Creating Angular Dimensions

This task shows you how to create angular dimension annotations.
Remember that:
  • When the dimension supports are related to a parameter (sketch's constraints, knowledge, etc) for which tolerances are still defined, they are set to the dimension tolerances.
Open the Annotations_Part_02.CATPart document:

  1. Click Dimensions  in Annotations toolbar.

  1. Select the surfaces as shown on the part.

    A linear dimension appears during the creation process before you select the second surface.
    The angular dimension appears.
    If the angular dimension does not appear, right-click the dimension and from the contextual menu select Angle.

  1. Right-click the angular dimension and select Angle Sector - > Sector 4 from the contextual menu. 

    The angular dimension is modified.

  1. Click outside any geometry to end the dimension creation process.
Since the Always try to create semantic tolerances and dimensions option has been selected, the dimension has not been set as semantic. This is why the Linear Dimension icon appears in the specification tree and the dimension is created as Dimension.1.
 

  1. Right-click the angular dimension and select Dimension.1 object > Angle Sector - > Sector 1 from the contextual menu.

    The angular dimension sector is modified.
     

If the Always try to create semantic general tolerances and dimensions option has been selected, the dimension is set as semantic. The Angular Size icon is displayed in the specification tree and the angular dimension named Angular Size.1 during the dimension creation process.
 
  1. Select the two surfaces as shown, to create semantic angular dimension.
  2. Click the Tolerancing Advisor in Annotations toolbar.
    The Semantic Tolerancing Advisor dialog box appears.
    The buttons and options available in the dialog box depend on your selection.
     

    The Propagation Selection options are displayed according to the type of face selected depending on the canonicity. In this scenario the options are not used. For more information, refer to Propagating Geometry Selection for Feature Creation.
  3. Click Angle Creation : . The Limit of Size Definition dialog box appears.
     
    The angular dimension dimension is previewed and the Limit of Size Definition dialog box appears, offering the following options:
    • General Tolerance: lets you define a pre-defined class of tolerance, see Tolerances for the default class setting.
       

      • From R18, the standards for general tolerance, ISO 2768-1 (1989) and ANSI B4.3 – 1978 is supported for angular dimensions.

      • If the semantic standard ISO is used, then the Standard field of the Limit of Size Definition dialog box allows you to choose between ISO 2768-f or ISO 2768-m or ISO 2768-c or ISO 2768-v.

      • If the semantic standard ASME is used, then the Standard field will give only one option of ANSI B4.3-1978.

      • According to ISO and ASME standards, only the nominal value of the dimension is displayed in 3D, the tolerance values are not displayed. The numerical values of the general tolerance will be seen without having to edit the dimension through the tooltip text. The angular general tolerance values are displayed through a tooltip in a yellow text box, when the mouse is moved over the dimension, both in the tree and in the 3D.

      • The general tolerance values will always be displayed in degrees/minutes/seconds in the tool tip. The values in millimeters per 100mm and in milliradians as described in the ANSI B4.3-1978 standard are not supported.

      • The general tolerance values of angular dimensions are based on the shortest length of the 2 legs forming the angle. Depending on this shortest length, the tolerance values have been defined for the standards (ISO, ANSI).

      • In this case, you can see that there are three angular dimensions created with different leg lengths.

      You can see that for the same angular value, the tolerance values change depending on the shortest leg length.

      • FTA supports angle dimensions between: a conical face, two non parallel planar faces, a cylindrical and planar face that are neither parallel nor perpendicular, a cylindrical facer perpendicular to parallel face, two cylindrical faces.

      • In case of circular surface, say a planar face (defined by the plane of the circle), then the leg length in this case is the always the diameter of the circle (even if it is only an arc of circle).

    • Numerical values: lets you define the Upper Limit and optionally the Lower Limit (provided you uncheck the Symmetric Lower Limit option).
    • Single limit: lets you enter a minimum or maximum tolerance value. Use the Delta / nominal field to enter a value in relation to the nominal value.
    • Information/Reference: lets you to set the dimension as information (ISO-based standards)/ reference (ASME-based standards). The information/reference dimension is displayed enclosed by parentheses in geometry window.
  4. Click OK. The angle is created.
  5. Click Close or click anywhere geometry window to validate the dimension creation.
  6. The numerical description of the angle can be changed using the Numerical Properties toolbar.
    In this case change it to NUM.ARAD.
    The dimension is updated.
  7. To edit the semantic angular dimension, right-click it and select Angular Size.1 object > Definition.
    The Limit of Size Definition dialog box appears.
    You will see that in the     Numerical values, Upper Limit and Lower Limit, the unit has been changed to rad from min even if the knowledge unit is still Degree, Minute, Second (Tools > Options > General > Parameters and Measures, Units tab).
  8. Change the Upper Limit to 0.005rad. Click OK.
    The dimension is updated.