Post Modification For Makino A51NX Pro6 Control

[Justin Beebe at Folsom Tool]

We just purchased a Makino A51NX  four axis horizontal mill with a Professional 6 control.  The control is Fanuc based and it runs along side windows 7.  Oddly every tool has to have an H value of 1 and a D value of 1 called out in the program for the tool length and diameter offsets.

For example I need the code to be:

T1 H1 D1

T2 H1 D1

T3 H1 D1

I am using Mastercam 2018 and I started with the 2018 MPmaster post. I'm not sure how to force H1 and D1 output for every tool. 

Any help is greatly appreciated.

 

[Colin Gilchrist]

Do this:

At the top of your post, enter the following Global Formulas, starting in the Left Column. (MP is a column position dependent language.)

tloffno$ = 1

tlngno$ = 1

A Global Formula, will override MP's output, just prior to output to the NC File.

That last bit is important, because it just means that the Global Formula will cancel whatever MP was about to output, and output the value of the formula instead. So in this case, H1 and D1 will always be output, no matter what you enter in Mastercam. All you need to enter is the Tool Number.

Conversely,

If you were to enter this:

tloffno$ = t$

tlngno$ = t$

Those formulas tell MP to always make the H and D numbers, match the Tool Number.

[Justin Beebe at Folsom Tool]

Colin,

Thank you for helping me. Everything works perfectly. I added the lines to the post here. 

# --------------------------------------------------------------------------
# FORMULAS - global formulas
# --------------------------------------------------------------------------
toolcountn = toolcount + 1   # Index!
toolcountp = toolcount - 1   # Index!
tloffno$ = 1 # ADDED TO FORCE T1 OUTPUT FOR EVERY TOOL JB
tlngno$ = 1 # ADDED TO FOR D1 OUTPUT FOR EVERY TOOL JB    

Is this where you would typically add these lines

 

 

 

[Colin Gilchrist]

7 hours ago, Justin Beebe at Folsom Tool said:

Colin,

Thank you for helping me. Everything works perfectly. I added the lines to the post here. 

# --------------------------------------------------------------------------
# FORMULAS - global formulas
# --------------------------------------------------------------------------
toolcountn = toolcount + 1   # Index!
toolcountp = toolcount - 1   # Index!
tloffno$ = 1 # ADDED TO FORCE T1 OUTPUT FOR EVERY TOOL JB
tlngno$ = 1 # ADDED TO FOR D1 OUTPUT FOR EVERY TOOL JB    

Is this where you would typically add these lines

 

 

 

That is exactly where I would add them... 

[Justin Beebe at Folsom Tool]

Colin thank you again. You are the man.

[Colin Gilchrist]

I'm happy to help when I can Justin. Glad it is working for you. 

[Kampfzentrum]

On 3/10/2019 at 11:09 AM, Colin Gilchrist said:

I'm happy to help when I can Justin. Glad it is working for you. 

Wanted to explore this because I am experiencing the same issue. Now, I could make the suggested post modification above, but we have a shop with a number of various machine tools that all require D/H offsets to match the tool. So, in keeping things uniform, is there an internal parameter in the Makino controller that will enable it to accept D/H offsets with the same number as the tool?

Just curious.