About Geometric Tolerances in Drawings
Geometric tolerances are the maximum allowable deviation from the exact sizes and shapes specified in the model design. Geometric tolerances are a comprehensive detailing tool that enable you 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), set datums, 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.
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. |
However, to attach a geometric tolerance directly to other geometric tolerances, dimensions, or datums, it must belong to the same model as the item to which it is attached.
You can specify a set datum plane or an axis as a reference for a geometric tolerance. Before you do so, you must set the datum plane or axis. You can also specify a set datum plane or an axis contained in an inheritance feature of a model as a reference for a geometric tolerance. To do so, select the set datum plane or the axis on the Model Tree or in the graphics window.
You can attach a model set datum to a model geometric tolerance if the gtol_datums Detail option value is set to std_iso, std_iso_jis, or std_jis. You can also attach draft set datums or draft datum axes to draft geometric tolerances.
After you attach a set datum to a geometric tolerance, you can drag or flip it using the set datum box or the drag handles. Within the drawing, you can drag the set datum beyond the control frame, in which case a witness 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. If you delete a shown geometric tolerance, it is deleted in both the drawing and the model.
• You cannot mix draft datums or draft axes with model geometric tolerances, or model datums with draft geometric tolerances.
• 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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