PP - M67 Haas
The standard has three configuration pages to manage all options available: The first page “CNC Controller” is about CNC options. The second page “Milling” allows to adapt the output for Milling, tools, coolant and origins. The third page “Milling” is about 5 axis parameters. |  |
CNC Controller page
CNC Controller Section
 |
% at program begin/end
Option | Result |
No | O1000 … M30 |
Yes | % O1000 … M30 % |
Program number defined by
Option | Result |
O | % O1000 … M30 % |
: | % :1000 … M30 % |
Program Name as comment
Option | Result |
No | % O1000 … M30 % |
Yes | % O1000 (PART NAME) … M30 % |
Use G10 to manage origins
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.. (G54.1) … M30 % |
Options Section
Spindle reverse parameter for drilling available (E)
Added as from V6.08.
Define if the machine can use the E parameter for drilling cycle. This parameter will invert the spindle direction to retract from the bottom of hole. The value is the spindle speed. The post processor will use the same speed to drill.
This parameter can be used only for G81, G82 and G83.
If the E parameter can’t be use, the output will be decomposed.
Option | Result |
No | S1000 M03 G0 X10 Y10 G0 Z2 G1 Z-10 F500 M04 Z2 |
Yes | S1000 M03 G00 X10 Y10 G00 Z2 G81 X10 Y10 Z-10 E1000 F500 G80 |
Milling page
Milling Section
 |
Output Stock for CNC Simulation
There is no output for Haas machine.
Option | Result |
No | % O1000 … |
Yes | % O1000 … |
Output Tool and Plane for all operations
Option | Result |
No | (OP 1 WITH TOOL 1 AND PLANE 1) T1 M6 G52 X0 Y0 Z0 B90 C0 G254 … (OP 2 WITH TOOL 1 AND PLANE 1) … |
Yes | (OP 1 WITH TOOL 1 AND PLANE 1) T01 M06 G52 X0 Y0 Z0 B90 C0 G254 … (OP 2 WITH TOOL 1 AND PLANE 1) T01 M06 G52 X0 Y0 Z0 B90 C0 G254 … |
Use Parameters for Feed
Option | Result |
No | T01 M06 G00 X.. Y.. G43 H1 Z.. Z-.. F160 G01 X.. Y.. F200 … |
Yes | #1 = 200 #2 = 160 T01 M06 G00 X.. Y.. G43 H1 Z.. Z-.. F#2 G01 X.. Y.. F#1 … |
Tool Option Section
 |
Output Tool List
Option | Result |
No | % O1000 … |
Yes | % O1000 (START TOOL LIST) (T01 END MILL D10) (T02 DRILL D08) … (END TOOL LIST) … |
Tool Change
Option | Result |
Manual | … M00 … |
Automatic | … T01 M06 … |
Auto + Preselect | … T01 M06 T02 … |
Preselect First Tool after Last Tool
Option | Result |
No | (FIRST OPERATION) T01 M06 T02 … (LAST OPERATION) T05 M06 … M30 |
Yes | (FIRST OPERATION) T01 M06 T02 … (LAST OPERATION) T05 M06 T01 … M30 |
Tool Change in
Option | Result |
1 Block | … T01 M06 … |
2 Blocks | … T05 M06 … |
Origin Option Section
 |
Output Origin List
Option | Result |
No | % O1000 … |
Yes | % O1000 (START ORIGIN LIST) (G54) (G55) (END ORIGIN LIST) … |
Origin position
Option | Result |
After axes Rotation | B0.C0. … G54 G52 X0. Y0. Z0 |
Before Axes rotation | G54 G52 X0.Y0.Z0 …. B0.C0.E |
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 defined in the name of the origin with the following syntax “$G54_”. It means G54 will be used in the NC program. If there is no decoded name defined, it will output the default origin G54.
If you use “Origin + Offset”, you must use only one origin for all your operation because all the offset are computed from the reference plane origin or single origin.
You can add any text after the underscore to recognized your offset “$G54_Up”, “$G54_Right”, …
Coolant Option Section
 |
Coolant Activation Position
Option | Result |
With Spindle | … T01 M06 S8000 M03 M08 G00 X.. Y.. G43 H1 Z… … |
With Plane Move | … T01 M06 S8000 M3 G00 X.. Y.. M08 G43 H1 Z.. … |
With Plunge Move | … T01 M06 S8000 M03 G00 X.. Y.. G43 H1 Z.. M08 … |
Milling 5X page
Milling 5X Parameters
 |
Use Tilted work Plane for 3+2 Axis
Option | Result |
No | … T01 M06 C180 B-90 … |
Yes | … … T01 M06 C180 B-90 G254 … … |
Rotation Axis
Option | Result | Option | Result |
Lock 1st Rotation Axis | Lock 2nd Rotation Axis | ||
empty | … C180 … | empty | … B-90 … |
“M10” | … C180 M10 … | “M12” | … B-90 M12 … |
Unlock 1st Rotation Axis | Unlock 2nd Rotation Axis | ||
empty | … C180 … | empty | … B-90 … |
“M11” | … M11 C180 … | “M13” | … M13 B-90 … |
Fixed blocks for plane change (Used without MTE)
 |
Active fixed blocks for plane change
This option is used only if there is no kinemac defined in the machine configuration.
Option | Result |
check | The fixed blocks defined will be output if there is a plane change |
uncheck | The standard blocks will be output if there is a plane change. G0 G91 G28 Z0 |
First and Second Block
To avoid the standard output, check the option to activate the fixed blocks and keep the first and second block fields empty.
Option | Result |
Empty | … … |
“G00 Z100” | … G00 Z100 … |
Launch page
With machine kinematic defined | Without machine kinematic defined |
 |  |
Name of the NC File
Define here the Name of the generated NC file. The extension must to be defined in the MCF configuration.
Program Number
If 0 is defined, the program Name will be set to 1.
Option | Result |
0 | % O1 … |
“10” | % O10 … |
“1234” | % O1234 … |
Comment Output
Option | Result |
No | … T01 M06 … |
Yes | … (FACING) (END MILL D12) T01 M06 … |
Origin Number
This parameter is used only if kinematic is not defined in the machine file. The parameter defines the first origin used in the NC program.
If the parameter to treat multi origin is set on “Origin Only” the origin number is incremented when a plane changes.
Option | Result Until 8055 |
54 | % O10 T01 M06 G54 … |
55 | % O10 T01 M06 G55 … |
Comment Output
Option | Result |
No | … T01 M06 … |
Yes | … (FACING) (END MILL D12) T01 M06 … |
Block Numbers
Option | Result |
With | O1000 N5 T01 M06 N10 G00 X.. Y.. N15 G43 Z.. H1 … N50 T02 M06 N55 G00 X.. Y.. N60 G43 Z.. H2 … |
Without | O1000 T01 M06 G00 X.. Y.. G43 Z.. H1 … T02 M06 G00 X.. Y.. G43 Z.. H2 … |
Tool Change Only | O1000 N5 T01 M06 G00 X.. Y.. G43 Z.. H1 … N10 T02 M06 G00 X.. Y.. G43 Z.. H2 … |
Code for Program End
Option | Result |
M30 | … … … M30 % |
M02 | … … … M02 % |
M99 | … … … M99 % |