Configure Mill menu

Use the options on the Configure Mill menu to configure milling process output.

NC File Header/Footer Formats

Use the options on the Configure Mill > NC File Header/Footer Formats menu to configure the NC File Header/Footer formats for milling process output. File headers and footers begin and end the NC code.

The following options are available:

• File Start
• Program End
• File End
• Developer Notes

File Start

This program format is the first format called in ConfigPost. It is only called once and is used to output %, program numbers, and so on. It can also be used to initialize variables that are to be used in other formats.

File Start is where you create and manage multiple files so that you can correctly output NC code for multi-channel machines.

Program End

This program format is output at the end of a part program before sub-programs if the End of File option is used. You can use this program format to position the tool to an end point (using the <tool-change-x> and <tool-change-y> reserved words), turn coolant off, or restart the part program.

For incremental programming, you can use <@tool-change-x> and <@tool-change-y> to move to the first tool change position in the part program.

{N<seq> }M09<eob>
{N<seq> }G91G30Z<z-coord><eob>
{N<seq> }G30X<tool-change-x>Y<tool-change-y>M05<eob>
{N<seq> }M06M30<eob>
{N<seq> }G90M30<eob>
%<eob>

File End

This program format specifies the format of one or more lines to be placed at the end of the part program file and is normally used after the sub-programs section of a part program. %<eob>

Developer Notes

This program format usually contains the post processor specific information. It is used by developer of the post processor for notes and comments. Machine specific M/G codes can be entered in this format. In addition, a history of changes can be inserted in this format.

Process Header/Footer Formats

Use the options on the Configure Mill > Process Header/Footer Formats to configure Process Header/Footer formats for milling process output. Process headers open and close individual processes or operations.

The following options are available:

• Program Start
• Tool Change
• Process Start
• Process End

Program Start

PartMaker outputs Program Start at the beginning of a part program. You must place general preparatory codes such as absolute, incremental, and so on, in this program format to define the dimension system. You must also define the first tool change in this program format. Reserved Words such as, <speed>, <spindle-on> and <coolant> as well as <x-coord> and <y- coord> specifying the first positioning move are commonly included in the Program Start format.

%<eob>
:<prog-num1> <eob>
(TOTAL MACHINING TIME: <time-total>) <eob>
{N<seq> }G80 G40 G17 <eob>
{N<seq> }G30 G91 Z0 <eob>
{N<seq> }T<tool-num> M6 <eob>
(<tool-name>) <eob>
(TIME FOR THIS TOOL: <time-process>) <eob>
{N<seq> }G90 <work-offset> <motion> X<x-coord> Y<y-coord> S<speed-rpm> <spindle-on> <eob>
{N<seq> }G43 Z<z-coord> H<tool-offset> <coolant> <eob>

Tool Change

When you use the Tool Change format, a tool change block is output in the part program for all processes that require a tool change. Reserved Words such as <speed>, <spindle-on>, and <coolant> as well as <x-coord> and <y-coord> specifying the first positioning point are usually included in Tool Change format.

{N<seq> }M9<eob>
{N<seq> }G91 G30 Z0 M5<eob>
{N<seq> }T<tool-num> M6<eob>
(<tool-name>)<eob>
(TIME FOR THIS TOOL: <time-process>)<eob>
{N<seq> }M1<eob>
{N<seq> }G90 <work-offset> <motion> X<x-coord> Y<y-coord> S<speed-rpm> <spindle-on><eob>
{N<seq> }G43 Z<z-coord> H<tool-offset> <coolant><eob>

Process Start

A process start block is output only between non-tool changing processes in the part program. The Process Start program format must contain all commands that might change between processes such as <speed>. You must also include the <x-coord>, <y-coord>, and <z-coord> reserved words in this program format.

{N<seq> }Z<z-coord><eob>
{N<seq> }{<work-offset> }{<motion> }X<x-coord> Y<y-coord> {S<speed-rpm> }{<spindle-on>}<eob>

Process End

It is not recommended to use Process End format for Basic Post Processors. For multi-axis post processors, the Process End format is commonly used to cancel synchronization modes and retract the tool to a safe location before the tool change.

Motion Formats

Use the options on the Configure Mill > Motion Formats menu to configure Motion formats for milling process output.

