NC Preferences > Toolpath

The Toolpath tab of the NC Preferences dialog specifies the default values in the NC Program dialog.

To display the NC Preferences dialog, from the NC Program context menu, select Preferences.

This tab contains the following:

Comments — Click to display the NC Program Commands/Comments Preferences dialog. Use this dialog to specify default commands and comments you want to insert into the NC toolpath.

Tool Change — Select the default value for the tool change. Determines when a Load Tool command is written.

• On Change — Select to add a load tool command at the beginning of the first toolpath and subsequently only if the tool geometry changes. This adds a load tool command if the tool length is different.
• Always — Select to add a load tool command at the beginning of every toolpath even if the tool parameters are the same.
• On New Tool — Select to add a load tool command at the beginning of the first toolpath and subsequently only if the toolpath uses a different tool entity from the previous toolpath.

Tool Numbering — Select the default value for the tool number. Determines which tool in the carousel or reference number to use.

• Automatic — Select to give a new number to each new tool used. When a tool is reused in another toolpath, its existing number is used.
• As Specified — Select to use the tool number specified in the Tool entity dialog. If a tool number has not been specified in any dialog, a ? is displayed in the toolpath list — however, if it is the first toolpath, the tool number is assumed to be 1.
• Sequential — Select to sequentially name the tools. By default, the first tool is named 1, followed by 2, 3, 4 and so on. The Tool Number field in the specific toolpath area of the NC program dialog defines the first number in a sequential series. If the same tool is used in the subsequent toolpath in an NC program, the tool number is enclosed in brackets, for example, (1).

The Tool Numbering and Tool Change options are more easily explained by an example.

This example contains four toolpaths. Each toolpath uses a specific tool entity.

• Toolpath 1, Tool Entity 4
• Toolpath 2, Tool Entity 7
• Toolpath 3, Tool Entity 7
• Toolpath 4, Tool Entity 3

In this example, tools 7 and 3 are 10 mm ball-nosed tools.

The tool numbers are summarised in the table below:

Tool Change Position — Select whether the tool change takes place before or after the connection move.

• After Connection — Select for the tool change to take place after the connection moves. This is the default option.
• Before Connection — Select for the tool change to take place before the connection moves.

Cutter Compensation — Specifies the default value for cutter compensation.

For example, suppose you require a tool radius offset of 0.2 in the first toolpath and 0.4 in the second toolpath and set the radius offset number to 31 in the first toolpath and 32 in the second toolpath, the NC program file contains the codes G41 ... D31 in the first toolpath and G41 ... D32 in the second. Then type 0.2 into register 31 and 0.4 into register 32 and the values 0.2 and 0.4 will be used for the first and second toolpaths respectively.

Most people use the same number for the length offset number, the radius offset number, and the tool number. For example they expect to see T5, H5 and D5 in the same toolpath. Alternatively the radius offset number may have a fixed connection with the tool number. For example, if the tool number is 5 the radius offset number is 35, if the tool number is 7 the offset is 37. This can be easily taken care of by the postprocessor.

Occasionally however it is not possible to do this, so PowerMill has the ability to change the numbers if this is really required, but the default numbers are usually correct, and the numbers are used only if length or radius compensation is used.

Length — Select the type of cutter length compensation on the machine tool controller. The tool length used in PowerMill remains unchanged. This only appears on files postprocessed for the Heidenhain control. It enables you to alter the length of the tool in the NC toolpath.

• Off — When selected, the value 0 appears in the file.
• On — When selected, the default is the tool entity length.

Radius — Select the type of cutter radius compensation on the machine tool controller. The tool radius used in PowerMill remains unchanged.This enables you to offset a toolpath at the machine controller by an amount stored in a specific offset register.

• None — When selected, there is no radius cutter compensation.
• 2D — When selected, uses 2D cutter compensation which issues a left code.
• Left — When selected, cutter compensation is added by issuing a G41command at the beginning of the tool moves that require compensation.
• Right — When selected, cutter compensation is added by issuing a G42 command at the beginning of the tool moves that require compensation.
• 3D — When selected, writes contact normal vectors for use with 3D cutter compensation. This is essential when the machine tool does the 3D cutter compensation and PowerMill outputs i, j, k vectors in the tape file.

Coolant — Select the coolant type:

• None — When selected, there is no coolant output.
• Standard — When selected, turns the coolant on.
• Flood — When selected, turns the coolant to flood.
• Mist — When selected, turns the coolant to mist.
• Tap — When selected, turns the coolant to tap.
• Air — When selected, turns the coolant to air blast.
• Through — When selected, turns the coolant to through spindle.
• Double — When selected, enables two coolant codes.

PowerMill turns the coolant off at the end of a toolpath.

You can apply coolant several different places. For more information see Coolant and how it updates/flows.