Creo Elements/Direct Modeling GD&T
USER GUIDE
Contents:
GD&T Advisor's Analysis Capability
GD&T Advisor Suggestions and Tips
GD&T Advisor's Analysis Capability - The
"GD&T" module provides a limited capability for
ensuring valid GD&T creation. GD&T classifies functional
features in the 3D product model by type (e.g. hole/pin, slot/tab or
general surface) and uses this information to provide some guidance to
the user in creating valid GD&T specifications. Complete GD&T checking
is not supported within the GD&T module. This comprehensive
analysis will be offered by a third party application, VSA-GDT. VSA uses
a 5 level categorization for VSA-GDT analysis as follows:
Complete Syntax checking is supported by GD&T
(within Creo Elements/Direct Modeling and performed on all GD&T callouts
in accordance with the ASME Y14.5M - 1994 standard.
Example: the GD&T will give the valid option of a concentricity control when the functional feature has been classified as an axial feature (i.e. hole or pin) and inform the user that this callout requires a datum reference.
The GD&T does not check to
see if the axis of the toleranced feature is concentric with the datum
axis or whether the datum is even an axial feature. VSA-GDT analysis
provides complete coverage in this area.
Example: the GD&T informs the user that the zone size of the orientation callout must be greater than the zone size of the flatness callout when a flatness (explicit form control) and a parallelism (explicit orientation control, implicit form control) callout are applied to the same planar functional feature.
The GD&T does not check
to see if the user has applied an explicit location control to this functional
feature. VSA-GDT analysis provides complete coverage in this area.
No Network Analysis is performed by Creo Elements/Direct Modeling. VSA-GDT analysis will cover this area.
No Functional Analysis is performed by Creo Elements/Direct Modeling. VSA-GDT analysis will cover this area.
Main Menu - GD&T
Creo Elements/Direct Modeling->Document 3D->GD&T
Note This module is also part of the Advanced Design Module, that comprises all Legacy Modules into one module.
Create
Tolerances - Tolerances include all GD&T symbols. These tolerances will be placed on a selected feature of the current part.
Datums - Allows both simple and complex datums to be defined on the current part. The creation of datums is required prior to the creation of tolerances that require a datum reference.
Edit
Modify GDT - Allows for the modification of any tolerances or datums that were created though the create process.
NOTE: When modifing tolerances, this option will only allow for the modification of tolerance details and not fundamental characteristics such as the functional feature attachment and tolerance type. If changes in these characteristics are required then delete and recreate the tolerance (applies to the Modify Tolerance or Modify Datum dialogs).
NOTE: When Modifying Datums, it is advisable to update all tolerances which reference this datum. This is done automatically if the "Update Refs" button is pressed.
Delete GDT - Allows for the deletion of any tolerances or datums that were created.
NOTE: Since some tolerances reference datums, deleting a datum in this case will result in the invalidation or if possible modification of the tolerance information.
Display
Report - This option will use the standard Design Info report generation utility to produce a HTML based report for all or part of the GD&T information on a part. This report information can then be used for down stream design and manufacturing activities.
Highlight - This option uses the standard Design Info functionality to highlight all or part of the GD&T information found on a part.
Show - This option uses the standard Design Info functionality to show all or part of the GD&T information found on a part.
Properties - This option brings up the standard Design Info label properties utilities.
Tolerance Dialog - This is the first step in creating a new tolerance. This dialog is only shown on the creation of a new tolerance.
Elements - Specify an element or list of elements for a new tolerance specification to be added to the model. Where no functional feature exists for the current element selection, a functional feature will be created and maintained automatically by GD&T. Functional features created this way are also deleted automatically when a datum and/or all tolerances which reference the functional feature have been deleted. GD&T will internally map the tolerance definition to the functional feature and determine which tolerance options will be available in the Valid Types section.
Tol Type - A display only field that provides a text description of the GD&T characteristic symbol shown in the Valid Types field.
Valid Types - Select the desired tolerance type from the options provided. The options available depend on the class of face selected above. Reference material on the GD&T symbols can be found in the Symbol Library. Once the tolerance type has been defined then select the OK button to go onto the Tolerance Details dialog.
NOTE: If the tolerance type requires 1 or more datums and there are no datums currently defined on the part then those tolerance types will not be shown.
Tolerance Details Dialog - This dialog will have the title of the tolerance type that is being created or edited. This dialog is shown as the second step in the tolerance creation process or by the Modify GDT button when a tolerance is specified.
The following is a list of all options found on the tolerance details dialog. The options shown to the user depends on the tolerance type.
Zone Shape - Specify a sperical or clindrical zone shape as needed. (available only for spherical and cylindrical faces)
Zone Size - Enter a numeric value for the zone size. For composite tolerances the hierarchy of tolerances may limit the size of this value. The unit of this distance are those of the current session.
Modifiers - Specify the any zone modifiers that apply. Possible
options include 
.
Zero Tolerance at L/MMC
Max Dev - Defines the maximum allowable bonus tolerance. This restricts
the available bonus tolerance available from the use of Zero Tolerance
at LMC or MMC.