Horizontal Rapid Move

• Scenario A: If your CNC allows X, Y, and Z axis motion programmed in the same line, you must place all three reserved words in the Horizontal Rapid Move format, leaving the Vertical Rapid Move format empty.
• Scenario B: If your CNC does not allow X, Y, and Z axis motion programmed in the same line, you must use both the Horizontal Rapid Move format and the Vertical Rapid Move format.

The Horizontal Rapid Move program format determines the output of rapid positioning moves in the part program. When you use modality delimiters { } around the <x-coord> and <y-coord> reserved words in this program format, PartMaker will strip redundant X or Y coordinates from each line as they are encountered.

If Scenario A above is true, you must leave the Vertical Rapid Move format empty.

{N<seq> }{<motion> }{X<x-coord> }{Y<y-coord> } {Z<z-coord>}<eob>

Vertical Rapid Move

• Scenario A: If your CNC allows X, Y, and Z axis motion programmed in the same line, you must place all three reserved words in the Horizontal Rapid Move format, leaving the Vertical Rapid Move format empty.
• Scenario B: If your CNC does not allow X, Y, and Z axis motion programmed in the same line, you must use both the Horizontal Rapid Move format and the Vertical Rapid Move format.

If Scenario A is true, you must leave the Vertical Rapid Move format empty. If Scenario B is true, you must include the <z-coord> reserved word in this program format.

{N<seq> }{<motion> }{Z<z-coord> }<eob>

Linear Move

The Linear Move program format defines the part program output for linear moves. You must define the <x-coord>, <y-coord>, <z-coord>, <motion>, and <feed-upm> reserved words in this program format. You can use the <comp-start> reserved word to turn cutter compensation on or off.

{N<seq> }{<motion> }{<comp-status> }{X<x-coord> }{Y<y-coord> }{Z<z-coord> }
<IF><comp-start><THEN>
D<comp-num>
<ENDIF>
{F<feed-upm>}
<eob>

Circular Move

In this program format, the reserved words <arc-x>, <arc-y>, <radius>, <center-x>, and <center-y> can be used.

{N<seq> }{<motion> }{X<x-coord> }{Y<y-coord> }I<arc-x> J<arc-y> {F<feed-upm>}<eob>

Helical Move

In this program format, the reserved words <arc-x>, <arc-y>, <radius>, <center-x>, and <center-y> can be used. This program format should only be used if the machine is capable of helical interpolation (very few are):

{N<seq> }{<motion> }{X<x-coord> }{Y<y-coord> }{Z<z-coord> }I<arc-x> J<arc-y> {F<feed-upm>}<eob>

Move to Hole Location

This program format defines the output for a specific hole location.

{N<seq> }{X<x-coord> }{Y<y-coord> }{Z<depth-abs>}<eob>

Subprograms Related Formats

Use the options in the Configure Mill > Subprograms Related Formats menu to configure Subprograms-Related formats for milling process output.

Linear Move in Subprogram

This program format is similar to the Linear Move (Motion) program format, but is used within a subprogram definition only without the <z-coord> reserved word.

{N<seq> }{<motion> }{<comp-status> }{X<@x-coord> }{Y<@y-coord> }
<IF><comp-start><THEN>
D<comp-num>
<ENDIF>
{F<feed-upm>}<eob>

Circular Move in Subprogram

This program format is similar to the Circular Move (Motion) program format, but is used within a subprogram definition only.

{N<seq> }{<motion> }X<@x-coord> Y<@y-coord> I<arc-x> J<arc-y>{ F<feed-upm>}<eob>

Helical Move in Subprogram

This Subprogram command is not used.

Move to Hole Location

This program format is similar to the Move to Hole Location (Motion) program format, but is used within a subprogram definition only. {N<seq> }{X<x-coord> }{Y<y-coord>}<eob>

Open Subprogram

This program format specifies the format of the lines that precede a subprogram definition. You must use the <subprogram-num> reserved word and a preparatory function to define the incremental mode if you are using incremental subprograms.

:<subprogram-num><eob>
<IFNOT><drilling><THEN>
{N<seq> }G91<eob>
<ENDIF>

Close Subprogram

This program format specifies the format of the lines that follow a subprogram definition. You might want to use a preparatory function to redefine the absolute mode if the main part program starts in the absolute mode.

