Manufacturing > Tooling > Tool Setup Dialog Box > About the Tools Setup Dialog Box
About the Tools Setup Dialog Box
The top portion of the Tools Setup dialog box contains the Tool Table for the current machine. The Tool Table defines the correspondence between a descriptive tool name (Name) and its type.
When you select a Tool Table entry in the top portion of the dialog box, Creo NC displays the tool parameters and section sketch in the bottom portion. You can view the details of the selected tool by clicking the tabbed pages in the bottom portion of the Tools Setup dialog box.
The bottom portion of the Tools Setup dialog box contains six tabbed pages: General, Settings, Cut Data, BOM, Offset Table, and User Defined.
The General tabbed page contains text boxes for defining tool parameters, that is, parameters that specify all the dimensions of the tool. These dimension values are used in calculating the tool path and material removed, and should accurately reflect the actual tool dimensions and length units. Some of the parameters are required for defining the cross section of the tool. The actual parameter names in this category depend on the tool Type. In addition to these parameters, the General tabbed page also displays the current tool section sketch, and the text boxes for defining the following tool elements:
Name—A descriptive tool name (for example, BALL125), which uniquely identifies the tool with a certain set of parameter values. The tool name is used throughout Creo NC to identify the tool. You can store the tool’s parameters in a text file and then retrieve it to use in a different manufacturing process. The tool Name serves as the name for this parameter file, therefore, all the operating system’s restrictions for file names apply to Name (for example, it cannot contain spaces or periods). The name must be less than thirty-two alphanumeric characters long.
* The tool name cannot contain hyphens (-). Underscores (_), however, can be used.
Type—Select one of the predefined tool types available in Creo NC. Tool types correspond to the types of NC sequences performed in the workcell; the tool type, in turn, defines the tool’s cross-section and, therefore, the set of parameters you have to specify for the tool.
Material—Specify the material from which the tool is made.
Units—Length units of the tool. The default length units of a tool are those of the stock. If you change the Units, this affects the actual tool dimensions.
In addition to the tool elements listed above, you can also specify the holder diameter, holder length, tool length, flute length, cutter diameter, gauge offset of a truncated countersink tool, point angle for the drilling tool, and the point diameter in the Geometry pane of the General tabbed page.
The Settings tabbed page contains the text boxes for defining some of the tool table elements and various optional parameters that define tool properties other than geometry:
Tool Number—Corresponds to the Number field of the Tool Table, which defines the tool's pocket number.
Offset Number—Corresponds to the Offset field of the Tool Table, which supplies a value for the gauge length register.
Tool gauge lengths (Gauge X Length and Gauge Z Length)—Optional parameters used to create length qualifiers in the LOADTL or TURRET statements.
Comp. Oversize—Represents the difference between the largest measured diameter of the cutting tool and the nominal cutting tool diameter (Cutter Diameter). Set this parameter if the actual cutting tool diameter is greater than the programmed cutting tool diameter. Creo NC uses this value for gouge checking.
Long Tool—Select this checkbox if the tool is too long to retract to the Rotation Clearance level during 4-axis machining. If you mark the tool as long, the tip of the tool moves to the Safe Rotary Point (specified in the Operation Setup dialog box) during table rotations.
Comments—A text string that is stored along with the tool parameters and is output with the tool table using PPRINT. If you want the tool table to show this comment, click Edit > Table Comments on the top menu bar of the Tool Setup dialog box, and select the Use TOOL_COMMENT parameter option. If you want the Tool Table to show a comment other than the comment in the Comments string for a tool, then click Edit > Table Comments, select New comment, and type in a new comment.
Custom CL Command—Insert a CL command that you want to run during the change of tool. The CL command is inserted before the LOADTL command in the CL file. A maximum of five lines of Custom CL commands are allowed in the notes.
The Cut Data tabbed page lets you specify cutting data—feed, speed, axial and radial depths for roughing and finishing with the tool, based on the stock material type and condition. Before specifying the cutting data you must set up your Materials directory structure. The cutting data (feed, speed, axial and radial depths) for roughing and finishing with this tool, based on the stock material type and condition. This data is stored in a separate file with the same file name as the geometry and other tool parameters, but located in the appropriate Materials directory.
