posting tap cycle

[jeffl]

I am using Mastercam v8 with an old OKK cnc mill. The post processor that I am using does not produce the correct line of code for a canned tap cycle. The post has the following:

 

ptap # Canned Tap Cycle

pdrillref

n, drillref, sgdrill, *x, *y, *depth, *refht, pdwell, *frplunge, e

 

... and produces:

 

G99G84X-1.125Y-.625Z-.5R.1F1.

 

I need the line to have the # of threads at the end of the line of code. for example:

 

G99G84X-1.125Y-.625Z-.5R.1F1.E13

 

for 1/2-13 tap.

 

How can I do this?... it has to be be something simple that I am not seeing.

 

Thanks

[Roger Martin from CNC Software]

The information you need can be accessed from the "n_tap_thds" post variable.

You will want to format "n_tap_thds" for the desired output formatting.

 

Something like ->

 

# Create a format specification (if needed)

fs2 17 2 0 2 0n # Integer

 

# Format the "n_tap_thds" variable

fmt E 17 n_tap_thds #Tapping "feed"

 

 

Then replace the "*frplunge" in the PTAP postblock to be "*n_tap_thds"

 

 

*** Was this ->

 

ptap # Canned Tap Cycle

pdrillref

n, drillref, sgdrill, *x, *y, *depth, *refht, pdwell, *frplunge, e

 

 

*** Now this ->

 

ptap # Canned Tap Cycle

pdrillref

n, drillref, sgdrill, *x, *y, *depth, *refht, pdwell, *n_tap_thds, e

[jeffl]

thanks, it worked