Manage Annotations
Unvalidated Annotations
The Unvalidated tab in the Manage Annotations window shows a list of all the
annotations in the model that have been created with native Creo tools and have not been validated by GD&T Advisor. Each item in the list includes the annotation ID and the status condition indicating the reason it cannot be validated. When you click on an item in the list, the annotation is highlighted in the
CAD model unless the annotation is on a hidden layer (e.g., not shown in the active combination state).
This tab includes the following action buttons:
Delete Selected — Select one or more items in the list and then click on this button to delete the selected annotations from the model.
Refresh List — After making modifications to annotations in the model (e.g., to correct issues identified in this window), click on this button to update the list of unvalidated annotations.
Status Conditions
Any Annotation
• Annotation cannot be validated; license option not available — Annotation validation requires the GDT_ENTERPRISE license option.
Datum Feature Symbols
• Reference surface belongs to an existing feature — One or more, but not all, of the datum feature symbol reference surfaces is also referenced by an existing
functional feature. A surface may only be referenced by a single functional feature. You should remove the surface from the datum feature symbol references and then click
Refresh List.
• Another DFS is attached to the feature — There is already another datum feature attached to the functional feature. You should probably delete this annotation.
• Duplicate DFS label — There is another datum feature with the same label. All datum feature symbols must have unique labels.
Dimensions
• No associated feature identified — No functional feature that is associated with the angular dimension has been identified. You should probably delete this annotation.
• Dimension type not supported — The dimension type is not supported. It is OK to leave the dimension in the model, but its effect on the constraint state of the functional features in your model will be ignored.
• There are no surface references — The dimension does not have any surface references defined. You should identify the applicable surface references for the dimension and then click Refresh List.
• Reference surface belongs to an existing feature — One or more of the dimension reference surfaces is referenced by an existing functional feature. You should either delete the dimension or remove the surface from the dimension references and then click Refresh List.
• Dimension references not supported — The dimension is not supported. Linear offset dimensions may only reference planar surfaces. It is OK to leave this dimension in the model, but its effect on the constraint state of the functional features in your model will be ignored.
• Dimension cannot be validated automatically — One or both surface references is also referenced by an existing feature. You should edit the applicable functional feature to include the dimension.
• Dimension may not be applicable to feature type — The dimension may not be applicable to the functional feature that would be created based on the dimension’s the surface references.
• Related dimensions are missing — The functional feature defined by the dimension references requires other dimensions that are missing from the CAD model.
• Hole placement reference is not supported — The
CAD feature must reference either a planar surface feature or a shaft feature.
Geometric Tolerances
• No attachment to part geometry — The geometric tolerance it not attached to the part geometry. You should either attach the geometric tolerance to a part surface or to another annotation that is properly attached to the part and then click Refresh List.
• Invalid attachment to part geometry — The geometric tolerance has an invalid attachment to the part geometry (for example, attached to an edge). You should either attach the geometric tolerance to a part surface or to another annotation that is properly attached to the part and then click Refresh List.
• Reference surface belongs to an existing feature — One or more, but not all, of the geometric tolerance reference surfaces is referenced by an existing functional feature. You should either delete the geometric tolerance or remove the surface from the annotation references and then click Refresh List.
You may select one or more items in the list and the click on the Delete Selected button to delete the annotation from the CAD model.
After making changes to your Creo model, you should click the Refresh List button to have the application update the model and refresh the list.
Mismatched Annotations
The Mismatched tab in the Manage Annotations window shows a list of all the
annotations for which there is a mismatch with the corresponding GD&T Advisor data. Each item in the list includes the annotation ID and the status condition indicating the reason it cannot be validated. When you click on an item in the list, the annotation is highlighted in the
CAD model unless the annotation is on a hidden layer (e.g., not shown in the active combination state).
This tab includes the following action buttons:
Update Selected — Select one or more items in the list and then click on this button to update the selected annotations to the expected values, as specified in the GD&T Advisor model. Note that in some cases, the annotations cannot be updated automatically. In those cases, the selection checkbox is disabled.
Refresh List — After making modifications to annotations in the model (e.g., to correct issues identified in this window), click on this button to update the list of mismatched annotations.
Status Conditions
Datum Feature Symbols
• Surface references do not match feature references — The CAD annotation surface references do not match the GD&T Advisor feature surface references. Click Update Selected to update the CAD annotation references to match the feature references.
• Additional text differs from expected value — The additional text for the CAD annotation differs from what is expected by GD&T Advisor. Click Update Selected to update the additional text to match the expected value.
Dimensions
• Surface references do not match feature references — The CAD annotation surface references do not match the GD&T Advisor feature surface references. Click Update Selected to update the CAD annotation references to match the feature references.
• Origin symbol not applicable to size dimensions — The dimension origin symbol is not applicable for size dimensions. Click Update Selected to remove the origin symbol from the dimension.
• Origin symbol applied to wrong endpoint — The dimension origin symbol should be applied to the origin feature of the dimension (i.e., the earlier of the two features in the Feature Tree). Click Update Selected to apply the origin symbol the other dimension endpoint.
• Dimension is expected to be basic — GD&T Advisor expects the dimension to be basic. Click Update Selected to make the dimension basic.
• Dimension is expected to be toleranced — GD&T Advisor expects the dimension to have a tolerance. Click Update Selected to make apply a tolerance to the dimension. You should modify the tolerance type and values as desired.
• Unexpected text in prefix or suffix — The text in the prefix and/or the suffix of the dimension does not match the expected values. Click Update Selected to update the prefix and suffix to the expected text.
