Converting from the Single Body Environment to the Multibody Environment
In sheet metal models created prior to Creo Parametric 11.0.0.0, there is one, legacy, sheet metal body and it is linked to the part. Legacy parts can have a body with geometry or an empty body.
• Bodies with geometry behave like a legacy body.
• Empty bodies behave like new bodies.
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All sheet metal models created prior to Creo Parametric 11.0.0.0, are referred to as legacy parts in this topic.
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The following sections describe converting parts from a single body environment to the multibody environment.
When you open a legacy sheet metal part with geometry created using a version earlier than Creo Parametric 11.0.0.0, the part contains one sheet metal body with all sheet metal geometry of the part. All parameters and relations are present in the part and can be edited. The sheet metal body parameters are linked to the part and are read-only.
Unlinking a Legacy Body from the Part
When you unlink the legacy body from the part, it becomes a sheet metal body with parameters taken from the part. The values of these parameters are no longer linked to the part, they are not updated when the part parameter values change, and they are no longer read-only. You can now change the values of these parameters in the Sheetmetal Preferences dialog box. When you unlink a body from the part, feature relations are removed, but the features are still dependent on the body preferences.
When you link a legacy body back to the part, the features will still point to the body parameters.
Relations
Starting in Creo Parametric 11.0.0.0, standard sheet metal relations are no longer created and managed by the Creo Sheetmetal module. Sheet metal parameters driven by relations in legacy parts are read-only in the Sheetmetal Preferences dialog box. These relations can still drive parameters in the part, and in legacy bodies that are linked to the part. When you unlink the body from the part or create a new body in a legacy part, features point to the body parameters. You can now change the value of these parameters in the Sheetmetal Preferences dialog box. Changing them to thickness related values from the Sheetmetal Preferences dialog box will show them as Locked by Sheetmetal in the Parameters dialog box.
For example: when the part relation SMT_DFLT_BEND_RADIUS=SMT_THICKNESS appears in a part, the part bend radius parameter is locked by the relation and is read only. To change the bend radius for the part, you must first delete this relation in the Relations dialog box.
When you edit the definition of a legacy feature in Creo Parametric 11.0.0.0 or later, the dimensions of the feature use the body parameters.
Thickness Dimension in Legacy Parts
In parts created prior to Creo Parametric 11.0, the thickness dimension value is linked to the part thickness parameter. When you unlink the legacy body from the part, the feature dimension is driven by the body thickness parameter. The body parameter and the thickness dimension are no longer affected by the part parameter value.
Bend Allowance Driven by Material in Legacy Parts
In parts created prior to Creo Parametric 11.0.0.0, the bend allowance, if it is taken from the material, it is taken from the material of the legacy body. When you unlink and then link a legacy body, the bend allowance values are taken from the master material.
Legacy Model with a Merge or Inheritance Feature
In legacy models with a merge or inheritance feature, the part thickness is controlled by the legacy part thickness and is locked. When you open the part in Creo Parametric 11.0.0.0 or later, and unlink the body from the part, the following occurs:
• The thickness parameter of the part becomes unlocked and can be edited.
• The thickness parameter of the body is locked by copy and points to the legacy source body thickness.
Legacy Templates
When you create a new sheet metal part from a legacy template, the sheet metal body is linked to the part during retrieval. We strongly recommend that you use templates created in Creo Parametric 11.0.0.0 or later.