PP - T67 Haas
General Information
The standard has four configuration pages to manage all options available :
|
1 CNC Controller page
1.1 CNC Controller - % at program begin / end
Option | Result |
No | O1000 … … M30 |
Yes | % O1000 … … M30 % |
1.2 CNC Controller - Program number defined by
Option | Result |
O | % O1000 … … M30 % |
: | % :1000 … … M30 % |
1.3 CNC Controller - Program Name as comment
Option | Result |
No | % O1000 … … M30 % |
Yes | % O1000 (PART NAME) … … M30 % |
1.4 CNC Controller - Use G10 to manage origin
Option | Result |
No | % O1000 … … M30 % |
Yes | % O1000 G10 L2 P1 X.. Y.. Z.. (G54) G10 L2 P2 X.. Y.. Z.. (G55) G10 L20 P1 X.. Y.. Z.. (G110) … … M30 % |
1.5 Cycles – Threading Cycle
Option | Result |
G76 | … G00 X44 G76 X38.506 Z-10. P1 K0.747 A60 D0.2 F1.25 … |
G92 | … G92 X39 Z-43 G00 Z3 G92 X38 Z-43 G00 Z3 … |
2 Turning page
2.1 Turning – Output Stock for CNC Simulation
This option is not use for Haas because there no stock simulation on the CNC
Option | Result |
No |
|
Yes |
|
2.2 Turning – Output Tool and Plane for all operations
Option | Result |
No | O1000 (FACE) T0101 G00 X20 Z2 … … (ROUGH) G00 X20 Z2 … … |
Yes | O1000 (FACE) T0101 G00 X20 Z2 … … (ROUGH) T0101 G00 X20 Z2 … … |
2.3 Turning – Use Parameters for Feed
Option | Result |
No | … T0101 G00 X20 Z2 G01 Z-20 G95 F0.1 … … |
Yes | #1 = 0.1 T0101 G00 X20 Z2 G01 Z-20 G95 F#1 … … |
2.4 Turning – Position Constant Cutting Speed
Option | Result |
Start cycle | T0101 G92 S9000 G96 S40 M04 G00 G90 X24. Z2.8… … |
Start machining | T0101 G97 S530 M04 G00 G90 X24. Z2.8 G92 S9000 G96 S40 M04 G01 G95 Z0. F0.1 … |
2.5 Tool Option – Output Tool List
Option | Result |
No | O1000 T0101 … … |
Yes | O1000 (START TOOL LIST) (T1 CMNG 04) (T2 ...) (T3 ...) (END TOOL LIST) T0101 … … |
2.6 Origin Option – Output Origin List
Option | Result |
No | O1000 T0101 … … |
Yes | O1000 (START ORIGIN LIST) (G54) (...) (END ORIGIN LIST) T0101 … … |
2.7 Origin Option – Multi Origin Management
Option | Result |
Origin Only | % O1000 … G54 … |
Origin + Offset | % O1000 … G54 G52 X10 Y20 Z10 … |
Without MTE :
If the option is set to “Origin Only” for each origin define on the part, we will output a different G code, G54, then G55, G56 … It means you are limited by the number of origin managed by the CNC. If you can have more origin, you must use the second option “Origin + Offset”
If the option is set to “Origin + Offset” it will only output G54 and offset with G52
With MTE :
The origin can be define in the name of the origin with the following syntax “$G54_”. It means G54 will be used in the NC program. If there is no decoded name define, it will output the default origin G54.
If you use “Origin + Offset”, you must use only one origin for all your operation because all the offset are compute from the reference plane origin or single origin.
You can add every text after the underscore to recognized your offset “$G54_Up”, “$G54_Right”, …
2.8 Coolant Option – Coolant Activation Position
The second and third option will give the same output for turning operation.
There will be a difference by milling operations using livetools.
Option | Turning operation | Milling operation (livetool) |
With Spindle | … T0101 S1000 M03 M08 G00 X15 Z2 … | … T0101 S1000 M03 M08 G00 X15 C0 Z2 … |
With Plane Move | … … T0101 S1000 M03 G00 X15 Z2 M08 … | … … T0101 S1000 M03 G00 X15 C0 M8 Z2 … |
With Plunge Move | … T0101 S1000 M03 G00 X15 Z2 M08 … | … T0101 S1000 M03 G00 X15. C0 Z2 M8 … |
3 Code management page
3.1 Code Management – Enable C Axis Code
Option | Result |
“empty” | … T0101 S1000 M3 G17 G28 G90 H0 M154 C10 … |
M51 | … T0101 S1000 M3 G17 M51 G28 G90 H0 C10 … |
3.2 Code Management – Disable C Axis Code
Option | Result |
“empty” | … X200 M155 M09 … |
M50 | … X200 M50 M09 … |
3.3 Code Management – Clamping Code
If the field is empty the code for main spindle will be M14 and for rework spindle M114.
