Feedrate Setting In Post

[phoodieman]

This pertains to lathe. The generic post works great for me except when threading. It posts out an "E" instead of an "F". Once I edit to F everything runs good. It only puts the E when threading. All other operations use an F. So where in the post can I change to get the F I need?

Phoodieman

[concoo]

it easy to do .
open the post -> goto here
# --------------------------------------------------------------------------
# General Output Settings
# --------------------------------------------------------------------------
force_wcs : yes$ #Force WCS output at every toolchange?
progname$ : 1 #Use uppercase for program name
css_start_rpm : yes$ #Do direct RPM spindle start prior to CSS?
css_end_rpm : yes$ #Do direct RPM spindle prior to Retract?
prog_stop : 1 #Program stop at toolchange: 0=None, 1=M01, 2 = M00
tool_info : 3 #Output tool information?
#0 = Off - Do not output any tool comments or tool table
#1 = Tool comments only
#2 = Tool table only
#3 = Tool comments and tool table
use_pitch : 0 #0 = Use feed for tapping (force Feed/Min), 1 = Use pitch for tapping (force Feed/Rev)
rigid_tap : 1 #0 = Floating tap output
#1 = Rigid tap output (Set parameter 5200 bit 0 to 1 for rigid)
#(Set M code for rigid tap in parameter 5210)
tap_feed : 1 #0 = 2/1 (in/mm) decimal places, 1 = 4/3 (in/mm) decimal places
thread_address :1 #Thread pitch address for lathe threading, 0 = Use F, 1 = Use E

change number 1 to 0 at red color, you will got F instead of E .
hope it will help .

[phoodieman]

it easy to do .
open the post -> goto here
# --------------------------------------------------------------------------
# General Output Settings
# --------------------------------------------------------------------------
force_wcs : yes$ #Force WCS output at every toolchange?
progname$ : 1 #Use uppercase for program name
css_start_rpm : yes$ #Do direct RPM spindle start prior to CSS?
css_end_rpm : yes$ #Do direct RPM spindle prior to Retract?
prog_stop : 1 #Program stop at toolchange: 0=None, 1=M01, 2 = M00
tool_info : 3 #Output tool information?
#0 = Off - Do not output any tool comments or tool table
#1 = Tool comments only
#2 = Tool table only
#3 = Tool comments and tool table
use_pitch : 0 #0 = Use feed for tapping (force Feed/Min), 1 = Use pitch for tapping (force Feed/Rev)
rigid_tap : 1 #0 = Floating tap output
#1 = Rigid tap output (Set parameter 5200 bit 0 to 1 for rigid)
#(Set M code for rigid tap in parameter 5210)
tap_feed : 1 #0 = 2/1 (in/mm) decimal places, 1 = 4/3 (in/mm) decimal places
thread_address :1 #Thread pitch address for lathe threading, 0 = Use F, 1 = Use E

change number 1 to 0 at red color, you will got F instead of E .
hope it will help .

This is the General Settings Info....no mention of feed rate there. I have looked for the thread addres info. Couldn't find that. Has to be in the post somewhere I just can't figure out where. I checked the G76 section. couldn't see anything having to do with feedrate.
# --------------------------------------------------------------------------
# General Output Settings
# --------------------------------------------------------------------------
sub_level : 1 #Enable automatic subprogram support
breakarcs : 1 #Break arcs, 0 = no, 1 = quadrants, 2 = 180deg. max arcs
arcoutput : 1 #0 = IJK, 1 = R no sign, 2 = R signed neg. over 180
arctype : 2 #Arc center 1=abs, 2=St-Ctr, 3=Ctr-St, 4=unsigned inc.
do_full_arc : 0 #Allow full circle output? 0=no, 1=yes
helix_arc : 0 #Support helix arc output, 0=no, 1=all planes, 2=XY plane only
arccheck : 1 #Convert small arcs to linear
atol : .01 #Angularity tolerance for arccheck
ltol : .002 #Length tolerance for arccheck
vtol : .0001 #System tolerance
maxfeedpm : 500 #Limit for feed in inch/min
lcc_move : .05 #Enter the move in X, Z for lathe canned cycle comp.
ltol_m : .05 #Length tolerance for arccheck, metric
vtol_m : .0025 #System tolerance, metric
maxfeedpm_m : 10000 #Limit for feed in mm/min
lcc_move_m : 1.25 #Enter the move in X, Z for lathe canned cycle comp.,mm

force_wcs : yes #Force WCS output at every toolchange?
spaces : 1 #Number of spaces to add between fields
omitseq : no #Omit sequence numbers? (use -1 to enable sequence for LCC)
seqmax : 9999 #Max. sequence number
nobrk : no #Omit breakup of x, y & z rapid moves
progname : 1 #Use uppercase for program name
rotaxtyp : 3 #Rotary axis type for toolplane
tooltable : 3 #Read for tool table and pwrtt (3 recalls pwrtt at sof)
ref_ret : 0 #G29 / G30 return variable from Mi3
css_start_rpm : yes #Do direct RPM spindle start prior to CSS ?

Phoodieman

[phoodieman]

I did a search for E and F and found this. I noticed the stre and strf callouts

# ---------------------------------------------------
#String and string selector definitions for NC output
# ---------------------------------------------------
#Address string definitions
stra "A" #String for address A
strd "D" #String for address D
stre "E" #String for address E
strf "F" #String for address F
stri "I" #String for address I
strk "K" #String for address K

Then I searched for stre and found this....

#Format feedrate for lathe thread
result = nwadrs(stre, feed)
result = newfs (19, feed)

When I changed the stre to strf I got the F for feedrate in the posted out program. What a hassle.

Phoodieman