Using D#517 for cuttercomp

[MIL-TFP-41]

On our matsuura's we do on occasion use sister tooling. The way it works with them, you can have multiple tool #1 (for example). When you call the height offset rather than using H1 you use H#518 and via the toolchange macro it loads the correct length offset.

 

Up till now, it has been roughing tools with little or no need for CDC. Things change, and now I want to post out D#517 rather than D1.

The way I have gotten the height to work is by this....

pbld, n$, "G43", "H", no_spc$, 35, no_spc$, "518", pfzout, e$

This works well since typically you only call your tool height once after a toolchange. However, CDC is turned off & on constantly.....

 

So is there any way to re-format this statement...

fmt  "D" 4  tloffno$    #Diameter Offset No

to something that will always force out D#517, no matter what tool is called?

[Guest]

I haven't tried it but...

 

What if you commented out that variable definition

 

#fmt "D" 4 tloffno$

 

and instead

 

tloffno$ : "D#517"

 

Like I said, not sure it will work but thinking out of the box at the moment

[MIL-TFP-41]

JParis got me going in the right direction on this. A few trial and errors and here is what I came up with....

 

First, changed my format to this...

 

fmt  "D#" 4  tloffno$    #Diameter Offset No

 

I didn't think that would work, and in previous versions I know it wouldnt work, as it used to see anything behind the # sign as a comment and it would ignore the rest of the line. However, after trying, it worked.

Then in my pccdia section just added this line....

 

tloffno$ = 517

 

and now my output looks like so...

 

G43 H#518 Z.1
G1 Z0. F6.42
G41 D#517 X-.9085
X1.6711
G2 X1.9211 Y1.3462 I0. J-.25

[MIL-TFP-41]

duplicate....