About Elements of Tools Setup
When you set up the tooling for a workcell or specify a tool to be used for an NC sequence, Creo NC displays the Tools Setup dialog box. This dialog box enables you to add, modify, and delete the tools, as well as view all the tools currently defined for the workcell.
When you select a Tool Table entry in the left pane of the Tools Setup dialog box, Creo NC updates the right pane to display the parameters and section sketch of the tool. Alternatively, click > to see the section view of the tool in the preview window. To remove the auto preview functionality, clear the check box adjacent to Auto Preview.
Creo NC requires the following categories of information about tools:
• Tool Table information—This set of elements defines the correspondence between a descriptive tool name (Name) and its location on the machine (Number). You can optionally supply a value for the gauge length register (Offset) and comments output for the tool (Comments). Each workcell has its own tool table.
• General—Information about the tool name, type, and tool dimensions.
• Settings—Various parameters, mostly optional, that define tool properties other than geometry:
• Cut Data—Cutting data related parameters such as speed, feed, axial depth, and radial depth. You can also specify some miscellaneous data.
• BOM—Information about the Bill of Materials for the tool.
• Offset Table—A table of offset registers and distances for mill tools with multiple tips.
• User Defined—The custom parameters to be associated with the tool. This functionality is controlled by the mfg_custom_tool_param_file configuration option.
Tool Table Elements
Name is a descriptive tool name (for example, BALL125), which uniquely identifies the tool with a certain set of parameter values. If two tools within a manufacturing process have the same Name, then all of their parameters (geometry, material, gauge lengths) are also the same. They may, however, be located in different pockets on the machine, that is, have a different Number. When you output CL data for an operation or NC sequence to a file, Creo NC outputs the pocket number (Number) in the LOADTL or TURRET statement. If the Tool Table line contains a value for Offset, it will be output as well.
For example, these Tool Table lines:
Number Name Offset Comments
------------------------------------------
1BALL1
2FLAT1 4flat end mill
------------------------------------------
1BALL1
2FLAT1 4flat end mill
produce the following CL output, respectively:
LOADTL / 1
LOADTL / 2, OSETNO, 4
LOADTL / 2, OSETNO, 4
Comments are output with the Tool Table when you use PPRINT. To add comments to a tool, type them in the Comment field on the Settings tab.
The tool name (Name) is used throughout Creo NC to identify the tool. You can store the parameters of the tool in the tool parameter file. This file has a .xml extension. You can later retrieve the saved tool parameter file and use it in a different manufacturing process. Name serves as the name for the tool parameter file. Therefore, all file naming restrictions of the operating system, such as the file name must not contain spaces or periods, apply to this parameter file too. The length of the file name must not exceed 32 characters.
 |
The tool name cannot contain hyphens (-). However, you can use underscores (_).
|
Tool Type
If you want to create a tool before you create an NC sequence, then Creo NC selects Milling as the default tool type. However, when you define a tool within a workcell, the tool types available for selection are consistent with the types of NC sequences used in the workcell. For example, if you have a Mill type workcell, the tool type selection includes milling and holemaking tools, but no turning tools. If you set up a tool at the time of creating an NC sequence, the tool types available are limited to those applicable for the current NC sequence type. For example, if you are creating a Standard Drill NC sequence, the tool types available for selection includes Drilling, Milling, and so on, while for a Tap NC sequence the only tool type available is Tapping.
The following is a list of default tools for the various NC sequences:
|
NC Sequence Type
|
Default Tool Type
|
|
Volume Milling
|
End Mill
|
|
Local Milling
|
End Mill
|
|
Surface Milling
|
Ball Mill
|
|
Profile Milling
|
End Mill
|
|
Drilling
|
Basic Drill
|
|
Roughing
|
End Mill
|
|
Re-Roughing
|
End Mill
|
|
Finishing
|
Ball Mill
|
|
Swarf Milling
|
End Mill
|
|
Pocketing
|
End Mill
|
|
Manual Cycle
|
End Mill
|
|
Face Milling
|
End Mill
|
|
Trajectory Milling
|
End Mill
|
|
HSM Rough
|
End Mill
|
|
HSM Rest Rough
|
End Mill
|
|
HSM Finish
|
Ball Mill
|
|
HSM Rest Finish
|
Ball Mill
|
|
Auto Deburring
|
Ball Mill
|
|
HSM 5 Axis Rough
|
End Mill
|
|
HSM 5 Axis Rest Rough
|
End Mill
|
|
Geodesic 5 Axis Finish
|
Ball Mill
|
|
Wall 5 Axis Finish
|
Ball Mill
|
|
Floor 5 Axis Finish
|
Ball Mill
|
|
HSM Undercut Machining
|
Side Milling
|
|
HSM 5 Axis Swarf Finish
|
End Mill
|
The tool type is stored with the tool parameters.