool - Unless there is a M01 - in which case the Haas cant look past it.

I looked through the control definition / machine definition / Tool path manager to see if there was a setting to disable it per tool or per program but I couldn't locate one. (Though to be fair I may have missed it)

So my dumb question, what setting in the post processor adds the M01 before a tool change?  Should I just add the "#" before it to comment it out? My best case scenario would be able to have it off by default but use canned text to put it on.

Thanks for any and all help

Link to comment
Share on other sites

I don't think removing it is a good idea. 

It is useful in setup of if you want to adjust a tool and need the current mood to finish.

But in the control def there should be a check box for enable staged tool routine.

 

But it's usually in the pretract post block and looks like -   sm01

 

You can use the # to prevent it

Link to comment
Share on other sites

If you are using the default Haas Mcam post. Turn on the prestage in the control definition as mentioned. This way you get a forced prestage, rather than relying on the control reading the next tool change to prestage. 

Deleting your M01 is not a good idea.

Link to comment
Share on other sites

First, there is no such thing as a dumb question. Everyone of us started as a blank slate; born into this world knowing nothing. Everything we know, was unknown to us before we learned it. So don't ever feel ashamed for asking.

I will tell you the answer, because I believe that every question asked in good faith deserves a good answer. But I'll also tell you how you can find the answer yourself. By knowing where to look for the answer, I'm hoping you'll discover many other things that could help you in the future.

In the Generic Haas Posts (and other Generic Posts) from CNC Software, there is a "variable switch" that controls the output of "M01". It is actually a "3-way" switch, with the 3 options being "Off", "M01", and "M00".

Open your Post Processor in a Text Editor (Code Expert is the best for Post Editing). Search for 'prog_stop'. Here is what that switch looks like:

prog_stop    : 1     #Program stop at toolchange: 0=None, 1=M01, 2 = M00

Change the '1' to '0', and it will eliminate the output of "M01".

Ok, but how did I know that?

At the top of every Post Processor, is a section of "comments" that are designed to be read by the user. There is a great deal of information there, that explains to you, if you read it, how the Post is setup to function (by default), but also "features" that the Post Writer has written into the Post.

I read the following comment at the top of the Post:

# - Switch for output of M00 or M01 at tool change (3 position switch, off, M00, M01 - see prog_stop)

So that single comment tells me that there is a switch that can be used to disable the "M01". In addition, it even tells me the name of the variable to search for; 'prog_stop'.

This Post has a bunch of "switches" to control the output of the code from your Post.

These "Switches" can change the following items:

  1. "on/off" Spindle Gear codes. (use_gear)
  2. force "Rigid Tapping". (use_rigid)
  3. Force output of "Work Offset" (G54, G55, G56, ... G54.1 Pxx), at each Tool Change (Yes/No)
  4. Force "uppercase" characters for Program Name?
  5. Tool Information: Controls Tool List, and/or Tool Comments at Tool Change (tool_info)
  6. Output XY Zero Reference Return at Tool Change (tlchg_home)
  7. Output G52 Shift for Subprogram Output (use_g52_shft)
  8. Comment Mode: Shorten or Truncate Comments over 80 characters.
  9. Force "Rotary Axis" Reset at Tool Change (frc_cinit)
  10. Output M-Code for Signed Direction (use_rotmcode)
  11. Enable "Lock/Unlock" M-Codes (use_rot_lock)

There are plenty of other "switches", but these are controlled either by the Control Definition, or the Machine Definition. This is reflected in the comments that follow these variables. Since they are "CD or MD" variables, the settings in the CD or MD override the settings inside the Post. That means that these "MD or CD" switches have to be changed inside the Machine or Control Definition Manager, inside Mastercam.

The most important thing I can point out here is that you should read the comments in the header of your Post!!!

This will go a long way towards helping you understand some features that are already built into the Post and Mastercam. For example, the Miscellaneous Integers and Real Numbers are "input parameters" that exist in every Operation inside Mastercam. By changing the values for these MI or MR values, you can change the NC Code output from the Post.

