NC Parameters

The NC Parameters softkey accesses these functions:

NC Configuration Parameters

NC M and G Code Parameters 

NC Variables

NC Configuration Parameters

Use this screen to change general NC part program parameters and set ASR Buffering.

Refer to the Field Glossary for definitions of the NC Configuration Parameters:

General 1

General 2

Intelligent ASR

When enabled, Intelligent ASR buffering begins automatically when certain conditions are met in the program.

M16 (Automatic Buffering On) and M17 (Automatic Buffering Off) are used to turn automatic buffering on and off within a program. The parameter must be turned on in order to use M16/17.

NC M and G Code Parameters

Use this screen to change M code and G code program numbers for an NC part program using NCPP:

• Enable User M/G Codes—enables user customization of M codes and/or G codes to perform specialized tasks. User defined M and G codes define a custom code which performs a specialized task, replace an existing G or M code, or provide compatibility between different NC dialects from various machine tool control manufacturers. 

• Enable User S/B/T Codes—enables user customization of S codes, B codes, or T codes to perform specialized tasks. User defined S, B, or T codes replace spindle and tool functions with custom subprograms.

• M-Code—allows programming of customized M codes. Up to 13 user defined M codes can be programmed from M01 through M255 (except M02, M98, and M99). Negative numbers cannot be entered in the column for user defined M codes. Enable programmed M codes using the Enable User M Codes function.

• G-Code—allows programming of customized G codes. Up to 10 user defined G codes can be programmed from G01 through G100 (except G65, G66, and G67). If a negative number is entered for a user defined G code, the subprogram becomes modal. Enable programmed G codes using the Enable User G-Codes function.

NC Variables

Use this screen to define Global and System NC variable codes and subprograms for an NC part program using NCPP. Programs with variables can be reused. All variables must begin with the "#" character followed by a valid, writeable register number and an equal sign. The following example sets the variable value (#500) to 100:

# 500 = 100

Some variables are read only when an operator attempts to write to the variable.

There are three types of variables that can be used in NC programming:

1. Global—can be used by all programs. Assign a global variable before it is used in an equation or expression, or the variable will be considered vacant, generating an error unless the Allow Vacant Variables field is set to Yes. Use the Global 100-199 and Global 500 - 999 softkeys to enter global variables on the NC Variables screen.

2. System—provide information about the state of the system such as X, Y, and Z external work compensation, miscellaneous system parameters, modal information, position information, and G code group status. Use the Tool Offset 2001-2200, Work Offset 2500-2999, Misc 3000-3014, Modal 4001-4320, and Position 5001-5083 softkeys to enter system variables on the NC Variables screen.

3. Local—are valid only within the current program. These variables are only available in Macro Mode B and range from #1 to #33. Enter local variables in the NC Editor screen. Refer to NC Editor.

   1. Assign a value to the local variable before it is used in an equation or expression, or the variable will be considered vacant, generating an error unless the Allow Vacant Variables field is set to Yes.

   2. When the subprogram call is not made using an M98, local variables are nested, meaning that when a subprogram call is made, a new set of local variables is received and the old set is stored. After leaving the subprogram, these local variables are destroyed and the previous set is restored.

   3. Passing parameters to subprograms automatically initializes local variables when subprogram calls other than M98 are made.

4. Arguments—available only Macro Mode A. Arguments are used to pass parameters to subprograms. Parameters are the addresses which follow G65, G66, and M98 codes. Enter arguments in the NC Editor screen. Refer to NC Editor.

Refer to the Macro Mode A G Code Group Status table.

Use the softkeys to select the type of NC Variable to appear on the NC Variables screen:

• Global 100-199

• Global 500 - 999

• Tool Len Offset 2001-2200

• Work Offset 2500-3000

The More è softkey accesses these softkey choices:

• Misc 3000-3021

• Position 5061-5083

• Tool Dia Offsets 12001-12200

The More è softkey returns to the first softkey menu described above.

The Toggle Units softkey toggles the dimensional variables (Tool Offset, Work Offset, Position) between inch and metric.

Macro Mode A Subprogram Variables

In this table, the values for the NC parameters are stored in addresses #8004 to #8026 for Macro Mode A subprogram calls.

The status for each variable is stored in address #8104 to #8126.

The status for the variables is non-zero (>1) if an argument is specified in the subprogram call, and zero otherwise.

Macro Mode A Subprogram Variables

 

Macro Mode A G Code Group Status

In this table, the value for each G Code Group is stored in addresses #8030 to #8046 for Macro Mode A subprogram calls G65, G66, and user defined G codes and M codes.

The status for each G Code Group is stored in addresses #8130 to #8146.

The status is non-zero if an argument is specified in the subprogram call, and empty otherwise.

Macro mode A G Code Group Status