Mastercam & Haas TL-2

[t.lewis]

Mastercam X3MU1. Haas TL-2 with turret and tailstock.New 1 1/2 months ago. Still trying to get a fully working post for my TL-2 Hass lathe. Have contacted my reseller about issues I am having and they keep telling me they are working on it. I still can not thread using canned cycle (unless I edit the NC file) but it will do it in boxed. I am unable to select Home possition, the post always sends turret to machine home to change tools and that does not work well when you need the tailstock. I have been able to edit the NC file to insert my selected home position but it is a pain when you have to do that every time. Thanks for all the responces.

[Superman]

We do try to help whereever possible,
*****Remember COPY YOUR POST before doing any alterations****
and TEST it very often. ( finding that a comma or a $ is missing is hard when major changes have occured ).
if the altered post stuffs up, it is easier to restore the last good post.

What basic post has been adapted to your HAAS ?
Paste in the top 10 lines


also show us what you need altered ( eg from this to be this )

This is what is posting

I want this

We will try to suggest the best way to guide you to altering your post

[t.lewis]

Here is a copy of what works and what does not,
First working post. (edited by me to sent turret to selected home)

G29X5.12Z0.M05 ( first edit point )
T0100
M01
(TOOL - 2 OFFSET - 2)
(OD FINISH RIGHT - TRIANGLE INSERT - TNMG332FF)
G0T0202
G97S500M03
G0G54X.5752Z0.
G50S500
G96S5000
G1X.3752F.0025
Z-.5669
X.4375
G3X.5Z-.5981R.0313
G1Z-1.8154
X.5359
G3X.5984Z-1.8466R.0313
G1Z-3.7391
G2X.8613Z-3.9304R.2049
G3X.8884Z-3.9406R.0313
G1X.9871Z-4.0047
G3X1.Z-4.0237R.0313
G1Z-6.4803
X1.625
X1.7664Z-6.4096
G29X5.12Z0.M05 ( second edit point )
T0200
M30

original post

G28U0.W0.M05 ( section that sends turret to machine home )
T0100
M01
(TOOL - 2 OFFSET - 2)
(OD FINISH RIGHT - TRIANGLE INSERT - TNMG332FF)
G0T0202
G97S500M03
G0G54X.5752Z0.
G50S500
G96S5000
G1X.3752F.0025
Z-.5669
X.4375
G3X.5Z-.5981R.0313
G1Z-1.8154
X.5359
G3X.5984Z-1.8466R.0313
G1Z-3.7391
G2X.8613Z-3.9304R.2049
G3X.8884Z-3.9406R.0313
G1X.9871Z-4.0047
G3X1.Z-4.0237R.0313
G1Z-6.4803
X1.625
X1.7664Z-6.4096
G28U0.W0.M05 ( this section sends to machine home )
T0200
M30

Thanks

[Superman]

Lets see if I can instruct some post reading / writing basics

pbld=block skip, n$=sequence number, e$=end of line
note, the comma is critical.

look in your post for this area
the pheader is obvious
next, "lsof0" =lathe start of file 0, it has a branch to "lsof", followed by "ltlchg".
Can you follow this general structure ?

pheader         #Start of file                         
      "%", e$
      *progno, e$
      pbld, n$, *smetric, e$      
      "(PROGRAM NAME - ", progname, ")", e$
      "(DATE=DD-MM-YY - ", date, " TIME=HH:MM - ", time, ")", e$
        
lsof0           #Start of file for tool zero, lathe                        
      lsof

lsof            #Start of file for non-zero tool number, lathe
      sav_cc_1013 = cc_1013                                   #eap 1/17/03
      ltlchg

ltlchg          #Toolchange, lathe                                        
      toolchng = one 
      gcode = zero
      copy_x = vequ(x)
      pcc_capture   #Capture LCC ends, stop output RLCC
      c_rcc_setup   #Save original in sav_xa and shif

now your changes relate to toolchanging befor and after running an operation with the same tool

find in your program the part that would output the G28
it would look like this

    pbld, n$, *sg28ref, "U0.", "W0.", e$

now insert some sort of indicator and post

    pbld, n$, *sg28ref, "U0.", "W0.", "...#1...", e$

The other is in the retract or endoftool section, use same method to find and then alter to suit

BTW -- these alterations will apply to every operation you post, every tool you use external and internal, I suggest using different codes in your program

ie
G28 U0. Z1. ( home in X and 1" off in Z0 )

it would also act as a check that tool has been set in Z or that the part origin has been set

      pbld, n$, *sg28ref, "U0. Z1.",e$

my suggestion

[t.lewis]

Superman
I have found everything you are talking about and will be able to try my Tuesday. I got a funeral Monday. Shouldn't mastercam do this for me when I pick Home Position - user defined, and select a point were i want the turret to home to before tool change.

[Superman]

You have a "user defined Home Postion"

BUT, if you notice in your post
pbld, n$, *sg28ref, "U0.", "W0.", e$
this ouputs your G28 and whatever string is in quotes "", is what is put into the NC file

if you turn on block skip and post the code, you will get
/ N1 G28 U0. W0.

Did you notice in my 1st post, how I showed how to output an indicator ?
pbld, n$, *sg28ref, "U0.", "W0.", "...#1...", e$ (in the post)
/ N1 G28 U0. W0. ...#1... ( is in your NC code )

[t.lewis]

Sorry for taking so long to get back to you.
I could not reproduce your indicator in my post output so I must be missing something or doing something wrong. Do the U & W represent X & Z incremental from machine home? I will keep working on it till I get it. Thanks

[Superman]

Do a search for sg28ref , as there may be more,
***leave the 2 up in the format statement area untouched***
( also serialise the indicators ie 1,2,3 easier to see which one creates that output )

The # is the start of a comment line, so don't put the "indicator" after one of those.
ie
"--123--", e$ # comment area
-in front of the # will be run through the post and you will get --123--
-behind is only a reference for reading the post by you

more info for you
The G28/G30 output is controlled by Misc. Interger #3, and should be set to zero for G28
The * ( asterisk ) in the post forces the output to the NC code, ( restates that item )

[t.lewis]

I finaly got something to work. Still going to try to keep learning how the post works so i can edit it and now what i'm doing. Thanks for the help.