Manufacturing > Manufacturing > Tooling > Tool Setup Dialog Box > Using the Cutting Data Supplied for the Tool
Using the Cutting Data Supplied for the Tool
When you use a tool in an NC sequence, the feeds and speeds stored with it are not automatically used as the NC sequence feeds and speeds. When you set the manufacturing parameters in the Edit Parameters dialog box, you can click Edit > Copy From Tool and select whether you want to copy All parameters, or just the Speed, Feed, or Depth. Finally, select whether you want the Roughing or the Finishing parameter values.
You can also use the following mechanism to utilize the speed and feed data stored with the tool when creating an NC sequence.
All the cutting data that you specify in the Tools Setup dialog box is stored as tool parameters. For each data type, there are two separate parameters, one for Roughing and one for Finishing. The following table lists the tool parameters corresponding to the cutting data and the miscellaneous data supplied for the tool.
Cutting Data
Speed (rev per minute)
Speed (length units per minute)
Feed (per minute)
Feed (per tooth or per rev)
Axial depth
Radial depth
Misc Data
Tool Parameter
Coolant Option
Coolant Pressure
Spindle Direction
When you create an NC sequence, you must assign the values of these tool parameters to the appropriate manufacturing parameters through relations. For example, you can specify relations such as:
You can specify these relations either in a site file or as a parameter value directly in the parameter tree for the NC sequence. To specify the relation above, for example, type =TOOL_ROUGH_FEED_RATE as a value for the CUT_FEED parameter.
If you change the tool, or change the cutting data supplied for the tool, the value of the speed or feed parameter driven by the relation is automatically updated.
Alternatively, use the mfg_param_auto_copy_from_tool configuration option to have Creo NC copy all, miscellaneous, or cutting parameters from the tool to the NC sequence. Based on the value that you specify for the mfg_param_auto_copy_from_tool configuration option, Creo NC copies and displays the tool parameter values in the Param Tree dialog box. However, Creo NC copies the tool parameters to the Param Tree dialog box only when you create an NC sequence.
Changes are not automatically updated if you redefine an NC sequence or make any changes to the tool parameters. If you make any changes to the tool parameters, you must then copy the parameters using the Edit menu in the Param Tree dialog box to update the NC sequence with the modified values.
If you switch from Rough machining to Finish, you must update the relations accordingly. Creo NC does not automatically switch to Finish parameters from the tool cutting data. The manufacturing parameter values are driven by whatever relations you specify.