About Geometric Tolerances in Drawings
Geometric tolerances are the maximum allowable deviations from the exact sizes and shapes specified in the model design. Geometric tolerances provide a comprehensive detailing tool to:
• Specify the critical surfaces on a model part
• Document the relationship between critical surfaces
• Provide information on how the part should be inspected and what deviations are acceptable
Within drawings, you can either show a geometric tolerance from the solid model or create one.
You can attach a geometric tolerance to dimensions (reference, driven, radius, or diameter), witness lines of dimensions, datum feature symbols, single or multiple edges, or another geometric tolerance. You can also place geometric tolerances as free notes anywhere on the drawing, attach them to leader elbow for notes, or relate them to dimension text.
When you attach a geometric tolerance to an annotation, the owner of the geometric tolerance changes to the owner of the annotation it is placed on. For example, in the drawing of an assembly, if you place a draft geometric tolerance on an assembly-owned geometric tolerance, the owner of the draft geometric tolerance changes to the assembly. If you place a draft geometric tolerance on the witness line of a part-owned dimension, the owner of the draft geometric tolerance changes to the part.
You can attach multiple lines of additional text and text symbols to a geometric tolerance while creating or editing it. By default, the text style of the additional text is the same as that of the geometric tolerance text. You can edit it independent of the geometric tolerance text.
You can stack multiple geometric tolerances on another tolerance; or, if the first tolerance in a stack is attached to a dimension, you can attach them to the same dimension. As you create each geometric tolerance for a stack, the most recently created geometric tolerance is added to the bottom of the stack. If you set the stacked_gtol_align Detail option to yes, then the stacked geometric tolerances automatically align in the control frame.
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The default value of the stacked_gtol_align Detail option is no.
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To change the reference of a geometric tolerance and attach it directly to other geometric tolerances, dimensions, or datum feature symbols, the geometric tolerance must belong to the same model as the item to which it is attached.
After you attach a datum feature symbol to a geometric tolerance, you can drag or flip it using the drag handles. Within the drawing, you can drag the datum feature symbol beyond the control frame, in which case an extension line is created.
Unlike dimensional tolerances, geometric tolerances do not have any effect on the part geometry.
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• You can erase or delete geometric tolerances that are shown in drawings.
• The following rules apply when you attach a geometric tolerance to a dimension in Part mode:
◦ If you place a geometric tolerance on a dimension in a part, and create a drawing using that part, you must first show the dimension in the drawing using the Show Model Annotations option on the Dimension ribbon tab. Otherwise, the geometric tolerance is not displayed.
◦ If you attach a geometric tolerance to a part dimension that Creo Parametric cannot display in an assembly drawing, it does not display the geometric tolerance either.
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