What's New: 2023
- In a sketch, double-click a dimension or click the Dimension
command in the Constrain panel and then click the dimension.
- In the Edit Dimension dialog box, click the arrow and choose Tolerance from the pop-up menu.
- In the Tolerance dialog box, change either of the following:
- Precision. Choose a decimal-precision value from the pop-up menu.
- Evaluated Size. Specifies the tolerance level of the selected dimension. The default is Nominal (the “actual” dimension, the value which must be adjusted for manufacturing purposes).
Note: The Model Value field shows the selected dimension’s value, for reference. To change the value, close the Tolerance dialog box, double-click the dimension, and enter a different value. - Under Tolerance, choose a Type:
- Default. The dimension does not have a tolerance value.
- Basic. Specifies the theoretically exact value.
- Symmetric. Specifies the same value at the upper and lower tolerance range.
- Deviation. Specifies a different value at the upper and lower tolerance range.
- Limits – Stacked. Displays the maximum and minimum tolerance values in a stack.
- Limits – Linear. Displays minimum values and maximum values side by side separated by a hyphen.
- Max. Displayed as a label on the maximum tolerance value. The upper tolerance is zero and is disabled; the lower tolerance level is any number equal to or greater than zero.
- Min. Displayed as a label on the minimum tolerance value. The lower tolerance is zero and is disabled. The upper tolerance is zero and is disabled; the upper tolerance level is any number equal to or greater than zero.
- Limits and Fits. Used to show tolerances on shafts and holes in addition to tolerances for the part. Nomenclature and tolerances are specified by the standard selected (such as ANSI or ISO) when Autodesk Inventor was installed. Limits are the tolerances for a part; fits are the pair of limits for a pair of mated parts. Stacked and Linear options are available. The Show Size Limits option displays the tolerance limits in parentheses. The Show Tolerances option displays values in parentheses with a plus and minus to indicate the upper and lower tolerances.
Note: In a drawing, model dimensions use the tolerance type. However, you can override the model tolerance type with a drawing dimension style. - If required for the tolerance Type, specify the following:
- Upper, Lower. Sets the value for the upper and lower tolerance. A value with a two-part sign of operation represents a tolerance range. A value with a single sign of operation is either added to or subtracted from the nominal value. If the value has a single sign of operation, click the plus or minus sign to change the sign.
- Hole. Sets the tolerance for the hole dimension when using Limits and Fits tolerance. Click the down arrow to select from the list.
- Shaft. Sets the tolerance value for the shaft dimension when using Limits and Fits tolerance. Click the down arrow to select from the list.
- Click OK.
Note: You can also edit the tolerance of an existing dimension by using the Dimension Properties dialog box. Right-click a dimension, choose Dimension Properties, and change options in the Dimension Settings tab.