Creating Datum Targets 

This task shows you how to specify datum targets on datum elements.
Before performing the task, here are a few principles you should be familiar with:
  • When defining a datum on planar or cylindrical surfaces the use of datum targets is optional.
  • A target element can be a point, line, circular or 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 shall define the location of the point.
    •  When the datum target is a line, then the circular frame is linked to a line placed on the surface. Framed dimensions shall define the length and the location of the line.
    • When the datum target area is square 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).

  • If the datum target is created on a point geometry then you can specify the form (point, circle and rectangle) and the size of the limited zone. Otherwise the options are disabled.

  • 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 non-parallel lines, tangent to the cylinder and perpendicular to its centerline, in order to define "equalizing" datum ("V-type-equalizers").
  • If the datum element is prismatic or complex, the use of datum targets is mandatory. 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.
Open the Annotations_Part_04.CATPart document:

  1. Activate the Front View.1 annotation plane.

  2. Click Datum Target in Annotations toolbar.

  1. Select the face as shown (It is defined as datum plane D).

    The Datum Target Creation dialog box appears.
     

    The Tools Palette is displayed according to the type of face selected depending on the canonicity. In this scenario the Tools Palette is not used. For more information, refer to Propagating Geometry Selection for Feature Creation.

 		 This scenario illustrates the creation of a datum target by selecting geometry, but you can also select any Part Design or Generative Shape Design feature in the specification tree. In this case, the created annotation will not be attached to the selected feature, but to its geometrical elements at the highest level.
 

  1. Click the diameter icon in the Datum Target Creation dialog box, enter 8 in the field opposite, enter D1 in the field to the left.

  2. Click OK to validate.

    You have created a datum target on datum plane D. The datum target corresponds to a 8mm-diameter surface. Its name is "D1" and it is identified as "Datum Target..xxx" in the specification tree.
 

The Semantic Up-gradation of the Non-Semantic Datum Target

  1. Select the option Always try to create semantic tolerance and dimensions, in Tools > Options > Mechanical Design > Functional Tolerancing & Annotation > Tolerancing tab, Semantic Control area.

  1. Click Datum Target in Annotations toolbar.

  1. The Datum Target Creation dialog box appears. Select the geometry (which should be inside the geometry referenced by the datum feature). .

  2. Add required values in the dialog box.

  3. Click OK to validate.
When non-semantic target is upgraded to semantic, the datum target representation updates itself according to the selected geometry.
  • If the selected geometry is a point, Ø10 appears in the datum representation.
  • If the selected geometry is a curve or a surface, the specified form size disappears as the selected curve or surface itself defines the form and size of the limited zone.
 

Change of the Target Geometry Using the Geometry Reconnect Command

When the geometry of the semantic datum target is reconnected using geometry reconnection command, if the datum target is connected on a curve or surface and the target has form defined with itself and the datum target is semantic KO.

If the old semantic datum target has been created with curve or surface and target has form defined with itself then datum target will be semantic KO after the part is updated on latest level.

The KO datum target will have following diagnostic report:

The KO annotation can be corrected by edition or recreation.