About Annotation Plane Requirements for Dimensions with Surface References
The Annotation plane requirements when creating a driven dimension that includes surface references are as follows:
• Planar surface reference—The annotation plane must be perpendicular to the planar surface reference.
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• If the planar surface reference is perpendicular to the annotation plane and parallel to the other dimension reference, Creo Parametric creates a linear dimension.
• If the planar surface reference is perpendicular to the annotation plane but not parallel to the other dimension reference, then Creo Parametric creates an angular dimension.
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• Cylindrical surface reference—The annotation plane must be perpendicular or parallel to the axis of the cylindrical surface.
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• If you select a cylindrical surface reference by clicking it and the annotation plane is perpendicular to the axis of the surface, Creo Parametric creates a radius dimension.
• If you select a cylindrical surface reference by double-clicking it and the annotation plane is perpendicular to the axis of the surface, Creo Parametric creates a diameter dimension.
• If you select a cylindrical surface reference by clicking it and the annotation plane is parallel to the axis of the surface, Creo Parametric creates a linear diameter dimension.
You can change the orientation of the diameter dimension by using the Change Orientation command. To access this command, right-click the dimension and select Change Orientation. In the Annotation Plane dialog box, click Named model orientation and select a named orientation from the list.
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• Conic surface reference—The annotation plane must be perpendicular or parallel to the axis of the cone for a dimension to be created.
• Spherical surface reference—There are no requirements for the annotation plane except those imposed by the other dimension reference.
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If you select the spherical surface reference by clicking it or by double-clicking it, Creo Parametric creates a spherical radius dimension or diameter dimension, respectively.
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If the Annotation plane requirements are not fulfilled, then Creo Parametric displays a message stating that it is unable to create a dimension.