Geometric Tolerancing

The geometric tolerance symbol adds geometric tolerances to parts and drawings using feature control frames. The SolidWorks software supports the ANSI Y14.5 Geometric and True Position Tolerancing guidelines.

• You can place geometric tolerancing symbols, with or without leaders, anywhere in a drawing, part, assembly, or sketch, and you can attach a symbol anywhere on a dimension line.
  
  

• The Properties dialog box for geometric tolerance symbols offers selections based on the symbol you choose. Only the attributes that are appropriate for the selected symbol are available.

• A geometric tolerance symbol can have any number of frames.

• The pointer changes to when it is on a geometric tolerancing symbol.

• You can add multiple symbols without closing the dialog box.

• You can display multiple leaders.

• You can add more leaders to an existing symbol by holding down Ctrl and dragging a leader attachment point.

• To edit an existing symbol, double-click the symbol, or right-click the symbol and select Properties.

• When you drag the leader of a geometric tolerance symbol off a model edge, an automatic witness line is created.

To create geometric tolerancing symbols:

1. Do one of the following:

   • For parts, click Geometric Tolerance ( DimXpert toolbar) or Tools, DimXpert, Geometric Tolerance. See DimXpert for Parts Overview.

   • For drawings, click Geometric Tolerance (Annotation toolbar) or Insert, Annotations, Geometric Tolerance.

2. Set options in the Properties dialog box and the Geometric Tolerance PropertyManager.
   
   As you add items, a preview is displayed.

3. Click to place the symbol.

   • Click as many times as necessary to place multiple copies.

   • If the symbol has a leader, click once to place the leader, then click a second time to place the symbol.

When you insert geometric tolerance symbols that use Auto Leader , you must hover over the entity to highlight the entity and to attach the leader. The leader does not appear until you hover over the entity.

4. Click OK.

To attach geometric tolerance symbols to dimensions:

1. Create a geometric tolerance symbol.

2. Drag and drop the symbol onto a dimension.
   
   If you move the symbol after attaching it to a dimension, you can drag it outside the dimension.

To detach geometric tolerance symbols from dimensions:

1. Select the geometric tolerance symbol.

2. Click the symbol handle, then drag the symbol away from the dimension.
   
   

To create an unattached geometric tolerance symbol from a symbol attached to a dimension:

Press Ctrl and drag the attached symbol to another area.

Related Topics

DimXpert Auto Dimension Scheme PropertyManager

DimXpert Geometric Tolerance Options