Post Help with Machine Setup-2

Where in the post processor file does the M00 between Machine setup -1 and Machine Setup – 2 originate?

I turned on Debugging and I could see no difference between a different Job and a 2nd Setup but in the NC file, a M00 is inserted. I would like to add more code with the M00.

Program snippet Next Job:
N72 G01 X3.0778 Z-.25 F76.8
************* 50 – Rapid moves//Rapid move Z **********
N73 G00 Z.1
************* 71 = Operations//End of operation **********
************* 4 – Tool Change//Move to next cut same tool **********
N74 ;JOB 3 PROFILE
N75 ;23MM HOLE
N76 X3.0778 Y-2.975
************* 40 – Operations//Start of operation **********
************* 51 – Feed moves//Feed move Z **********

Program snippet Next Machine Setup:
N83 G01 X3.0778 F76.8
************* 50 – Rapid moves//Rapid move Z **********
N84 G00 Z.1
************* 71 = Operations//End of operation **********
N85 M00
************* 4 – Tool Change//Move to next cut same tool **********
N86 ;JOB 4 PROFILE
N87 ;OUTSIDE PROFILE
N88 X6.215 Y.2906
************* 40 – Operations//Start of operation **********
************* 51 – Feed moves//Feed move Z **********

How does the post know to add the M00 on line N85?

Thanks for your help.

Quote:

---

Originally Posted by vfsi

************* 71 = Operations//End of operation **********
N85 M00
.

---

If you open your post in a text editor you should be able to look at section 71. and see how the M00 code is generated. If you cannot find it maybe attach your post file so others can look at it.

Quote:

---

Originally Posted by jmullett

If you open your post in a text editor you should be able to look at section 71. and see how the M00 code is generated. If you cannot find it maybe attach your post file so others can look at it.

---

Here is my post at Section 71, not much to see.

64. Arc move XY.
n,g_arc_plane,g_arc_move,x_f,y_f,arc_center,feed_r ate

65. Arc move YZ.
n,g_arc_plane,g_arc_move,y_f,z_f,arc_center,feed_r ate

66. Arc move XZ.
n,g_arc_plane,g_arc_move,x_f,z_f,arc_center,feed_r ate

71. End of 2axis cutting.

73. High speed peck drill canned cycle.
n,canned_feed_rate

Quote:

---

Originally Posted by vfsi

Where in the post processor file does the M00 between Machine setup -1 and Machine Setup – 2 originate?

I turned on Debugging and I could see no difference between a different Job and a 2nd Setup but in the NC file, a M00 is inserted. I would like to add more code with the M00.

Program snippet Next Job:
N72 G01 X3.0778 Z-.25 F76.8
************* 50 – Rapid moves//Rapid move Z **********
N73 G00 Z.1
************* 71 = Operations//End of operation **********
************* 4 – Tool Change//Move to next cut same tool **********
N74 ;JOB 3 PROFILE
N75 ;23MM HOLE
N76 X3.0778 Y-2.975
************* 40 – Operations//Start of operation **********
************* 51 – Feed moves//Feed move Z **********

Program snippet Next Machine Setup:
N83 G01 X3.0778 F76.8
************* 50 – Rapid moves//Rapid move Z **********
N84 G00 Z.1
************* 71 = Operations//End of operation **********
N85 M00
************* 4 – Tool Change//Move to next cut same tool **********
N86 ;JOB 4 PROFILE
N87 ;OUTSIDE PROFILE
N88 X6.215 Y.2906
************* 40 – Operations//Start of operation **********
************* 51 – Feed moves//Feed move Z **********

How does the post know to add the M00 on line N85?

Thanks for your help.

---

You may be missing this block in your post processor:

16. Machine Setup Change
" "
"(NEXT SETUP)"

If block 16 is empty or missing you get an M00. Add any kind of instruction in there and it will replace the M00 with whatever you put there. Have fun with it!

EDIT: I added the line feed " " and the (NEXT SETUP) in there to get rid of the M00. I can't remember what is there by default but you can look at BC_3x_Mill.Millpst for reference.

Quote:

---

Originally Posted by SBC Cycle

You may be missing this block in your post processor:

16. Machine Setup Change
" "
"(NEXT SETUP)"

If block 16 is empty or missing you get an M00. Add any kind of instruction in there and it will replace the M00 with whatever you put there. Have fun with it!

EDIT: I added the line feed " " and the (NEXT SETUP) in there to get rid of the M00. I can't remember what is there by default but you can look at BC_3x_Mill.Millpst for reference.

---

Thanks for the great help...

Earlier I had searched for the word "Setup" and my editor returned a blank. So I thought something was missing. I will reference BC_3x for insight. I started with the Siemens post supplied from bobcad which is almost functional but unusable without a lot of editing. Now I am trying to refine it for our use. Every week a set closer.

No problem! My post took a while to get it just right but man is it just right. Good luck and post back with any problems.

My lathe post (Siemens 840C) does not have a block 16. However in my Mill (Fanuc OMC) post I edited block 16 to read:

16. Machine Setup Change
n,"M9"
n,"G0Y4.0Z5.0"
n,"M5"
n,"( TURN PART )"
n,"M00"
"(TOOL#",list_tool_number," ",tool_label,")"
n_forced,t,"M6"
n,"M01"
n,rapid_move,absolute_coord,work_coord,force_x,xr, force_y,yr,rotar y_xy_angle
n,rapid_move,length_offset,spindle_on,s
n, force_no_add_spaces," /"coolant_on
default_add_spaces

This is a rather late reply but it might help someone out.

I think this should be referred to as section 16. Blocks are all in the 2000 series for doing calculations.

I learned from BOBcad that you cannot do a setup change in LATHE. They never allowed it in the code. Told me I need to make a new part in a new drawing and start part two there.