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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

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:

  3. Complete the specifications by typing tolerance values in the corresponding boxes.
  4. Click the plus sign 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:

    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:

    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.

Step 6 to creating a tolerance

Tolerance with leader:

example of a tolerance with leader

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.

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.

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
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
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 Regardless of feature size, indicates that the feature can be any size within the state limits. RFS
Projected tolerance zone