Model-Based Definition > Model-Based Definition > Model-Based Definition > Creating Various Annotation Types > Dimension Properties > Driven Dimensions > About Annotation Plane Requirements for Dimensions with Surface References
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.
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 or double-clicking it and the annotation plane is parallel to the axis of the surface, no dimension is created and an error message is displayed.
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.
If the Annotation plane requirements are not fulfilled, then Creo Parametric displays a message stating that it is unable to create a dimension.