[Xeno]

I have a haas SL-30
Mastercam X5 using Lathe Default

I want to thread using G32 command but it outputs a E instead of F

It's set up for NC code format: Long Hand
Snippet of the code is below,

G20
G0 T707
G18
G97 S200 M03
G0 G54 X1.9823 Z.2115
X2.2085
G99 G32 Z-1. E.0625
...

I wanted to change the "E.0625" to "F.0625"
when it outputs the g-code.
I looked in the post but it's not obvious where to change it.
Any idea how to do it?

Thanks
Tony

[txcncman]

Upload a copy of the post processor you are using.

[Superman]

Upload a copy of the post processor you are using.

Tx,
please do not be offended, but

-why has everyone have to upload their post to a public forum for you & everyone else to see.
Many put hard earned hours/days/weeks into that post, just to have some piracy noob knock it off.

It is in all legal user's interest to show a little restraint, in giving away a complete post. I also find it better to guide the thread starters into doing it themselves, ( so they learn post editting in the process )


Xeno
- read the upper section of your post, tells you how to program your part while using this post
Look in your post (general output settings) for the "thread_address" setting, change it from 1 to 0 to have F output instead of the E.

(didn't have a Haas post, this is from the MplmasterX5.pst....it should be nearly identical)

# --------------------------------------------------------------------------
# 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
use_clamp    : 1     #0 = No, 1 = Clamp
use_brake    : 1     #0 = No, 1 = Brake

[txcncman]

Because his post might not use that method for output? Now, I guess he could be asked, "Does your post have this line...?" Then told, "Change it to this..." But then you can get into a lot of back and forth exchanges of, "I didn't find that. Now what do I do." So, to me, it is easier to cut the chase and see the post myself. Everyone has their own style. I do not mind trying to help - if helping is not made too difficult. Just because we differ on methods, and having butted heads in the past, I will try to leave all future MasterCam questions for you, the expert, to answer them, no matter how many days it might take you to get around to answering them (if ever at all). Have a nice day.

[Xeno]

I have the default post mcamx5/lathe/post/MPLFAN.pst
the clip of Tx's post above isn't in my post.
I don't see any options for using either E or F
What does work is changing the stre variable of the clip below...

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

... so changing it to
stre : "F" #String for address E

For my 2001 Haas SL30 I never use the parameter "E"
Tony

[txcncman]

The expert will get to this in his own time frame. Good luck.

[Superman]

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

... so changing it to
stre : "F" #String for address E

That will work, but,,, if there is any other place that requires an E address, it will pump out an F.

If you want to alter the area that controls that output, this may be the best option

look in your post for the "Motion output components" section
- it is a "feed" component that we need to find
in the post for G32 threading, it looks for a pffr for the feed calcs
- pffr first does the pfr_l postblock before outputting the feed address, which has the change of F to an E, we need to comment that actual part out, but we need to keep everything else. The next line is a format statement for how many decimal places, you need threading (which is opcode$=104) to be accurate. So it will take up 5 decimal places in inch mode ( fs19

pffr            #Output feedrate, force
       pfr_l
      *feed
pfr             #Output feedrate
       pfr_l
      `feed
pfr_l           #Format feedrate for lathe
      if opcode$ = 104,
        [
        #Format feedrate for lathe thread
        #result = nwadrs(stre, feed)
        result = nwadrs(strf, feed) 
        result = newfs (19, feed)
        ]
      else,
        [
        result = nwadrs(strf, feed)
        result = newfs (18, feed)
        ]

Put the red #, & you should be good to go
or you could do what is marked in blue....change the E output to F, which doesn't change it at all.
----- this is what you suggested, but in the incorrect area

[MetalZilla]

Not sure why output with an E instead of an F is so undesirable? I know that when E is used you can actually carry the feed to 6 decimal places for greater accuracy.
Machining Formulas