Creating Geometrical Tolerances

You can create annotations with geometrical tolerances.

This scenario illustrates the creation of a geometrical tolerance by selecting geometry. You can also select any Part Design or Generative Shape Design feature in the tree.

In this case, the created annotation will not be attached to the selected feature, but to its geometrical elements at the highest level

Before you begin: Open an existing 3D shape.
See Also
Principles and Fundamental Rules
Definition
Symbols for Geometrical Tolerances
Symbols for Modifiers
  1. Select the Front View.x annotation plane.
  2. From the Annotation section of the action bar, click Geometrical Tolerance .
  3. Select the required face.

    The Geometrical Tolerance dialog box appears.

    This dialog box allows you to:

    • Specify as many specification lines as you want (with the Up and Down arrows).
    • Insert several modifiers anywhere in a tolerance or a reference.
    • Add notes upper and lower the set of specification.

    Notes:
    • At this step, you can apply the parameter values of an existing geometric tolerance to the tolerance you are creating: to do this, select the existing geometric tolerance.
    • If you have selected the Use style values to create new objects check box in Me > Preferences > App Preferences > 3D Modeling > Mechanical Systems > Drafting > Administration expander, the Geometrical Tolerance dialog box is automatically completed with custom style values (as defined in the Standards Editor). In this case, properties in the Object Properties panel and the Tools Palette are not available during the creation of the geometrical tolerance.

      If you have not selected this option, the Geometrical Tolerance dialog box is automatically completed with the last entered values (if any). In this case, properties in the Object Properties panel and the Tools Palette are active during the creation of the geometrical tolerance.

    • You can reset the current style values in the Geometrical Tolerance dialog box at any time by clicking Reset.
  4. In the Geometrical Tolerance dialog box, perform the following operations:
    1. Under Add Tolerance, click the required tolerance indicator to add it to the current feature.

      You can add as many tolerances as required.

      The tolerance indicator is added below the previous one in a separate line. Each line is represented by tabs in the Edit Tolerance section.
    2. Under Edit Tolerance, select the tolerance indicator.

      You can select the Remove Line check box to remove the selected line. This option is unavailable if the selected tolerance line is the only one.

    3. In the Edit Tolerance box, enter the tolerance value.
    4. In the Reference boxes, add references.

      You can add multiple references.

      Tip: Click datum systems and datum to expand the list of the existing datum features and datum systems.
    5. Select an engineering symbol.
    6. In the Auxiliary Feature Indicators list, select a local indicator.

      You can select the following local indicators:

      • Intersection Plane: Identifies a line on an extracted surface or a point on an extracted line. It is placed to the right of the tolerance indicator as its extension.
      • Orientation Plane: Identifies the orientation of the tolerance zone. It is placed to the right of the tolerance indicator as its extension.
      • Collection Plane: Identifies a closed compound contiguous feature. It is placed to the right of the tolerance indicator after the tolerance frame. It can be parallel to the projection plane in which the specification is indicated.
      • Direction Feature: Identifies the direction of the width of the tolerance zone. The direction feature is a cone, a cylinder, or a plane constructed from the datum or datum system indicated in the second compartment of the direction feature indicator. The geometry of the direction feature depends on the geometry of the tolerance feature. It is placed to the right of the tolerance indicator as its extension.
      Note: You can add maximum three non-identical local identifiers for a single tolerance.

    7. In the Auxiliary Feature Text Indicator box, add an indication text.

      You can also select engineering symbols.

    8. In the Global Text Indicators boxes, add an upper and a lower text.

      You can also select engineering symbols.

      You can add new 3D leaders in the 3D area or switch current 2D leaders to 3D to position the leader outside the annotation plane. For more information, see Adding a 3D Leader.

  5. Click OK to accept the values or Reset to clear all values.
    The geometrical tolerancing annotation is attached to the part.



    The geometrical tolerance entity (identified as Geometrical Tolerance.xxx) is added to the tree under the Geometrical Tolerances node.