About Datum and Datum Target Elements

Datum Concept

Creating and editing datum elements, including datum targets and datums involves understanding datum systems, datum system composition, and writing rules.

Datum Elements and Datum Systems

Datum elements and datum systems are specified only in the case of geometrical tolerancing (not on dimensional tolerancing and except on form tolerancing). You can specify simple datum elements, common datum elements, datum targets, or specified datum systems.

The feature that is assigned a tolerance is positioned relatively to the tolerance zone, and this set is positioned relatively to the datum or the datum system .

These related positions are specified using basic dimensions and are displayed or not displayed.

For more information about datum constitution and specification, see ISO 5459, ASME Y15.5M, and ISO 1101.

Datum System Composition

When the identifiers are specified separately in each frame of the tolerance frame, the datum elements represent a datum system. A hierarchy is established between the datum elements. Reference A is the primary datum and reference B is the secondary datum. The datum system fitting would be performed first on datum A, then on datum B, with respect to A. By the way, a tertiary datum can also be specified.

Datum elements must be fitted successively (following their specification order) with respect to the hierarchy for the measurement computations.

When only one identifier is specified in the tolerance frame, the datum is a single datum.

When two identifiers separated by a dash are specified in the tolerance frame, the datum is a common datum . The two datum elements are to be considered simultaneously. The datum system fitting is performed in the meantime on datum A and on datum B (both datum elements must be fitted simultaneously for measurement computations).

Datum Writing Rules

A capital letter is used to identify the datum element in the tolerance frame. The datum triangle can be filled or nonfilled.

When the datum triangle is placed on the outline of the element or on its extension line, the datum element represents the surface itself or the 2D representation of the surface, which is a line.

When the datum triangle is placed in the alignment of the dimension line, the datum element represents the median element (usually an axis plane or a median plane).

When the datum triangle points directly on a median element, the datum element represents either the median element itself (usually an axis plane or a median plane) or the resulting median element of the collection of the considered elements.

Datum Creation

Feature selection

A datum can be created by selecting:

A geometrical element
Any Part Design or Generative Shape Design feature in the tree. In this case, the created annotation is not attached to the selected feature, but to its geometrical elements at the highest level.

If you select a noncanonical geometry as support, the created datum is invalid because of a lack of information to define the orientation of the datum plane. To avoid this situation:

Edit the invalid datum and define the plane orientation in the Plane Direction box.
Create the datum using the Tolerancing Advisor that recognizes automatically the selected geometry as noncanonical and asks you to define the plane orientation in the Plane Direction box.

Datum Created from Patterns of Features

When a datum is created from a pattern of features, a label Nx appears to the right side of the datum, where N is the number of features the pattern is made of. The label:

Can be moved.
Can be deleted.
Reappears and updates when the datum is modified and updated.
Is invalid if the number of instances in the pattern is changed.
is removed when the standard of a feature is changed from ISO to ASME using the feature properties

Projected Extension Datum Modifier

The Projected extension area is available in the Datum feature dialog box when the datum feature is any of the following:

Thread surface
Extended cylinder construction geometry
Pattern of threads
Pattern of cylindrical holes or pins

At a given time, only one of the Projected extension option or Contacting Feature [CF] option is available for selection. Click any of the options to enable it. The other option is automatically disabled. Clicking the selected option again clears the selection and makes both the options available for selection.

Note: The selection field in the Projected extension area is available for creation or edition of extended cylinders. If the selected datum feature is a pattern:

The elements listed in the selection field correspond to the instances of the pattern in the same order.
You can click Create/Edit to create or edit each extended cylinder separately. You can only create or modify the parameters of the extended cylinder using Extended Cylinder Construction Geometry dialog box. See Creating Extended Cylinder Construction Geometry
The length and offset are never available for selection in the Projected extension area. You can choose to view their value in the DRF.
An error message appears if any of the listed extended cylinders is invalid.

If the selected datum feature is not a pattern:

The selection field is unavailable for selection.
The associated construction geometry is listed, if already available. You can click Create/Edit to create or edit one.
The length and offset are never available for selection in the Projected extension area. You can choose to view their value.

You can select the Show length and offset in DRF option to view length and offset in all the impacted DRFs and geometrical tolerances. The modification is enabled in the 3D area and in the tree. For example, if the length of the extended cylinder is 5mm and that of the offset is 6mm, the label is modified as (P)11-6, where 11 is the sum of the length and the offset, and 6 is the offset. Ensure that the datum with projected extension is always secondary or tertiary datum.

The annotation for the projected extension datum modifier is invalid when the standard of a feature is changed from ISO to ASME using the feature properties.