Advanced Options - Expands the dialog for advanced applications
Add'l Mods - If available, this will allow the user to specify
a tangent plane 
-
Defines a free state condition. The user will be prompted to provide a
free state note that will need to describe the nature of the application
of this modifier.
Projected Zone
Proj Zone - Enter a numeric value for the distance of the projected
zone. The units of this distance are those of the current session. The
direction of the zone is defined by the most primary datum on the datum
reference that also geometrically intersects the toleranced face(s).
Inspecton Info
Identifiers - Will bring up a table of dimension
critical identifiers. The options available are configurable by the software
administrator.
Selecting and De-selecting an Identifier - To associate a dimension critical identifier with the tolerance being specified click on the identifier description (de-select by pressing the "CTRL" key and click on the identifier description).
Help - To view an HTML based description of the identifier (if available), highlight the identifier and select the help button.
Apply - Select when all applicable identifiers have been turned on and the identifiers turned on will be applied to the feature or features being toleranced.
Cancel - Selecting this option will return the user the tolerance details dialog without registering any changes made in the identifier table .
Insp Notes - Brings up the inspection notes editor. These notes will not appear directly on the 3D model as a label. Additional utilities will need to be employed to view this information or send it to the 2D drawing for annotations. When the notes are complete select the Done button to apply the notes to the curent tolerance.
Datums - Brings up the Datum Reference Dialog. This dialog is used to specify datums in an order of precedence to properly position the part in a datum reference frame - a framework of three mutually perpendicular intersecting planes established by datum features on the part.
Primary - Select the primary datum feature from the part.
Modifiers - This option is enabled only after a datum is specified and allows the user to specify any desired modifiers. Only datums which are features of size allow modifiers.
Secondary - Select the secondary datum from the part.
Tertiary - Select the tertiary datum feature from the part.
Fixed Text - Brings up the Feature Control Frame (FCF) Fixed Text dialog. This dialog is used to specify the text that will appear above and below the feature control frame. This text will be shown with the FCF on the 3D label.
Superfix - Enter the text as desired for placement above the FCF. Not commonly used
NOTE: Size related information must be entered as a separate tolerance info on the same functional feature.
Subfix - Enter the text as desired for placement above the FCF. Text commonly found here includes the Between symbol, "ALL AROUND" and "4 PLACES"
Elements - Specify an element or list of elements for a new datum definition to be added to the model. Where no functional feature exists for the current element selection, a functional feature will be created and maintained automatically by GD&T. Functional features created this way are also deleted automatically when the datum and/or all tolerances which reference the functional feature have been deleted. GD&T will internally map the datum definition to the functional feature and determine a datum type.
Datum Type - A display only field that provides information to the user on the resultant datum type established from the element or elements selected. The following is a list of datum types classified according to:
Datum features not subject to size variation:
Plane
Complex (given any non-analytic or irregular surfaces)
Datum features subject to size variation:
Axial (given a cylinder)
Center Plane or Width (given a set of two opposed parallel planes)
Center Point (given a sphere)
Identifier - Enter a valid identifier for the datum. If the identifier entered is invalid an error message will appear. The identifier will default to the next available valid identifier.
Update Refs- When modifying datum information (e.g. changing the Identifier) and upon pressing the "OK" button GD&T will automatically update all tolerances which reference this datum.
NOTE: This option is disabled during creation of a datum.
The term Functional Feature is used to distinguish the features used in the definition of part function, inspection, and/or assembly from any other feature in Creo Elements/Direct Modeling. Functional features consist of a specified grouping of one or more surfaces (faces) or a group of two or more functional features called a Pattern Functional Feature. Functional Feature Points are features that can be applied to vertecies of faces with functional features. They are useful in measurment operations between parts/assemblies. Feature points are planned to be extended to support datum target definitions in the future.
When creating a datum or tolerance on the model and no functional features are currently defined for the selection, GD&T internally maps the tolernace or datum to an implicit functional feature that is created "on-the-fly." Functional features created this way are also deleted by GD&T automatically when a datum and/or all tolerances that reference the functional feature have been deleted.
NOTE: There must only be one feature pointing to any one face. All other features that are attached to the face are actually attached through this feature. Generally this feature is created automatically with the creation of a datum or tolerance, however explicit features can also be used in this capacity.
However, some users prefer to create their functional features in an "explicit modeling mode." In this case, the functional feature menu allows you the flexibility to specify and group functional features into patterns. An example of this case is the GD&T requirement of a pattern before a position or profile tolerance can become a composite.
Creo Elements/Direct Modeling->Design Info->Create->Functional Feature
Faces - Select a face or list of faces (not already part of a functional feature) to be used to specify a functional feature.
Features - Select two or more functional features to be used to specify a pattern functional feature. If a face is chosen which is not already a functional feature it will be ignored by GD&T. If a functional feature is chosen which is already a member of a pattern an error will be displayed and the selection will be ignored.
NOTE: The tolerances on the functional features chosen to be members of a pattern functional feature do not apply to the pattern functional feature, you must create them on the pattern.
Name - Specify the functional feature's name. This name will appear as a label attached to the first face or functional feature selected and is viewable from within the Structure Browser.
Descr - Specify a description for this functional feature.
GD&T Advisor Suggestions and Tips