Creating a Custom Shape Tool

Custom shape tools at the time this set of instructions was written is for use with Planar Mill and Planar Profile operations only.

The following steps are only a recommendation.

• Start NX9.0

• Create a new file inside NX

• Select OK
• Create a Sketch

• Sketch the Profile of your custom tool
• Your sketch should look similar to this:

• Print your sketch for reference in creating your custom shape tool
• Start Manufacturing Application inside NX

• Choose cam_general for the CAM Session Configuration
• Select mill_planar for the CAM Setup to Create

• Select OK
• Set the Machine Tool View in your operation navigator

• Create a New Tool

• Select Mill_user_defined as the subtype
• Enter 060_RADIUS_CUTTER for the nme
• Select OK
• The User Defined Mill Tool Dialog Appears

• Remove the current Segments for the default tool

• Enter the Flute length to 0.625
• Change the Number of Flutes to 1

• Enter the values to define your radius cutter

Note: At the time the smallest segment length permitted is 0.005. The second segment in the list is 0.005 and it defines the radius. We can account for the 0.005 when we define the tracking points. This will be an issue if you plan milling with the bottom of the tool. It will gouge the part by that 0.005. This is a current limitation of the user defined tool interface.

• Now it is time to define the tracking points of the tool

Note: A tracking point is a point on the cutting portion of the tool that will touch the boundary that you wish to cut in planar milling or planar profiling. Each tracking point contains a Diameter value and Distance value. The distance value is from the bottom of the tool. Tracking points can be named.

• Delete the tracking points

• For a best practice, create a tracking point and name it Centerline with a diameter of 0.000 and a distance of 0.000

• Create another tracking point and name it Rad_corner with a diameter of 0.505 and a distance of 0.065 (0.060 Radius of cutter + 0.005 for software shortcoming)

• Other optoins available in the tracking point dialog box include:
  • Z Offset
  • Tool Adjust Register
  • Cutcom Register

Note: All three of these options can also be utilized to eliminate the 0.005 for the software’s shortcoming.

• Select OK
• Assign the values in the dialog box
• Export the tool to the library if desired

• Select OK
• Save the NX file

This concludes the activity of creating a Radius cutting tool.