General Information dialog (Turn/mill)

Dogleg rapid moves — This setting only affects the simulation. When the option is selected, both simulated axes move at the maximum rate during a rapid move from point A to point B until one of the moves is completed. The machine then proceeds to B with the other axis continuing in a straight line.

When the option is unselected, the simulation shows all rapid moves from point A to point B as straight lines

B-Axis Support — Select this option for machines which have a B-axis that allows tools to engage part at various angles.

• Use coordinate transformation for B-Axis on OD — Select this option to use a work coordinate system for the B Axis even for an OD feature.
• Offset fixture to feature origin — This allows selection of origin for B-axis angular output.
• Use Fixed B-Axis Holders — Select this option to enable the machine simulation to use Fixed Holders and error checking.
• Use setup coordinates for B-Axis on OD — Select this option if you want to output the XYZ positions in the Setup Coordinate System located at the face of the part, along the rotary axis. If deselected, the Feature Coordinate system is used, and a coordinate transform (for example, G68.5) must be added to the Post Processor.
• B-Axis range — Select your B-Axis range.

Rotary Tool section:

Convert X coordinates to radius for: — Select which features to output radial values for.

In Turn/Mill posts, the reserved word <X-COORD> normally has a factor setting of 2 for outputting diameter values for turning. The X coordinates for Turning and Milling use this common reserved word and its formatting. Depending on the machine, the X coordinates for milling may need to be output in radial form.

Select from:

• Features on OD — Output radial values for features using X-axis tools.
• Features on Face — Output radial values for Z-axis tools working on end face of part.
• B-Axis Features — Output radial values for angled features.
• 5 Axis features — Output radial values for 5-axis simultaneous features.

Macro Type — Select how macros are formatted when the part program requires them.

Select from:

• Local — This places macro definitions within the main NC part program.
• End of Program — This places macro definitions at the end of the main part program (for example, Heidenhain controls). The PROGRAM END program format should be specified for output at the end of the main program and the FILE END program format should be specified for output at the end of these macro definitions.
• Not Available — Select this option if macros are not available.
• Individual Files — This places macro definition in a separate file (for example, FANUC and GE MC 2000 controls). The name of each macro file consists of the assigned name that was specified in Post and the system-assigned macro number. The internal sub-program name is automatically added to the main program name as the external file name.
• One File — This places all macro definitions in one file. Post generates two files, the main part program and a file containing all macros. This option can output to Bridgeport controls via the EZ-Utils module, CNCCOMMUNICATION option (Heidenhain DNC utility).

The name of the macro file comprises the assigned name specified in Post, MA (representing the macro specification) and the .txt file extension. For example, samplema.txt (macro file) and sample.txt.

Call local macro after it is defined — Select this option to automatically execute a macro when it is defined. Some controls (such as the Heidenhain 370) automatically execute macros when they are defined. For these controls deselect Call local macro after it is defined so that the macro is not called twice. For other types of controls, leave this option selected.

Reuse local macro number — This affects the behavior of the <MACRO#> reserved word which can be used in the Open / Close / Call Macro formats. Deselect this option to increment the number every time you define a new macro, or select it to keep using the same number.

If deselected, the first move is not in the macro, instead it is assumed that it is output on the canned cycle line.

To properly include the first move in a macro, you must enable this option and use the logical variable <CYCLE-MACRO> to suppress performing the canned cycle on the canned cycle line.

For a Fanuc 0M, if a canned cycle line ends with K0, the machine goes into canned cycle mode, but the actual canned cycle is not performed. Here is the drilling format for the Fanuc 0M.

{N<SEQ>}<CYCLE>{X<X-COORD>}{Y<Y-COORD>}
R<ABS-ZCLEAR>Z<ABS-DEPTH>F<FEED>
<IF><CYCLE-MACRO><THEN>
K0
<ENDIF>
<EOB>

Post supports local coordinates — Select this option for a post that redefines the coordinate system using datum shifts.

Post supports incremental macros — Select this option for a post that program milling macros incrementally.

Force segment start for each operation — Select from:

• Controlled by setting in the CAM software — Set this option in Options > Posting in FeatureCAM.
• ON — Select this option to force a Segment Start format for each operation.
• OFF — Select this option to disable forced Segment Start formats for each operation.
Note: If you select ON or OFF, the status is displayed in Options > Posting in FeatureCAM.

NC File Extension — The default file extension for your CNC programs. For example if it is set to txt, and your part is called bracket, the G-code file is called bracket.txt.

Sequence Max — Select this option to enter a maximum value for sequence numbers, after which sequence numbers restart. If Sequence Max is deselected, no limit is set.

Polar interpolation done by— Select how the polar interpolation is performed:

• The CAM software — FeatureCAM converts the Cartesian coordinates into polar coordinates before being sent to the post processor.
• Machine Tool — FeatureCAM sends the Cartesian coordinates to the post processor. The formats of the post processor must be configured to request polar interpolation from the machine control.

Machine tool and post support cylindrical interpolation — Enable this option to support cylindrical interpolation in the NC code for Turn/Mill and 4th-axis wrapped parts, using G07. This makes the NC code shorter, and smaller in memory size, and gives better interpretation of cutter compensation.

Restrict angles to be between -360 and 360 — When selected, moves containing rotations greater than 360 degrees are split into smaller pieces.