HAAS post edit, adding Tool break detection to post

[sales]

Hello,

We are using the current generic Haas 3axis mill post.

I’m trying to add tool break detection G65 P9023 A24. H.003 T# , Im harcoding most of it just nned to get the current tool #.

It is almost working except it is taking the wrong T#.

It will take the next tool but I need it to use the current one.

See Line 729

How can we change this?

Please see attached post.

Mike

[Anonymous]

One way that may be simpler, is to write a quick macro sub-program that looks at the current tool in the spindle & performs a break check.  

One that I have seen online is as following:

O9000;
#100 = #3026; (#3026 = register for current tool in spindle. Assign to #100 which is a visible register)
G53G49Z0M09; (Z-AXIS Safety Retract)
G00G90;
G65P9023A24.T#100H.02; (Renishaw tool breakage routine, H = tolerance of tool +/- compared to set value before alarming)
G103; (Resets block look ahead to default value)
M62; (Turns off touch probe)
M99;

I did not write this, it comes from user "haastec" on the CNC Zone forum.  

You could use this, or write a similar program, then alias it to an unused m-code.  

Then you can simply have your post insert that M-code at the end of each Operation prior to tool change to probe for breakage. 

Good luck,

Steve

[sales]

I will try that, Thank you!

[Anonymous]

One other thing I forgot to mention.  

Instead of hard-coding in the m-code for tool check on every operation, you can setup your post so when you insert a "manual NC - Tool Break Control", your post will output that M-code for you.  

This way, you can do selective break checks on known problem tools.

If you want help implementing that, let me know.

Steve

[sales]

That's a great idea.

Do you have a post sample that is doing this already?

Thank you.

[Anonymous]

Sure,
I'll post something tomorrow. I didn't bring my computer home tonight.

Steve

[Anonymous]

Give this a look. 

I wrote it into the post you provided above.  

Every time you place a Manual NC - Tool Break Control, it will call an M-code.  
Currently i set it to M100, but you can pick whatever you like.  

One note: this only works properly if placed after all operations for the tool you are using are completed.  

If you need to break check a tool, then continue using that same tool, please place a "Manual NC - Force tool change" right after the break control.  

If you search thru the post for my last name "Piche", you will find where I made edits.  

Let me know if you have any questions.  

Steve

[sales]

Looks great, Thank you so much!

I will give everything a try shortly.

Mike

[Anonymous]

Glad I could help. 

Achim gave me pointers on adding this a couple years ago, so I figure I should "pay it forward".  

Let me know if you have any questions or need anything else.  

Steve

[sales]

One question, how do you turn it off?

Let say I have 10 operations, and I turn it on after operation 5 by inserting "Manual NC Tool break control" it will stay on till op 10.

Would we need to add a new  Type: Tool break OFF?

Thank you.

[Anonymous]

Oops, my error.  

Try this one.  

I had a capital letter where I should of had a lowercase.  

[sales · Accepted solution]

Great it all works including the Haas macro.

Thank you!

[sales]

I noticed if we Pattern a tool path (order by tool ) it puts a M100 even if it just move over to the next pattern.

Which would be a problem because the spindel would not be running after the macro.

This might be more complex to fix.

Thank you.

Mike