For example, read about how Miscellaneous Integer #1 can be used to output "Work Offsets" (2), "G52 Shift Only" (3), or both "Work Offset and G52" at the same time (4).

Another option to understand is "Canned Text", and how it is used by default to control Block Delete.

 

 

 

  • Like 5
Link to comment
Share on other sites
  • 5 weeks later...
On ‎1‎/‎5‎/‎2018 at 1:12 PM, Colin Gilchrist said:

First, there is no such thing as a dumb question. Everyone of us started as a blank slate; born into this world knowing nothing. Everything we know, was unknown to us before we learned it. So don't ever feel ashamed for asking.

I will tell you the answer, because I believe that every question asked in good faith deserves a good answer. But I'll also tell you how you can find the answer yourself. By knowing where to look for the answer, I'm hoping you'll discover many other things that could help you in the future.

In the Generic Haas Posts (and other Generic Posts) from CNC Software, there is a "variable switch" that controls the output of "M01". It is actually a "3-way" switch, with the 3 options being "Off", "M01", and "M00".

Open your Post Processor in a Text Editor (Code Expert is the best for Post Editing). Search for 'prog_stop'. Here is what that switch looks like:


prog_stop    : 1     #Program stop at toolchange: 0=None, 1=M01, 2 = M00

Change the '1' to '0', and it will eliminate the output of "M01".

Ok, but how did I know that?

At the top of every Post Processor, is a section of "comments" that are designed to be read by the user. There is a great deal of information there, that explains to you, if you read it, how the Post is setup to function (by default), but also "features" that the Post Writer has written into the Post.

I read the following comment at the top of the Post:


# - Switch for output of M00 or M01 at tool change (3 position switch, off, M00, M01 - see prog_stop)

So that single comment tells me that there is a switch that can be used to disable the "M01". In addition, it even tells me the name of the variable to search for; 'prog_stop'.

This Post has a bunch of "switches" to control the output of the code from your Post.

These "Switches" can change the following items:

  1. "on/off" Spindle Gear codes. (use_gear)
  2. force "Rigid Tapping". (use_rigid)
  3. Force output of "Work Offset" (G54, G55, G56, ... G54.1 Pxx), at each Tool Change (Yes/No)
  4. Force "uppercase" characters for Program Name?
  5. Tool Information: Controls Tool List, and/or Tool Comments at Tool Change (tool_info)
  6. Output XY Zero Reference Return at Tool Change (tlchg_home)
  7. Output G52 Shift for Subprogram Output (use_g52_shft)
  8. Comment Mode: Shorten or Truncate Comments over 80 characters.
  9. Force "Rotary Axis" Reset at Tool Change (frc_cinit)
  10. Output M-Code for Signed Direction (use_rotmcode)
  11. Enable "Lock/Unlock" M-Codes (use_rot_lock)

There are plenty of other "switches", but these are controlled either by the Control Definition, or the Machine Definition. This is reflected in the comments that follow these variables. Since they are "CD or MD" variables, the settings in the CD or MD override the settings inside the Post. That means that these "MD or CD" switches have to be changed inside the Machine or Control Definition Manager, inside Mastercam.

The most important thing I can point out here is that you should read the comments in the header of your Post!!!

This will go a long way towards helping you understand some features that are already built into the Post and Mastercam. For example, the Miscellaneous Integers and Real Numbers are "input parameters" that exist in every Operation inside Mastercam. By changing the values for these MI or MR values, you can change the NC Code output from the Post.

For example, read about how Miscellaneous Integer #1 can be used to output "Work Offsets" (2), "G52 Shift Only" (3), or both "Work Offset and G52" at the same time (4).

Another option to understand is "Canned Text", and how it is used by default to control Block Delete.

 

 

 

Hi Colin,
   Is there away can I make it switches from M01 to M0 when I use MANUAL ENTRY AS CODE?

 

like...
 

M1....
cut here....
M0(if Next operation is MANUAL ENTRY AS CODE)

X.. Y... CUT... (from MANUAL ENTRY AS CODE)

Thank you Colin.

 

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...