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

Program number defined by

Program Name as comment

Use G10 to manage origins

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.

Milling page

Milling Section

Output Stock for CNC Simulation

There is no output for Haas machine.

Output Tool and Plane for all operations

Use Parameters for Feed

Tool Option Section

Output Tool List

 Tool Change

 Preselect First Tool after Last Tool

Tool Change in

Origin Option Section

Output Origin List

Origin position

Multi Origin Management

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

Milling 5X page

Milling 5X Parameters

Use Tilted work Plane for 3+2 Axis

Rotation Axis

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.

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.

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.

Comment Output

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.

Comment Output

Block Numbers

Code for Program End