Theoretically Exact Size

The Theoretically exact size option is selected, by default, at the time of feature creation in the following cases:

Cones
Angular tabs and slots
Patterns of angular tabs and slots

The Theoretically exact size option is not selected, by default, at the time of feature creation in the following cases:

Spheres
Cylindrical pins and holes
Tabs and slots
Rectangular or square pockets, pins, and holes
Patterns of spheres, cylindrical pins and holes, tabs, and slots

At a given time, only one of the Theoretically exact size option or Contacting Feature [CF] option is available for selection.

When the option is selected, a framed basic dimension is created and associated with the datum feature. Clearing the option, deletes the framed dimension.

Note: In the case of a torus, you can choose the following options:

Theoretically exact small-diameter size
Theoretically exact high-diameter size

The annotation for theoretically exact size is invalid when the standard of a feature is changed from ISO to ASME using the feature properties.

Datum Target Creation

Datum targets involve a datum and a context.

When defining a datum on planar or cylindrical surfaces the use of datum targets is optional.
A target element can be a point, a line, a circular or a rectangular surface lying on the datum element. When the datum target is:
- A point, then the circular frame is linked to a cross placed on the surface. Framed dimensions must specify the location of the point.
- A line, then the circular frame is linked to a line placed on the surface. Framed dimensions must define the length and the location of the line.
- An area - squared or circular, the area dimensions are indicated in the upper compartment of the circular frame, or placed outside and connected to the appropriate compartment by a leader line (when there is no sufficient space within the compartment).
The minimum number of targets is defined by the datum depending on whether it is used as primary, secondary, or tertiary datum in a reference frame.
For instance, if the datum feature is a cylinder, the targets may be two nonparallel lines, tangent to the cylinder and perpendicular to its centerline so as to define an equalizing datum (V-type-equalizers).
When the datum element is prismatic or complex, you must use datum targets. In this case when selecting targets, a message indicates the current step of the datum definition.
When the datum is established from datum targets, then the letter identifying the surface is repeated on the right side of the datum indicator followed by the list of numbers identifying the targets (separated by comas).
When there is no sufficient space within the compartment, the dimensions of the datum target area are placed outside the circular frame and connected to the appropriate compartment by a leader line terminated by a dot.

Important:

With the Tolerancing Advisor , when you select:
- A point or a vertex, Point only, Circular or Rectangular options in the Datum Target dialog box are enabled
- A curve or a surface, Point only, Circular or Rectangular options in the Datum Target dialog box are unavailable as the selected element defines the area
With the Annotation Set Creation, naming is controlled according to the related datum. If you select:
- A point or a vertex, both the diameter option and value box in the Datum Target Creation dialog box are available
- A curve or a surface, both the diameter option and the value box in the Datum Target Creation dialog box are unavailable as the selected element defines the area

When you define a square datum target for the datum target point you selected, the datum target size is displayed in 3D using a square symbol.

You can select the Display the size(s) check box. This option enables you to view the sizes:

inside the compartment
outside the compartment


Size displayed inside the compartment	Size displayed outside the compartment

Note: The Display the size(s) check box is unavailable when the selected datum target feature is:

A point and the Point only option is selected.
Neither a rectangular nor a circular face.

Datum and Datum Target Edition

You can edit datums and datum target at any time.

To edit a datum or a datum target, double-click either a datum or a datum target. Alternatively, select Properties from the context menu.

Important:

When the Always try to create semantic general tolerances on dimensions check box is selected under Semantic Control the editing dialog box differs from the creation dialog box. For more information, see Semantic Control in the Native Apps Preferences Guide.

Datum and Datum Target Leaders

This section describes the salient features of the datum and datum target leaders.

Extremity of Datum Target Leaders

A datum target leader can have different types of extremities. The extremity of a leader is decided by the selected datum target feature.


Selected datum feature	Leader extremity	Illustration
Point or vertex	Cross
Curve or wireframe plane	Open arrow
All other cases	Filled circle

Notes:

You can right-click a datum target in the tree and change the associated geometry of the datum feature using Geometry Connection Management. Doing so does not change the type of leader extremity. You can change the extremity manually.
A datum target leader extremity is retained when the standard of a feature is changed from ISO to ASME using the feature properties. It is also true when the standard is changed from ASME to ISO.

Datum Target Indicator for Datums

For datums established using datum targets, an indicating label appears to the right side of the datum.

Note: The label:

Can be moved.
Can be deleted manually.
Reappears and updates when the datum or the datum targets are updated.
is removed when the standard of a feature is changed from ISO to ASME using the feature properties