How to get feed in mm/rev in Face contour operation for lathe

[vikc]

Hello Gents,

How can I get feed value in mm/rev for Milling toolpath in lathe?

My output is in G98 I need to convert it into G99.

[AHarrison1]

Depends on what control you are using.

On our HAAS G99 commands Feed Per Revolution. This ties in with spindle RPM commanded by S (S1000) and M03

This does not work if we are using live tooling as the RPM is commanded by a P (P1000) and  a different M to turn on the Live Tooling.

 

[BehindYou]

Greetings @Hemkant HEMKANT

This is how I did in my post

Go in prpm  postblock
and search for sgfeed string
 pbld, n$, [if nc_system_type = 0, *sgfeed], [if nc_system_type >= 1, *sgfeed_b] *sg97, *speed, "P12" , *spindle_m, e$
What I did above?
If I change variable  nc_system_type  to value 1 it will output G99 if  I keep value 0 output is G98
( depends which G-system code I am using)
N170 G98 G97 S2315 P12 M03

Or just change string sg98 

 

# --------------------------------------------------------------------------
# Feed mode G code selection
sg98    : "G98"      #UPM  Fanuc A Group of G-code
sg99    : "G99"      #UPR  Fanuc A Group of G-code
sgfeed  : ""         #Target string

fstrsel sg98 ipr_actv$ sgfeed 2 -1
# --------------------------------------------------------------------------
# Feed mode G code selection
sg98_b    : "G94"      #UPM  Fanuc B Group of G-code
sg99_b    : "G95"      #UPR  Fanuc B Group of G-code
sgfeed_b  : ""         #Target string

fstrsel sg98_b ipr_actv$ sgfeed_b 2 -1
# --------------------------------------------------------------------------

But you should provide more information's how your output should look like for the milling mode and turning mode so I can give you accurate info where/what and how to change.
 

Once again example above is how I did for my machine (Controller (Fanuc) machine (puma 5100)))

Kind regards

Ivan Žugec