Option | Main Spindle | Rework Spindle |
“empty” | … C10 M14 G01 Z-10 … | … C10 M114 G01 Z-10 … |
M10 | … C10 M10 G01 Z-10 … | … C10 M10 G01 Z-10 … |
3.4 Code Management – Unclamping Code
If the field is empty the code for main spindle will be M15 and for rework spindle M115.
Option | Result | Rework Spindle |
“empty” | … G0 Z20 M15 C10 … | … G0 Z20 M115 C10 … |
M11 | … G0 Z20 M11 C10 … | … G0 Z20 M11 C10 … |
3.5 Code Management – Use axial interpolation mode
If machine don’t have G112 or G12.1 option the output can be done in decomposed.
No circular interpolation will be output don’t use tool offset
Option | Result |
Output axial operation with G112 | |
Output axial operation decomposed |
3.6 Code Management – Enable Axial Interpo Code
If the field is empty, the code used by default will be G112.
Option | Result |
“empty” | … G01 Z-5 G112 … |
G12.1 | … G01 Z-5 G12.1 … |
3.7 Code Management – Disable Axial Interpo Code
If the field is empty, the code used by default will be G113.
Option | Result |
“empty” | … G113 G00 Z20 … |
G13.1 | … G13.1 G00 Z20 … |
5.8 Code Management – Use radial interpolation mode
If machine don’t have G107 option the output can be done in decomposed.
No circular interpolation will be output don’t use tool offset
Option | Result |
Output axial operation with G107 | |
Output axial operation decomposed |
3.9 Code Management – Enable Radial Interpo Code
There is not radial interpolation of Haas CNC.
Option | Result |
“empty” |
|
G107 |
|
3.10 Code Management – Disable Radial Interpo Code
Option | Result |
“empty” |
|
G107 |
|
3.11 Primary axis option – Management of primary axis
Option | Result |
Modulo | … C0 … C359 C0 … |
Linear | … C0 … C359 C360 … |
Incremental | … C0 … H1 H1 … |
4 File management page
There is not multi-channel Haas CNC. Those option will output the same as Fanuc controller and will be update when Haas CNC will be able to have multi channel.
4.1 File Management – One physical File per Channel
Option | File 1 | File 2 |
O1000 (FIRST CHANNEL PROGRAM) … … M30
O1001 (SECOND CHANNEL PROGRAMM) … … M30 |
| |
O1000 (FIRST CHANNEL PROGRAM) … … M30 | O1001 (SECOND CHANNEL PROGRAMM) … … M30 |
4.2 File Management – Generate the channel even if empty
Option | Result |
If a channel is empty no output of the program | |
If a channel is empty, the program will be output (but empty (Just O1001 and M30 will be output) |
4.2.1 Listing / Synchronized File – Generate the Listing File
You need to set the Synchro Number mini & maxi to output the listing
Option | Result |
Don’t generate the file to see the synchro between channels. | |
Generate the file to see the synchro between channels. |
The file with the name Listing.TXT will be temporarily generated and shown.
![]() |
4.3 Listing / Synchronized File – Synchro Numbers (Mini / Maxi)
Define here the synchronization Numbers (for example 500 – 540)
The post processor will search for the synchronizations numbers between these mini and maxi values to generate the Listing.TXT file.
5 Launch page
![]() |
5.1 Name of the NC File :Define here the Name of the generated NC file.
The extension is to be defined in the MCF configuration.
5.2 Program Number : If 0 is defined, the program Number will be set to 1.
Option | Result |
0 | % O0001 … … |
“10” | % O0010 … … |
“1234” | % O1234 … … |
5.3 Comment Output :
Option | Result |
No | … T0101 … |
Yes | … (FACING) (CNMG 04) T0101 … |
5.4 Block Numbers :
Option | Result |
With | O1000 N5 T0101 N10 G00 X10 Z20 N15 Z10 … … N50 T0202 N55 G00 X20 Z20 N60 Z10 … … |
Without | O1000 T0101 G00 X10 Z20 Z10 … … T0202 G00 X20 Z20 Z10 … … |
Tool Change Only | O1000 N5 T0101 G0 X10 Z20 Z10 … … N10 T0202 G0 X20 Z20 Z10 … … |
5.5 Code for Program End :
Option | Result |
M30 | … … … M30 % |
M02 | … … … M02 % |
M99 | … … … M99 % |