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Feature Toolbar with Geometric Tolerance Icon Highlighted

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

Creating a tolerance

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

Creating a tolerance:

  1. Click Geometric tolerance icon.
  2. In the dialog, from corresponding lists, specify the symbols and associated tolerances for your drawing:

    Example of entering a tolerance in the Geometric tolerance dialog

  3. Complete the specifications by typing tolerance values in the corresponding boxes.
  4. Click the plus sign Plus sign icon to add additional frames to the geometric tolerance. Change the bottom symbol to Composite to create a composite frame.
  5. If desired, click the minus sign Minus sign icon to remove the last frame added.
  6. Include additional information to be displayed beside the tolerance information, if desired.
  7. Use the text box to provide text to accompany the tolerance, if desired.
  8. 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:
    Placing a tolerance with a leader
    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:
    Placing a tolerance on an edge in the view
    To place the tolerance along an extension line, drag the tolerance away from the snap point, until an extension line appears:
    Placing a tolerance along an extension line
    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

Grouping a tolerance with more information:

Example of grouping a tolerance with more information

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 a tolerance to an annotation

To group a tolerance to an annotation, for example, a dimension or hole callout:

  1. Click to select the tolerance.

  2. Drag the tolerance to an existing dimension. When the dimension gains a highlight, release the drag.

To group a tolerance during creation:

  1. Once the tolerance dialog is open, make your necessary changes in the dialog.
  2. When placing the tolerance in the drawing area, click on the dimension you wish to group it with.

When you move a tolerance, the tolerance is ungrouped.

To move them both together, click and drag the dimension to the new location. To move the tolerance, click and drag it to a new location.

Moving the tolerance breaks the group connection between it and the dimension. To regroup it, drag and drop the tolerance on the dimension.

Grouping a tolerance to a callout group

To group a tolerance to a dimension that has a grouped callout, for an example, a dimension with a balloon callout grouped with it:

  1. Click to select the tolerance.
  2. Drag the tolerance to the existing dimension. When the dimension gains a highlight, release the drag.

To group a tolerance during creation:

  1. Once the tolerance dialog is open, make your necessary changes in the dialog.
  2. When placing the tolerance in the drawing area, click on the dimension.

To move the callout group together, click and drag the dimension to the new location. Alternately, click on the tolerance or callout to select it. Then click anywhere outside the grip point (shown by the cursor below) to move the entities together to a new location.

Example of moving the callout group together

To move the tolerance without moving the group, click to select it. Then click its grip point and move it to a new location. The tolerance remains part of the callout group, even after it is moved to the new location.

Editing a tolerance

To edit a tolerance:

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

Styling tolerances

To style a tolerance:

  1. Click on the tolerance you want to style, then click the Styles panel icon on the right side of the page:

    Drawings styles panel icon

  2. Edit the Font, Text height, Color, and Arrowhead:

    Drawings Styles panel

Add/remove leader nodes:

  1. Right-click on the leader and click Add node:

    Screenshot of Add node command selected in context menu

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

  1. To remove a node from a leader, right click on the node and select Remove node.
  2. 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.

Geometric characteristic symbols

Symbol Characteristics Type
Position symbol Position Location
Concentricity or coaxiality symbol Concentricity or coaxiality Location
Symmetry symbol Symmetry Location
Parallelism symbol Parallelism Orientation
Perpendicularity symbol Perpendicularity Orientation
Angularity symbol Angularity Orientation
Cylindricity symbol Cylindricity Form
Flatness symbol Flatness Form
Circularity or roundness symbol Circularity or roundness Form
Straightness symbol Straightness Form
Square symbol Square Form
Profile of a surface symbol Profile of a surface Profile
Profile of a line symbol Profile of a line Profile
Circular runout symbol Circular runout Runout
Total runout symbol Total runout Runout

Leader symbols

Symbol Characteristics
Leader symbol Leader
All around symbol All around
All over symbol All over

Diameter symbols

Symbol Characteristics
Ø Diameter
SØ Spherical diameter
R Radius
SR Spherical radius
CR Controlled radius

Modifier symbols

Symbol Characteristics Type
indicates a feature contains the maximum amount of material stated in the limits At maximum material condition, a feature contains the maximum amount of material stated in the limits MMC
indicates a feature contains the minimum amount of material stated in the limits At least material condition, a feature contains the minimum amount of material stated in the limits. LMC
indicates that the feature can be any size within the state limits Regardless of feature size, indicates that the feature can be any size within the state limits. RFS
Free state symbol Free state F
Tangent plane symbol Tangent plane T
indicates that the feature can be any size within the state limits Unequally disposed profile/Unilateral tolerance. Specifies the amount of material out of the total tolerance that is added to the part.  
℗ Projected tolerance zone  
Statistical tolerance icon Statistical tolerance. Indicates tolerances to related assembly components based on sound statistics.  
Translation icon Translation. Indicates that a datum feature simulator is not fixed at its basic location and shall be free to translate.