When you construct a GD&T tolerance symbol, a tolerance label is constructed that conforms to the GD&T standard. The label includes such information as the appropriate GD&T symbol, zone size, maximum/minimum material conditions, datum references, and so on. The tolerance symbol, modifiers, and any text are enclosed in a box which is referred to as the Feature Control Frame (FCF). The tolerance label is colored green (by default) when it refers to a single part and magenta (by default) when it refers to an assembly. You can set different defaults for these colors; see
Change default settings.
Before specifying some tolerances, you must first define a datum (or datums) as a reference from which the tolerance can be measured.
You can view the tolerance symbols that have already been applied to a model in the Structure Browser, as you would other custom process features.
To start creating a tolerance symbol, you first select the features of the model to attach it to, and then select the required tolerance symbol. These are specified in the Tolerances dialog box which is accessed by double-clicking Tolerance in the Template Browser. The Tolerances dialog box contains the following options:
Elements:
Specify the feature or list of features to be referenced by the tolerance definition. A feature can be a valid face, a functional feature, or an existing GD&T tolerance or datum on which the tolerance will be constructed. The selected feature(s) determine which tolerance symbols can be displayed in the Valid Types cascade list.
Owner:
To select features over multiple parts of one assembly, first specify the assembly in the Owner box and then specify the features with Elements. When the features are specified first, this field is used to display the name of the owning part of the selected features.
Tol Type:
This display field indicates the type of tolerance, for example, "Position" or "Concentricity".
Valid Types:
Select the desired tolerance symbol from the available options.
Only those tolerance types that make sense for the geometry selected are displayed as Valid Types.
To create a tolerance on a part,
The tolerancing menu enables you to add a symbol to define the tolerancing constraints of the selected feature. To attach a tolerance symbol:
1. Click 3D Documentation and then, in the Annotate group, click Symbol.
2. Click to expand the GD&T category in the template browser and double-click Tolerance.
3. To specify features over a single part: Specify the desired elements of the model to which you want to attach a tolerance symbol. The owner of the elements is displayed in the Owner box.
4. To specify features over multiple parts of one assembly: Specify the assembly name in the Owner box, and then specify the elements.
5. Click the Valid Types box. Creo Elements/Direct Modeling displays all the tolerancing symbols relevant to the selected feature.
6. Click the symbol which represents the type of tolerance that you want to define.
7. Click . A tolerancing dialog box which is specific to that symbol is displayed. For example, if you select the symbol representing Straightness tolerances, the Straightness dialog box opens.
8. Specify if the symbol should be attached to a docuplane or be free.
9. Complete the symbol-specific dialog box to define the tolerance characteristics.
10. Specify the size or shape of the tolerance zone as appropriate.
11. Specify a material modifier symbol if required, for example MMC or LMC.
12. Specify the maximum permitted bonus tolerance if appropriate.
13. Specify a tangent plane symbol, or a free state condition as additional modifiers if appropriate.
14. Define inspection information if required.
15. Specify the datum(s) to be used as references for the tolerance if required.
16. Click to attach the defined tolerance symbol.
To update datum references
In the Datums dialog box, Upd. Refs automatically updates all tolerances that reference the modified datum. For example, if you modify datum A to be called datum B, Upd. Refs corrects the tolerances referencing this datum.
Upd. Refs also re-evaluates the tolerances referencing a new datum definition. For example, if a tolerance uses datum A, and this is changed from a feature of size datum to a planar datum, then the tolerance is updated to show a GD&T call-out to a planar datum and not to a feature of size datum.
To reassociate lost datums
ReAssoc in the Datums dialog box can be used to "reassociate" a datum to a tolerance that refers to a datum of that name. In other words, if you delete a datum (with identifier B, for example) that is referenced by a tolerance, you can create a new datum (also called B) and use this as the datum reference for the now-invalid tolerance.
To use ReAssoc, simply create or modify a datum with the desired identifier, and click ReAssoc in the Datums dialog box.
Symbol.
. A tolerancing dialog box which is specific to that symbol is displayed. For example, if you select the symbol representing Straightness tolerances, the Straightness dialog box opens.