Making the Most of Model Tolerances

30 Jun, 2003 By: Jeff Wymer

Autodesk Inventor's model tolerances allow you to define tolerances at the part level, which controls a model's size based on its tolerances. The model tolerances defined at the model level can be extracted and documented in the drawing environment automatically. In this column we'll cover how to set up model tolerances, update your model to specific tolerances, and document these tolerances at the drawing level.

Getting Started

As shown in Figure 1, you can apply tolerance settings in the Tolerance dialog box, which is accessible from the Dimension dialog box in model mode or in a drawing view. You can access the Tolerance dialog box for feature parameters (such as extrusion extents or shell thickness) in the Parameters dialog box. You can also use the Parameters dialog box to quickly review and edit dimension values, feature parameters, and tolerance settings for every model dimension and feature parameter in the entire part, as shown in Figure 2.

Figure 1. The Tolerance dialog box allows you to quickly define model toleranes and set the evaluated dimension value to the upper/nominal/lower values

Figure 2. The Parameters dialog box lets you quickly review and edit dimension values, feature parameters, and tolerance settings for every model dimension and feature parameter.

Model Tolerances for Sketch Dimensions

You can define model tolerances when editing the dimensions of a sketch or part-editing dimensions. When the Edit Dimension dialog box appears, right-click and select Tolerance. The Tolerance dialog box will now appear. Here you can set the precision of the tolerance and the tolerance type. You can set how the model evaluates the tolerance (for instance, evaluate the dimension to the upper/lower/nominal tolerance value) during model creation or updates. This is useful for simulating what-if design scenarios to understand the impact of the tolerances on the model and mating components in the assembly.

Model Tolerances for Feature Parameters

Model tolerances can be accessed and defined on all feature parameters by accessing the Parameters dialog box from the Tools pulldown and Parameters option. Here you can right-click the equation from the feature parameter's equation and choose "Tolerance..." from the context menu. This will access the same tolerance dialog box used when editing dimensions previously defined in Model Tolerances for Sketch Dimensions. You can now adjust parameter tolerance settings in the dialog box and click OK to incorporate all of the changes.

In the Parameters dialog box, you can easily specify whether the dimension is evaluated at the positive or negative tolerance setting. Simply select the tolerance cell and a pulldown list will appear, allowing you set the specific parameter to the upper/nominal/lower tolerance setting. You can also set the entire model to be at its upper/nominal/lower tolerance setting in one step by using the Reset Tolerance option in the Parameters dialog box. To review the model at the evaluated sizes for all dimensions and parameters, update the model using the Local Update icon.

Predefining Tolerance Values

A company standard usually establishes the allowable tolerance for dimensions. You can set up your company standards as defaults in Document Settings, as shown in Figure 3, and specify standard tolerances based on the number of decimal places defined. This can be set up and saved in a template file for easy access and reuse. To access it, select the Tools pulldown menu and select the Document Settings options and choose the Default Tolerance tab. The Use Standard Tolerance Value option allows the model to use the predefined tolerance settings defined in the dialog. If no values are provided (default) you can define the tolerances based on the number of decimal places you enter. To automatically retrieve the tolerances defined during modeling in drawings, use the Export Standard Tolerance Values option.

Figure 3. The options in Document Settings are useful for specifying company standards.

When editing the tolerances of the sketch and model dimensions the tolerances will automatically be set based on the settings predefined in documents settings. This option is only available when using the default tolerance type. Any tolerance type setting other than default will override the predefined settings.

Retrieving Tolerances in Drawings

The tolerances defined at the model level can be retrieved automatically in the drawing. This will ensure that there is no miscommunication between designing and documenting. To retrieve the model tolerances and dimensions, use the Get Model Annotations option in the drawings. The model dimension and tolerance can be changed from the drawing by using the edit model dimension and the tolerance option from editing dimensions. This change is fully associative with the model; therefore, any changes made at the drawing level will be reflected at the model level.

Figure 4. Here is a view of the model with tolerances applied and displayed at the part level.


In Autodesk Inventor, you can select standard limits and fits or specify custom tolerance values for sketch dimensions and features. After selecting the type of tolerance and specifying the upper and lower limits, you can choose whether the evaluated size will be the Nominal, Upper, or Lower limit. The model can then be set to the evaluated size to check specific fit conditions or for exporting 3D data with all dimensions set to the appropriate condition for manufacturing (such as nominal for a machined part). You can do what-if design scenarios to analyze the impact of tolerances on you designs and make appropriate design changes to decrease costly errors and mistakes during manufacturing and assembly.