Dimensioning and Tolerancing a Hole 

This task shows you how to create tolerances in a series using the Tolerancing Advisor.

  1. Click the Tolerancing Advisor in Annotations toolbar.

    The Semantic Tolerancing Advisor dialog box appears.

  2. Select the planar surface as shown.

    The Semantic Tolerancing Advisor dialog box is updated.
    The buttons and options available in the dialog box depend on the selected features and the standard used:
  3. Click Datum Feature (1 Plane): .
    The     Datum Feature dialog box appears.
    The datum specification appears both in the specification tree and in the geometry.
  4. Enter the required letter as an identifier.
    Press the Ctrl key and move the created annotation to place it as required.
  5. Click OK.
    Datum is created.
    The Semantic Datum icon in the Semantic Tolerancing Advisor dialog box is turned to red indicating that this specification is already defined on the feature.
  6. Select the circular hole located at the center as shown.

    The Semantic Tolerancing Advisor dialog box is updated.

  7. Click the Diameter (1 Cylinder): .
    The     Limit of Size Definition dialog box appears.
  8. Select Tabulated values.

    By default, the tabulated value is H7.
    While creating dimensions, the uppercase and the lowercase letters of tabulated values appear based on the selected feature, hole or shaft. You can also enter it manually.

    Press the Ctrl key and drag the created annotation in the geometry to place it as required.
    • If the Propose the last created tolerance values check box is selected under New Size Tolerances Creation in Tools > Options > Mechanical > Functional & Tolerancing Annotations, Tolerances tab, the last tolerance type and values defined for Tabulated values in the previous command are proposed as default for the next command.
    • If you manually enter the lowercase letter for hole and uppercase letter for shaft, the same is proposed as default for the next hole or shaft selection.
    • If you select a vertex or an edge of a feature, default tabulated value is applied.

  9. Click OK.
  10. From the Datum Systems list in the Semantic Tolerancing Advisor dialog box, select the required datum identifier (A in this case) and then select the cylinder dimension.
    The     Semantic Tolerancing Advisor dialog box is updated.
  11. Click the Perpendicularity Specification .
    The     Geometrical Tolerance dialog box appears.
     You can see that the options and modifiers that are relevant to the tolerance type and the features that have been selected are proposed.
  12. Enter the required Numerical value and select the required modifiers.
    The perpendicularity tolerance is automatically grouped with the previously created size tolerance.
  13. Click OK.
    Press the     Ctrl key and move the created annotation in the geometry to place it as required.

  14. Under Two parallel Planes Tolerance Zone, define the definition element:

    • Face: To define the toleranced zone perpendicular to the axis of the toleranced cylinder between selected face and axis.
    • Edge: To define the toleranced zone parallel to the axis of the toleranced cylinder between selected edge and axis.

  15. Click Unselect to clear the remove the defined definition element.

  16. Select the tolerance frame and click Datum Feature (1 plane): in the Semantic Tolerancing Advisor dialog box.
    The     Datum Definition dialog box appears.
    The datum feature specification is automatically grouped to the previously created size tolerance and perpendicularity tolerances. Press the Ctrl key and drag the created annotation in the geometry to place it as required.

  17. Click OK. You can see that datum B is created.

  18. Do not close the Semantic Tolerancing Advisor dialog box to perform the next task.