Options > NC Programs

The NC Programs items define the default NC Program options. The dialog contains these options:

Verification

Automatically ignore warnings for missing connections — Select to automatically ignore warnings about connections that are not verified.

Automatically ignore warnings for missing shank — Select to automatically ignore warnings about shanks that are undefined.

Output

File Type — Specify the file type used to output the toolpaths:NC Program (*.tap), a Cutter Location (standard cutter location format file extension .cut) or a Duct Picture (.pic).

Format — Specify the format of the cut file (Binary, ASCII, or Print). This option is not available if you select NC program as the File type.

The default setting is Binary, which is the standard format used by the Autodesk Manufacturing Post Processor Utility. ASCII formats create much larger cut files, but are necessary when:

• User edits are required.
• Files are transferred between UNIX and Windows platforms. An alternative way to transfer files between the two platforms is to use the edit tpoutput cutfformat command.

  The Print format is recommended when Autodesk Manufacturing Post Processor Utility is NOT used.

Write File for Each Toolpath — Select so a separate file is written for each toolpath in an NC program.

Use Toolpath Workplane for Output — The NC program is written using each toolpath workplane. When deselected, the NC program uses the output workplane defined in the NC program dialog.

Produce Info File — Select if an Information File is required. $$$MAH what is an info file?$$$

Allow duplicate toolpaths — Select so you can add a toolpath to an NC program multiple times. When you write the NC program, PowerMill displays a message to tell you that the NC program contains duplicates of a toolpath.

Option File — Specify the appropriate extension for a machine-tool option file. For example, if you have a Heidenhain controller, it is likely that you need to change the default .tap extension to be .hnc. The list selection specifies the machine tool controller; the second box specifies the extension applied to the output file. If you do not want your output file to have an extension, enter a period (.) in the extension box.

Path — Specify the file directory where NC programs are written to.

Append toolpaths

Automatically append toolpaths to active NC Program — Select this option to automatically add toolpaths to the active NC program.

Cutter Compensation

Wear compensation matches full radius — Apply the options selected for full-radius-cutter compensation to wear compensation.

There are different ways to apply cutter compensation:

Full radius compensation — If the tool should be on the left of the part, you need a compensation-left code (G41 on Fanuc) and enter the radius value in the offset register.

Wear compensation — To allow for a tool that is slightly smaller than the specified tool. In this case, you have a choice:

• If the tool is on the left of the part, you may want to use G41 and enter a negative value into the offset register. In this case, select Wear compensation matches full radius.
• You may want to use G42 and enter a positive value in the register. In this case, deselect Wear compensation matches full radius.