X6 post setup questions (sub program and canned text)

[Matt@RFR]

Hey guys, I'm trying to help a friend get his post cleaned up. He's running a Haas 3 axis VMC, X6 and is using the generic machine and control definitions. The post is MPFAN.

I've got everything done that he wanted except two things I can't seem to figure out: Is it possible to post local sub programs (M97) with N addresses for the subs, versus the M98 and P address it's posting now? Everything I've changed in the control definition under subroutines has done nothing to change this, and I can't find an area in the post that has switches to go from M98 to M97.

The other question I have is how to use custom canned text. I added G187 P1 E0.025 (which is exactly what he wants to see in the posted code) to position 11 in the control definition and saved it, but it refuses to add anything but "M11" to the NC code. It shows up fine in the canned text dialog while creating tool paths, it just doesn't post correctly.

I'm having fun learning how to do this on my own, but just got stuck on these two things. Any help would be appreciated.

[MMTZ]

Have you give a try to the Haas Machine Def's and posts?? I think MC comes with a couple Good ones that don't need more editing.

What's that G187 for? Does it need to be a canned text option? What are you trying to acomplish? 1st of all Canned Text from the control does not post the text you see on the CD, you have to configure your post for it, i.e. It doesn't really outputs the G187 you entered on the CD but it's position within the menu.

HTH

[txcncman]

When I last visited this problem with Matt, we had over come the G97 Pxxxx issue in his post processor. Still need to output Nxxxx for the local sub-programs instead of Oxxxx.

[Matt@RFR]

You guys are right, just using a manual entry for the G187 works just fine. Thanks.

For the local subroutine structure, I thought I found where to change the O call for the sub, but changing it had no effect at all. See the two "N" s... neither had any effect. But changine the "O" in the top line does change the main program number, so I figured I was in the right place, but I guess not. What does the 7 mean in each line?

#Move comment (pound) to output colon with program numbers
fmt  "O" 7  progno$     #Program number
#fmt ":" 7   progno$     #Program number
fmt  "N" 7  main_prg_no$ #Program number
#fmt ":" 7   main_prg_no$ #Program number
fmt  "N" 7  sub_prg_no$ #Program number
#fmt ":" 7   sub_prg_no$ #Program number
fmt  "X" 2  sub_trnsx$  #Rotation point
fmt  "Y" 2  sub_trnsy$  #Rotation point
fmt  "Z" 2  sub_trnsz$  #Rotation point

[MMTZ]

Leave the mods you are showing on your last comment and then give this a shot, look for this on your post:

psub_st_m$ #Header in main level
result = nwadrs(stro, main_prg_no$)
" ", e$
*main_prg_no$, e$
#G51/G68 requires absolute position on first move
if mr_rt_rst,
[
sav_absinc = absinc$
if absinc$ = one,
[
absinc$ = zero
prv_absinc$ = m_one
prv_xabs = m_one
prv_yabs = m_one
]
]
else, pbld, n$, sgabsinc, e$


And then try and remove the text in red. Remember to always make a copy of your post before you modify it!!!

So you're all set with the G187??? Can you share a snippet of the code using it?

[txcncman]

Numbers like the 7 and 2 are the format pattern for the numbers.

# --------------------------------------------------------------------------
# Format statements - n=nonmodal, l=leading, t=trailing, i=inc, d=delta
# --------------------------------------------------------------------------
#Default english/metric position format statements
fs2 1 0.7 0.6 #Decimal, absolute, 7 place, default for initialize ( : )
fs2 2 0.4 0.3 #Decimal, absolute, 4/3 place <---------Format Statement 2
fs2 3 0.4 0.3d #Decimal, delta, 4/3 place
#Common format statements
fs2 4 1 0 1 0 #Integer, not leading
fs2 5 2 0 2 0l #Integer, force two leading
fs2 6 3 0 3 0l #Integer, force three leading
fs2 7 4 0 4 0l #Integer, force four leading <---------Format Statement 7
fs2 9 0.1 0.1 #Decimal, absolute, 1 place
fs2 10 0.2 0.2 #Decimal, absolute, 2 place
fs2 11 0.3 0.3 #Decimal, absolute, 3 place
fs2 12 0.4 0.4 #Decimal, absolute, 4 place
fs2 13 0.5 0.5 #Decimal, absolute, 5 place
fs2 14 0.3 0.3d #Decimal, delta, 3 place
fs2 15 0.2 0.1 #Decimal, absolute, 2/1 place (feedrate)
fs2 16 1 0 1 0n #Integer, forced output
fs2 17 0.2 0.3 #Decimal, absolute, 2/3 place (tapping feedrate)

# This format statement is used for sequence number output
# Number of places output is determined by value for "Increment Sequence Number" in CD
# Max depth to the right of the decimal point is set in the fs statement below
fs2 21 0^7 0^7 #Decimal, 7 place, omit decimal if integer value
fs2 22 0^3 0^3 #Decimal, 3 place, omit decimal if integer value

[Matt@RFR]

result = nwadrs(stro, main_prg_no$)

Doing this makes the sub line from an O to a P, which I don't understand since I've got N's in the area I posted earlier. This is not so bad... he can just replace the P's with N's manually. Would be nice to not have to do that, but it certainly isn't the end of the world. To be clear it was:

M97 P1
and
O1

Now it's M97 P1
and
P1 ---- This is the line that needs to be N1.

So you're all set with the G187??? Can you share a snippet of the code using it?

G187 for Haas controls both accuracy and acceleration rate of the axes. G187 P1 E0.025 tells the control to go into "rough" mode (faster acceleration) and to set max corner rounding to .025", which is the default. Setting this to G187 P1 E0.050 will make these things really fly around 3D parts, but you best have atleast .075 of material left on the part to avoid gouges in the finished part when feeding at 350 IPM and up. This tuning works well with HSM toolpaths as well. The way he's using it now is to do a manual entry of G187 Pp Ee.eee before his roughing toolpaths, then a manual entry of G187 with no inputs (which sets it back to default) after his roughing toolpaths. In retrospect, this actually works better than the canned text I was originally after, since this way he's free to enter any values he wants instead of picking for a short list.

txcncman, thanks for the explanation. I applied that to these sub calls and got exactly what I wanted. It was 7 (outputs 0001), I changed it to 4 (outputs 1).

[MMTZ]

then try this:

result = nwadrs(strn, main_prg_no$)

[Matt@RFR]

No dice, that changed nothing in the posted code. Thanks a lot for the help, but don't spend any more time on this. It's not a big deal to just change the sub addresses.