Lathe threading problem

[DaveR]

Using a fanuc OT-c, generic Fan 2x post

 

For the G76 cycle I need X,Z,R,P,Q,F output

 

Instead of F I get the feed rate post output preceded by an E

 

Like so:

 

 

G97 S499 M03

G0 X1.17 Z.3588

G76 P012429 Q0. R.001

G76 X1.421 Z-.45 P255 Q87 R0. E.04167

M9

 

Machine errors out I am assuming this is the problem I may be wrong, I am totally new to lathe programming.

 

Thanks for any advice.

 

Dave

[Guest]

In this section

 

code:

---

pfr_l           #Format feedrate for lathe

if opcode$ = 104,

[

#Format feedrate for lathe thread

result = nwadrs(stre, feed)

result = newfs (19, feed)

]

else,

[

result = nwadrs(strf, feed)

result = newfs (18, feed)

]

---

comment out this line

 

code:

---

result = nwadrs(stre, feed)

---

[DaveR]

Appreciate the help, please forgive me but what does "comment out" mean?

 

Dave

[Guest]

Place a # sign in front of the offending line

 

 

[DaveR]

Thanks a lot John!

 

*edit* worked!

 

Dave

[DaveR]

OK the change to the post worked but the control still chokes here on the Qs

 

G76 P012429 Q.005 R.001

 

I need that Q value to be a radial value with no decimal.

 

Example I see in the book is "Q003"

 

I changed it by hand and got it to run.

 

Is there a post change for that?

 

Dave

 

[ 01-24-2009, 09:30 PM: Message edited by: DaveR ]

[Guest]

Dave find the fs 2 statements and add this one at the bottom

 

code:

---

fs2 25  0 4 0 3      #No Decimal, no trailing

---

then find this line

 

code:

---

fmt  Q  2   thdlast$     #Last depth cut in thread

---

and change it to this

 

code:

---

fmt  Q  25   thdlast$     #Last depth cut in thread

---

[DaveR]

Amazing

 

Thanks a lot John.

 

Dave

[Guest]

Glad to help Dave

 

[g-codeguy]

Don't know if your post looks like this, but if it does, then this is where I changed my threading feedrate from 'E' to 'F'. I included the whole section to make it easier to find. Sorry 'bout that.

 

# General Output Settings

# --------------------------------------------------------------------------

force_wcs : no$ #Force WCS output at every toolchange? #AG-

progname$ : 1 #Use uppercase for program name

css_start_rpm : yes$ #Do direct RPM spindle start prior to CSS? #AG-

css_end_rpm : no$ #Do direct RPM spindle prior to Retract? #AG-

prog_stop : 1 #Program stop at toolchange: 0=None, 1=M01, 2 = M00

tool_info : 2 #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 : 1 #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 : 0 #Thread pitch address for lathe threading, 0 = Use F, 1 = Use E

use_clamp : 1 #0 = No, 1 = Clamp

use_brake : 1 #0 = No, 1 = Brake

lathe_stop : 0 #Stop lathe spindle on lathe tool change? 0 = no, 1 = yes

drop_offset : 0 #Drop offset at end of tool? 0 = no, 1 = yes #AG-

tseqno : 3 #Output sequence number at toolchanges when omitseq = yes

#0=off, 1=seq numbers match toolchange number, 2=seq numbers match tool number 3=seq numbers match offset number #AG- Added 3

 

This section may be set up for our lathes rather than from the generic post. Couldn't say as I am not the one who created our posts. I only make an occasional change to get the correct output.

[Guest]

g-codeguy, just as an FYI for others who may find this thread, he is using the 2ax generic post, yours is out of the MPLMaster.

[g-codeguy]

Thanks, John, I see you posted while I was editing mine. I'm just too slow a typer!

[g-codeguy]

Thanks, John, I see you posted while I was editing mine. I'm just too slow a typer!