NC Data Options

In the Numerical Control tab, specifies the value to be used for the minimum radius constraint for circular interpolation.

In the Numerical Control tab, specifies the value to be used for the maximum radius constraint for circular interpolation.

In the Numerical Control tab, lets you include Home Point information in the NC data output, using the GOTO or FROM information defined in the machine of the Part Operation.(see Working with Generic Machine Editor).

In the NC Ouptut tab:

• when selected, you can include a GOTO statement before each tool change.
• when cleared, you cannot include a GOTO statement before each tool change.

In the NC Ouptut tab:

• when selected, the PP word syntax specified in the PP word table is output for axial machining operations.
• when cleared, GOTO statements is generated in the NC data output.

For axial machining operations using SYNTAX output mode (CYCLE), you can choose whether or not to output GOTO statements corresponding to Jump and Clearance motions.

In the NC Ouptut tab:

• when selected, points that were added by the clearance approach and distance points that were added by the jump distance are removed.
• when cleared, those points are not removed.

In the NC Ouptut tab, specifies whether to process COPY Operator Instruction or TRACUT Operator Instructions found in the Manufacturing Program.

• when selected, COPY Operator Instruction and/or TRACUT Operator Instructions are processed. In this case there is no Copy or Tracut statements remaining in the generated APT source.
• when cleared, COPY Operator Instruction and/or TRACUT Operator Instructions cannot be processed and Copy or Tracut statements remain in the generated APT source.

In the NC Ouptut tab, lets you keep or remove points that are repeated after PP statements:

• when selected, the first point after the PP instruction or user syntax is not kept if the previous one is a coincident point.
• when cleared, the first point after a PP instruction or user syntax is always kept.

In the NC Ouptut tab:

• when selected, one or more points that are aligned between two other points cannot be output.
• when cleared, one or more points that are aligned between two other points is output.

A tolerance value equal to the Machining tolerance set in the Machining Operation is used to decide whether a point needs to be kept or not.

In the NC Ouptut tab:

• This provides the capability to output the same point even if the end point of a Machining Operation and start point of the subsequent Machining Operation are exactly the same.

In the NC Ouptut tab, defines the formatting for rapid motions:

• when selected, rapid motions is preceded by a FEEDRATE syntax whose value is the Rapid feedrate specified on the machine (see Working with Generic Machine Editor).
• when cleared, rapid motions is preceded by a RAPID syntax.

In the NC Ouptut tab:

• when selected, a RAPID statement is included at the start of each operation. However, if a Clearance macro is defined on an operation, the macro definition is taken into account.
• when cleared, no RAPID statement can be included at the start of each operation.

In the Numerical Control tab, defines the format describing tool motion statements on the NC data output:

• Point (X,Y,Z): Tool point coordinates are output. A TLAXIS statement is given at the start of the generated APT source. A fixed-axis CLFile record 9000 is given at the start of the generated CLFile.
• Axis (X,Y,Z,I,J,K): Tool point coordinates and tool axis components are output. A MULTAX statement is given at the start of the generated APT source. A MULTAX CLFile record 9000 is given at the start of the generated CLFile.

In the NC Ouptut tab, defines how information such as tool names and operation sequence numbers is generated.

• None: Not generated,
• PPRINT: Generated with the PPRINT word,
• $$: Generated as a comment (not available for CLFile).

except $$

except $$

In the NC Ouptut tab, defines how Part Operation comments is generated:

• None: Not generated,
• PPRINT: Generated with the PPRINT word,
• $$: Generated as a comment (not available for CLFile).

except $$

except $$

In the NC Ouptut tab, defines how Machining Operation names is generated:

• • None: Not generated,
  • PPRINT: Generated with the PPRINT word,
  • $$: Generated as a comment (not available for CLFile).

except $$

except $$

In the NC Ouptut tab, allows you to define other formats for NC data statements allowing better accuracy for large parts:

• Number of digits: Specifies the total number of digits for each point coordinate.
• Digits after decimal: Specifies the number of digits after the decimal point for each point coordinate

In the NC Ouptut tab:

• Number of digits: Specifies the total number of digits for tool axis vector component.
• Digits after decimal: Specifies the number of digits after the decimal point for tool axis vector component.

See also Generating NC Code.