<IFNOT><drilling><THEN>
{N<seq>}G90<eob>
<ENDIF>
{N<seq>}M99<eob>

Call Subprogram

This program format specifies the format of a line that calls a subprogram. You must identify the subprogram using the <subprogram-num> reserved word.

<IF><drilling><THEN>
{Z<depth-abs>}<eob>
<ENDIF>
M98 P<subprogram-num><eob>

Canned Cycle Formats

Use the options on the Configure Mill > Canned Cycle Formats menu to configure Canned Cycle formats for milling process output.

DRILL Cycle

This program format specifies a canned drilling cycle.

{N<seq> }{<retract> }<cycle> {X<x-coord> }{Y<y-coord> }R<clear-abs> Z<depth-abs> F<feed-upm><eob>

SPOT FACE Cycle

This program format specifies a canned spot face cycle.

{N<seq> }{<retract> }<cycle> {X<x-coord> }{Y<y-coord> }R<clear-abs> Z<depth-abs> P<dwell> F<feed-upm><eob>

DEEP HOLE Cycle

This program format specifies a canned deep hole cycle.

{N<seq> }{<retract> }<cycle> {X<x-coord> }{Y<y-coord> }R<clear-abs> Z<depth-abs> Q<step>F<feed-upm><eob>

CHIP BREAK Cycle

This program format specifies a canned chip break cycle:

{N<seq> }<cycle> {X<x-coord> }{Y<y-coord> }R<clear-abs> Z<depth-abs>Q<step>F<feed-upm><eob>

VARIABLE STEP Cycle

This program format specifies a canned variable step cycle:

<IFNOT><is-full-retract><THEN>
G73 I<step> J<step-decrease> K< step-min> Z<depth-abs> F<feed-upm><eob>
<ENDIF>
<IF><is-full-retract><THEN>
G83 I<step> J< step-decrease> K< step-min> Z<depth-abs> F<feed-upm><eob>
<ENDIF>

FLOAT TAP Cycle

This program format specifies a canned float tapping cycle.

{N<seq> }{<retract> }<cycle> {X<x-coord> }{Y<y-coord> }R<clear-abs> Z<depth-abs> F<feed-upm> <eob>

RIGID TAP Cycle

This program format specifies a canned rigid tap cycle.

{N<seq> }{<retract> }<cycle> {X<x-coord> }{Y<y-coord> }R<clear-abs> Z<depth-abs>
F<feed-upm> <eob>

BORE, DWELL Cycle

This program format specifies a canned boring cycle with a dwell.

{N<seq> }{<retract> }<cycle> {X<x-coord> }{Y<y-coord> }R<clear-abs> Z<depth-abs>
P<dwell> F<feed-upm><eob>

BORE Cycle

This program format specifies a canned boring cycle.

{N<seq> }{<retract> }<cycle> {X<x-coord> }{Y<y-coord> }R<clear-abs> Z<depth-abs>
F<feed-upm><eob>

CIRCLE MILL Cycle

This program format specifies a canned circle milling cycle for machines that support such cycles (very few do).

THREAD MILL Cycle

This program format specifies a thread milling cycle for machines that support such cycles.

HELICAL MILL Cycle

This program format specifies a canned helical mill cycle for machines that support such cycles. Helical mill cycles are typically not defined for lathes or mills, however this option is available for your use if provided by your control manufacturer.

Canned Cycle

G80<eob>

Procedure Formats

For more information, see Procedures.

Modes, Moving Stock

For more information, see Synchronization Modes.

Modes, Stationary Stock

For more information, see Synchronization Modes.

General Information

Use this menu option to display the General Information dialog where you can specify information for a part program such as machining data, subprograms support for milling and drilling operations (if your CNC is capable), and the type of circular interpolation your CNC uses.

Preparatory Functions

Use this menu option to display the Preparatory Functions dialog, where you can specify machining codes to be used in the part program for cycle names, motion formats, cutter compensation, coolant type, and spindle direction.

Words Information

Use this menu option to display the Words Information dialog where you can specify parameters for reserved words used in a Post file.