Geometric Tolerance

Often associated with datum, use Geometric tolerance to create and place basic dimension notations in the drawing, like this:

example of the result of using Geometric Tolerance tool

Video example: Datums and geometric tolerances

Video transcript

Datums and Geometric tolerances are an integral part of communicating manufacturing variation within a drawing.

Add a Datum to the drawing. Stay in the Datum tab to quickly place datums along drawing view edges. The Label field automatically populates with a letter, but it is customizable. Click a view edge to attach the Datum symbol with a leader. Click again to place it. The tool stays active for continuous placement of additional symbols.

Click the Datum target tab to define a specific area to apply another datum. In the Target area dropdown, select a shape. In the Style dropdown, select a callout. Check Area size to specify the target shape. A diameter defines the size of an X, Point, or Circle, while the size of a Rectangle is defined by side lengths. Select the precision from the dropdown. Enter a value for Diameter. Click a view location to attach the symbol. Click again to place it.

Accept the dialog or choose to add dimensions using Targets. Use the Origin target location when there is a vertex where the X and Y axis intersects, or define the X and Y directions by selecting edges in the view. Click the X and Y opposite direction arrows to flip the dimension placement. Accept the Datum.

Reposition by selecting the grip points at the base or dragging the end. Edit from its right-click context menu or double left-click.

Add a Geometric tolerance. Select the tolerance Symbol, enter the tolerance, and input any needed Datums. Insert a Leader, add Symbols, and add Geometric tolerance modifiers such as maximum material condition. Select any combination of Free state, Tangent plane, or Projected tolerance zone.

Add additional frames by clicking the Add frames icon. Successive frames provide a new option in the Symbols dropdown for Composite. This spans the Symbol across both frames. Remove extra frames by clicking the Remove last frame icon.

Click anywhere on the sheet or click a dimension to place the Geometric tolerance. Continue placing additional Geometric tolerances or accept the dialog. When placed on a dimension, it is snapped to the dimension, following it when moved. Drag a Geometric tolerance off a dimension to unsnap it. Drag it on a dimension to snap it.

Edit a Geometric tolerance from its right-click context menu or double left-click to open the edit dialog.

Creating a tolerance

Tolerances can be attached to edges, holes, dimensions (with or without leaders), dimension extension lines, extension lines, surface regions, and even away from an edge (with no leader).

Creating a tolerance:

Click .
In the dialog, from corresponding lists, specify the symbols and associated tolerances for your drawing:
Complete the specifications by entering the following information:
1. The upper text field adds information above the Geometric tolerance.
2. Select the type of Geometric tolerance by using the Symbol dropdown. The symbol is placed to the left of the Tolerance.
3. Enter a Tolerance value into the Tolerance field.
4. Enter up to 3 datum values into the 3 datum fields.
5. Enter a Prefix or Suffix to add information to the left or right of the Tolerance, respectively.
6. Click the Add frame icon () to add additional frames to the geometric tolerance. Change the bottom symbol to Composite to create a composite frame.
7. If desired, click the Remove last frame icon () to remove the last frame added.
8. Click the Leader symbol dropdown and select Leader (), All around (), or All over ().
9. Click the Geometric tolerance symbol dropdown to select the type of Geometric tolerance. The symbol displays to the left of the Geometric tolerance value in the Tolerance field.
10. Click the Geometric tolerance modifier dropdown and select Maximum material condition (), Least material condition (), or Regardless of feature size (). The symbol displays to the right of the Geometric tolerance value in the Tolerance field.
11. Select any combination of Free state (), Tangent plane (), or Projected tolerance zone (℗). The symbol displays to the right of the Geometric tolerance and Geometric tolerance modifier in the Tolerance field.
12. Enter information in the Lower text field below the leader to add information below the Geometric tolerance.
13. The Insert symbol dropdown at the bottom left of the dialog is used to insert a symbols to the upper and lower text fields, as well as the Prefix and Suffix fields. Place your cursor in the field where you want the symbol placed, and then use the dropdown to select the symbol to insert.
Click in the graphics area to place the tolerance.
To place tolerance with a leader, hover over drawing view until a snap point appears, click with the desired snap point visible, drag tolerance and click to place. To add another leader, right-click the leader and select Add leader. Click to place additional leader. Repeat to add more leaders:
The leader includes a moveable node along the horizontal segment:

Click and drag the node to extend or shrink the horizontal segment of the leader line.
To place the tolerance on an edge in the view, place the tolerance first, then drag it to the edge and release when there is no leader visible:

To place the tolerance along an extension line, drag the tolerance away from the snap point, until an extension line appears:
To place the tolerance on a surface region, click at the surface location and drag the tolerance to the desired location:
You can also place tolerances on centermarks as well as manually placed centermarks.
When aligning dimensions and annotations, you can hover over edges, midpoints, or other lines to activate red inference points. Use the inference points to snap the location of the entity when creating or dragging a dimension or annotation. Similarly, you can move the mouse vertically or horizontally over views, lines, dimensions, or annotations to activate pink vertical and horizontal inference lines. Use these inference lines to align the location of the entity vertically or horizontally from the desired referenced annotation.

The tolerance displays in the graphics area.

Tolerance displayed in the graphics area

Tolerance with leader:

example of a tolerance with leader

You can drag a geometric tolerance closer to or farther away from its placement point on the drawing, and the extension line adjusts appropriately. You also have the ability to attach and orient the geometric tolerance to other drawing annotations.

When dragging away from a dimension, the geometric tolerance automatically gains a leader and remains inline with the dimension.

Grouping tolerances

Editing a tolerance

To edit a tolerance:

Double-click on the tolerance in the graphics area.
Make your changes in the dialog that opens.

Styling tolerances

To style a tolerance:

Click on the tolerance you want to style, then click the Styles panel icon on the right side of the page:
Edit the Font, Text height, Color, and Arrowhead:

Add/remove leader nodes

Right-click on the leader and click Add node:

A node will appear on the leader. To add another node, right click on the leader and select Add node again.

To remove a node from a leader, right click on the node and select Remove node.
You are also able to add leaders to nodes by right clicking on the node and selecting Add leader. This will add a leader starting from that node and ending wherever you click next.