• Shape modifier required in prefix — The required shape modifier is missing in the dimension prefix. Click Update Selected to update the prefix to include the expected shape modifier.
• Specified shape modifier not allowed — The shape modifier in the prefix is not allowed. Click Update Selected to update the prefix text to the expected value.
• Missing or incorrect pattern member count — The dimension applies to a pattern but the dimension text is either missing or includes an incorrect pattern member count. Click Update Selected to the dimension text to include the correct pattern member count.
• Independency not applicable to dimension — The independency modifier is not applicable to the dimension. Click Update Selected remove the independency modifier from the dimension text.
• Stock size not applicable to dimension — The stock size indication is not applicable to the dimension. Click Update Selected remove the stock size indication from the dimension text.
• Statistical tolerancing modifier not applicable to dimension — The statistical tolerancing modifier is not applicable to the dimension. Click Update Selected remove the statistical tolerancing modifier from the dimension text.
• Dimension text differs from expected value — The dimension text differs from the expected value. Click Update Selected to update the dimension text to the expected value.
• Continuous Feature indication expected — The dimension text should include a continuous feature indication. Click Update Selected to include a continuous feature indication in the dimension text.
• Envelope requirement not applicable to dimension — The Envelope Requirement is not applicable to the dimension. Click Update Selected remove the envelope requirement symbol from the dimension text.
• Dimension is expected to be in decimal format — GD&T Advisor only supports dimensions in decimal format. Click Update Selected to change the dimension to decimal format.
Geometric Tolerances
• Surface references do not match feature references — The CAD annotation surface references do not match the GD&T Advisor feature surface references. Click Update Selected to update the CAD annotation references to match the feature references.
• Shape modifier required — The required shape modifier is missing in tolerance specification. Click Update Selected to update the geometric tolerance to include the expected shape modifier.
• Shape modifier not allowed — The shape modifier in tolerance specification not allowed. Click Update Selected to update the geometric tolerance shape to the expected value.
• Varying tolerance zone not allowed — A varying tolerance zone is not allowed for this geometric tolerance. Click Update Selected to update the geometric tolerance value.
• Material condition modifier not allowed — The specified material condition modifier is not allowed for this geometric tolerance. Click Update Selected to remove the material condition modifier from the geometric tolerance.
• Statistical tolerancing symbol not allowed — The statistical tolerancing symbol is not allowed for this geometric tolerance. Click Update Selected to remove the statistical tolerancing symbol from the geometric tolerance.
• Tangent plane symbol not allowed — The tangent plane symbol is not allowed for this geometric tolerance. Click Update Selected to remove the tangent plane symbol modifier from the geometric tolerance.
• Projected zone not allowed Projected zone is not allowed for this geometric tolerance. Click Update Selected to remove the projected zone specification from the geometric tolerance.
• Unequally disposed zone not allowed — An unequally disposed zone is not allowed for this geometric tolerance. Click Update Selected to remove the unequally disposed zone specification from the geometric tolerance.
• Specified offset not allowed — A specified offset is not allowed for this geometric tolerance. Click Update Selected to remove the specified offset specification from the geometric tolerance.
• Combination specification element required — A combination specification element is required for this geometric tolerance. Click Update Selected to add the default combination specification element to the geometric tolerance. You should review the geometric tolerance that the desired combination specification is indicated.
• Dynamic profile modifier not allowed — The dynamic profile modifier is not allowed for this geometric tolerance. Click Update Selected to remove the dynamic profile modifier from the geometric tolerance.
• DF boundary modifier not allowed — A boundary modifier is not allowed for the specified datum feature. Click Update Selected to remove the DF boundary modifier from the geometric tolerance.
• DF boundary value not allowed — The specified datum feature value is not allowed. Click Update Selected to remove the specified boundary value from the geometric tolerance.
• DF boundary shape modifier not allowed — The specified datum feature shape modifier is not allowed. Click Update Selected to remove the specified boundary shape modifier from the geometric tolerance.
• Required DF boundary shape modifier not specified — The boundary value requires a shape modifier. Click Update Selected to add the required shape modifier to the datum feature boundary value in the geometric tolerance.
• DF translation modifier not allowed — The datum feature translation modifier is not allowed for this geometric tolerance. Click Update Selected to remove the datum feature translation modifier from the geometric tolerance.
• DF material requirement not allowed — The specified material requirement is not allowed for the datum feature. Click Update Selected to remove the datum feature material requirement from the geometric tolerance.
• Composite tolerance segment not allowed — A composite tolerance segment is not allowed for this geometric tolerance. Click Update Selected to remove the composite tolerance segment from the geometric tolerance.
• Indicators not supported in ASME tolerancing standards — Indicators are only applicable to models that reference ISO GPS. Click Update Selected to remove the indicators from the geometric tolerance.
• Unilateral tolerance zone not allowed — The unilateral tolerance zone indication is not supported. Click Update Selected to remove the unilateral tolerance zone indication the geometric tolerance.
• Additional text above differs from expected value — The additional text above the geometric tolerance does not match the expected value. Click Update Selected to update the text above the geometric tolerance to the expected value.
• Additional text to the right differs from expected value — The additional text to the right of the geometric tolerance does not match the expected value. Click Update Selected to update the text to the right of the geometric tolerance to the expected value.
• Tolerance string syntax error — The tolerance string has syntax errors. This problem cannot be fixed automatically. You should edit the tolerance string in the geometric tolerance in the CAD system and then click Refresh List.
• Datum reference string has syntax errors — The datum reference string has syntax errors. This problem cannot be fixed automatically. You should edit the datum reference strings in the geometric tolerance in the CAD system and then click Refresh List.