I use solid tools to simulate G code in a full blown seat of Vericut. I have a solid tool in Creo that is giving me a problem. The tool design is a 3/8 bull nose end mill with a .06 radius. When I run the tool path in Creo the tool stays away from drive surface as if it were a regular end mill. It has been a long time since I have try to setup a solid tool. Who out there can tell me how to setup a solid tool?
Here is what I found on Creo Help:
To Create a Tool Model
1. Create a new Creo Elements/Pro model of type Part or Assembly, give it the name of the tool.
2. Reproduce the tool geometry by using the appropriate construction features (protrusions, cuts, and so on).
3. Create a coordinate system to represent the tool origin, that is, the tool control point. This is the point that will follow the tool path computed for the NC sequence. Make sure the Z-axis of the coordinate system points in the upward direction (into the tool) for Milling and Holemaking tools; for Turning, the axes of the tool coordinate system must be oriented so that they coincide with the direction of the NC sequence coordinate system’s axes when the tool is in default orientation. Change the coordinate system’s name to TIP.
4. Establish associativity between the dimensions of the model and the tool parameters. There are two ways to do this:
• Modify appropriate dimension symbols so that they correspond exactly with the parameter names. Select the feature, display its dimensions, right-click the dimension text, and click Properties on the shortcut menu. The Dimension Properties dialog box opens. Go to the Dimension Text tabbed page and type the new symbolic name in the Name box, for example, Cutter_Diam.
• Add parameters to the model with the names corresponding exactly with the tool parameter names. This method is convenient when you want to define the tool parameters directly in the tool assembly (for example, Cutter_Diam for an insert drill as opposed to a drill bit).
• Parameter names are case-insensitive. For example, when modifying a dimension symbol or adding a model parameter for Cutter_Diam, you can use Cutter_Diam, cutter_diam, or CUTTER_DIAM; NC Manufacturing recognizes either of these strings as a tool parameter name.
• If an assembly is to be used as a tool model, you can modify dimension symbols or add parameters to any of the component parts as well as the assembly itself.
For more detail look on Help Center / Functional Areas / Manufacturing / Tooling / Solid Tools models
If you have an PTC account you can use this link:
Toolpath calculation will be based on the parameters (or dimensions named to the parameters), so it looks like using a parametric tool with same geometry settings.
Only simulation will use the solid tool.