Sign in to follow this  
offrey414

lathe post x5 m6 on tool line

Recommended Posts

I am wondering if any one has ever ran into this. I can not for the life of me get my lathe post to call out an M6 on the tool line. I have tried clicking "Force tool change" in parameters and I can not find any thing in post file or machine definition file that would allow me to add M6 anywhere? I have been pulling my hair out for a while and I do not want to keep adding M6 in a text editor every time I want to run this machine. Any help would be greatly appreciated. 

 

******What I am getting*****

1
[PROGRAM NAME - 101 POST TEST JDV
[DATE=DD-MM-YY - 23-01-20 TIME=HH:MM - 06:19
[MCX FILE - C:\USERS\OFFRE\DESKTOP\RED FOX PROGRAMING\CNC TEST.MCX-5
[NC FILE - C:\USERS\OFFRE\DESKTOP\RED FOX PROGRAMING\101 POST TEST JDV.NC
[MATERIAL - STEEL INCH - 1030 - 200 BHN
N100 G20 G90
[TOOL - 3 OFFSET - 3
[OD ROUGH RIGHT - 80 DEG.  INSERT - CNMG-432
N110 G0 X3. Z10.
N120 G0 T0303

]

 

***need it to post ******

1
[PROGRAM NAME - 101 POST TEST JDV
[DATE=DD-MM-YY - 23-01-20 TIME=HH:MM - 06:19
[MCX FILE - C:\USERS\OFFRE\DESKTOP\RED FOX PROGRAMING\CNC TEST.MCX-5
[NC FILE - C:\USERS\OFFRE\DESKTOP\RED FOX PROGRAMING\101 POST TEST JDV.NC
[MATERIAL - STEEL INCH - 1030 - 200 BHN
N100 G20 G90
[TOOL - 3 OFFSET - 3
[OD ROUGH RIGHT - 80 DEG.  INSERT - CNMG-432
N110 G0 X3. Z10.
N120 G0 T0303 M6

]

SOUTH BEND POST.pst

south bend post.LMD-5

Share this post


Link to post
Share on other sites
if home_type = m_one, pbld, n$, *sgcode, *toolno, e$ #line 1490 of your post


if home_type = m_one, pbld, n$, *sgcode, *toolno, "M6", e$ #add the "M6"

Will only be helpful if you always need an M6.

Share this post


Link to post
Share on other sites
4 hours ago, offrey414 said:

I am wondering if any one has ever ran into this. I can not for the life of me get my lathe post to call out an M6 on the tool line. I have tried clicking "Force tool change" in parameters and I can not find any thing in post file or machine definition file that would allow me to add M6 anywhere? I have been pulling my hair out for a while and I do not want to keep adding M6 in a text editor every time I want to run this machine. Any help would be greatly appreciated. 

 

******What I am getting*****

1
[PROGRAM NAME - 101 POST TEST JDV
[DATE=DD-MM-YY - 23-01-20 TIME=HH:MM - 06:19
[MCX FILE - C:\USERS\OFFRE\DESKTOP\RED FOX PROGRAMING\CNC TEST.MCX-5
[NC FILE - C:\USERS\OFFRE\DESKTOP\RED FOX PROGRAMING\101 POST TEST JDV.NC
[MATERIAL - STEEL INCH - 1030 - 200 BHN
N100 G20 G90
[TOOL - 3 OFFSET - 3
[OD ROUGH RIGHT - 80 DEG.  INSERT - CNMG-432
N110 G0 X3. Z10.
N120 G0 T0303

]

 

***need it to post ******

1
[PROGRAM NAME - 101 POST TEST JDV
[DATE=DD-MM-YY - 23-01-20 TIME=HH:MM - 06:19
[MCX FILE - C:\USERS\OFFRE\DESKTOP\RED FOX PROGRAMING\CNC TEST.MCX-5
[NC FILE - C:\USERS\OFFRE\DESKTOP\RED FOX PROGRAMING\101 POST TEST JDV.NC
[MATERIAL - STEEL INCH - 1030 - 200 BHN
N100 G20 G90
[TOOL - 3 OFFSET - 3
[OD ROUGH RIGHT - 80 DEG.  INSERT - CNMG-432
N110 G0 X3. Z10.
N120 G0 T0303 M6

]

SOUTH BEND POST.pst

south bend post.LMD-5

Seeing how almost every lathe on the planet doesn't need M06 unless they have B head I am not sure why that machine does.

Share this post


Link to post
Share on other sites

Kalibe -  For some reason that tool out the tool change line all together when I put it in at the lathe tool change section.  

 

5th Axis CGL -  I know I never ran into a lathe that needs an M6 called out to rotate the turret. If its the active turret position its all good but if it is not it wants an M6. The Weird thing if you run it in MDI you do not need the M6. This is definitely a weird machine to me.  

Share this post


Link to post
Share on other sites

Did you just add the "M6", or the entire line below what was there? Just adding the "M6" had it posting the way you wanted, not sure why the whole line would go missing... 

Share this post


Link to post
Share on other sites

Post it using the de-bugger and see where it's processing the output. Probably line 1498 in the lathe part and 1560 for the milling tools.

Share this post


Link to post
Share on other sites

You probably use as Work coordinate system the option Home position (mi1 = 1) 

Try changing the post to the following:

      if home_type < two, #Toolchange G50/home/reference position
        [
        sav_xh = vequ(copy_x)
        sav_absinc = absinc$
        absinc$ = zero
        pmap_home   #Get home position, xabs
        ps_inc_calc #Set start position, not incremental
        #Toolchange home position
        if home_type = one,
          pbld, n$, *sgcode, pfxout, pfyout, pfzout, e$
        else,
          [
          #Toolchange g50 position
          pbld, n$, *sg28ref, "U0.", [if y_axis_mch, "V0."], "W0.", e$
          toolno = t$ * 100 + zero
          if home_type = m_one, pbld, n$, *sgcode, *toolno, e$
          else, pbld, n$, *sg50, pfxout, pfyout, pfzout, e$
          ]
        pe_inc_calc #Update previous
        absinc$ = sav_absinc
        copy_x = vequ(sav_xh)
        ]
      toolno = t$ * 100 + tloffno$
      pbld, n$, *sgcode, *toolno, "M6", e$
      pbld, n$, pfsgplane, e$

 

  • Thanks 1

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now
Sign in to follow this  

  • Recently Browsing   0 members

    No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us