The BOM tabbed page provides information about the Bill of Materials for the tool.
The Offset Table tabbed page lets you set up tools with multiple tips.
For tools of type TURNING and TURN-GROOVING, the Offset Table tabbed page contains the Enable Multiple Tips and Tool Flashing check box. Click this option, right-click a row for a tip with a Standard orientation, and click Add Flashed Tip on the shortcut menu. Another row for the tip with its orientation set to Flashed is created. The new row has the same Z Offset, X Offset, and Angular Offset values. You must specify unique values for Offset Number.
Use standard selection methods to select multiple rows. If you delete a row for a tip with a Standard orientation, its corresponding row with a Flashed orientation is also deleted.
The following columns in the Offset Table tabbed page contain attributes of a tip for a tool.
For Milling:
Offset Number—Specify a unique integer for a tip. This value in the CL data is output as OSETNO in a LOADTL/TURRET statement.
Z Offset—Specifies the Z-offset value for a tip.
Comment—Adds any comments associated with the tip.
Output Tip—Specifies the tip to be used for the CL output of the sequence. This column is available only for multi-tip tools.
Additionally, for tools of type TURNING and TURN-GROOVING, the table contains the following columns:
X Offset—Specifies the X-offset value for a tip.
Angular Offset—Represents the rotation about the holder’s axis for each tool tip of the multi-task holder. TIP/TIP1 is the zero position for the angular offset. You cannot edit this value in the Tools Setup dialog box.
Orientation—Specifies whether the orientation of the tip is Standard or Flashed. A Flashed orientation is possible only if tool flashing is enabled.
In case of tools of type Multi-Task, the table contains the following additional columns. You cannot edit these values in the Tools Setup dialog box.
GAUGE X LENGTH—Specifies the gauge length of the tip along the X-axis.
GAUGE Z LENGTH—Specifies the gauge length of the tip along the Z-axis.
The User Defined tabbed page lets you define custom parameters to be associated with the tool. The mfg_custom_tool_param_file configuration option controls the appearance of this tabbed page. The User Defined tabbed page appears in the Tools Setup dialog box only if you set the value of the mfg_custom_tool_param_file configuration option to point to a valid user-defined parameter file. The user-defined parameter file must have a .xml extension. While parsing the user-defined parameter file, if Creo NC encounters a parameter that is not valid, the entire file is ignored and the User Defined tabbed page is not displayed. Any changes that you want to make to the user defined parameter definitions can be done only by editing the user defined parameter file. To update these changes in the Tools Setup dialog box, click Reload UDP file in the User Defined tabbed page. Alternatively, you can reload the manufacturing model for the changes to take effect.
The user defined manufacturing parameters are stored within the manufacturing model. To delete all the user defined parameter definitions from the manufacturing model, delete the mfg_custom_tool_param_file configuration option and restart Creo Parametric. When you reopen the manufacturing model for which you deleted the tool parameter definitions, Creo Parametric prompts you to choose whether to delete the existing definitions or keep them.
* If you specify two values for the same parameter using any of the tabbed pages other than the General tabbed page in the Tools Setup dialog box, the value specified using the User Defined tabbed page takes precedence over the former. For example, if you specify 1000 as the value for the SPINDLE_SPEED parameter in the Cut Data tabbed page and 1500  as the value for this parameter in the User Defined tabbed page, then the value specified in the User Defined tabbed page is used as the spindle speed of the tool.
After specifying the details for a tool you can save the tool for later use in another NC sequence. The tool along with the parameters are saved in a file with the same name as that of the tool. This file has a .xml extension. You can also open and edit tool parameters saved in the previous versions (in files with .tpm and .tprm extensions) in the current Tool Manager. However, you can save the tool parameters only with the .xml extension from the current Tool Manager.
For solid tool models, you can also add user-defined parameters in the tool model.
The Tools Setup dialog box is not available on the top toolbar when you right-click and invoke the PLAY PATH dialog box for an NC sequence or an operation from the Model Tree Window.