Autodesk Inventor – Dimension tolerances

By Chris Smith

Introduction

When designing our products, it may be necessary to add finer control to the sizes of features in our model to ensure proper functionality of our design. All engineering designs need dimensions to pass the design intent on to the manufacturer to allow them to make the product efficiently and cost effectively.

By adding tolerances to our design we can -

• Ensure that the manufacturing process can be completed easily and at reasonable cost.
• Ensure the proper fit of our designed components.
• Control the precise placement of feature positions.
• Reduce overall rework cost of non-compliant parts.

Tolerances are an essential part of good engineering design, and with Autodesk Inventor it has never been easier to apply dimensional tolerancing to models. In this blog we will look at how you too can apply tolerances to your designs.

Generic tolerances

Below is a simple model of a small plate with a cut out and some hole features. I have shown the first sketch that is used to create the plate to show the current dimensional inputs.

These sizes may not have much of an effect on our product, but we still should apply a general tolerance to them to ensure clear instructions to the manufacturer. All technical drawings should show a general dimension tolerance scheme, and this allows the designer to create designs without spending additional time applying tolerances to each dimension.

To apply general tolerances to a model we need to edit the document properties. This option can be found on the Tools ribbon.

Opening the document settings and selecting the Default Tolerance tab, we can start to add our default tolerance values. You can see from the image below that I have already created my standard tolerance and saved the values to my template file to apply these values to all the models I create. The values below mean that:

1. All linear dimensions with a precision of one decimal place with have a general tolerance of +/- 0.5mm
2. All angular dimensions with a precision of one decimal place with have a general tolerance of +/- 0.5o

You can apply additional tolerances by clicking the “Click here to add” option.

To add an additional tolerance, select the precision value from the list on the left, and input the tolerance value on the right (as above).

The sketch below shows the initial dimensions. None of the default tolerances have been applied at this time as the default tolerance precision is set to 3 decimal places.

To modify the tolerances, we have a few options.

Right clicking on a dimension in Autodesk Inventor will open the context menu which will give the option to edit the dimension properties.

From the Dimension Properties tool window, we can apply properties to our dimension. Here we can apply our tolerance precision to automatically apply our general tolerance. Note that the tolerance type is set to default to denote the default general tolerance.

Clicking ok on the tool window applies the precision value, and the dimension in the drawing now shows the tolerance.

As we have applied a tolerance to the dimension, the GUI automatically changes the dimension display to “Tolerance”.

Opening the parameters window, we have a column for tolerances. Selecting the tolerance cell for a dimension gives an option to edit the tolerance. This will open a tool window similar to Dimension properties, but this tool window does not have the option to change the dimension name. This can be done in the parameters window so no need for the option in this window.

In certain dimension input fields, there is the option to edit the tolerances from the expanded tool menu. This tool is available when editing dimension values (as below), and in some feature tool windows.

Tolerance types.

When creating our designs, it may be necessary to apply a non-standard tolerances to a particular dimension. This can be done through the tolerance type drop down menu.

For the rectangular cut out in the model I have applied a deviation to the vertical dimension, and a limit to the horizontal dimension.

Evaluated Size

When adding tolerances to our dimensions we can choose to display our values by one of 4 options:

1. Upper limit
2. Lower limit
3. Median value
4. Nominal Value

When we create a dimension, it is set to nominal by default. This will create the model as the entered value for the dimension.

The Upper and lower options will change to model size to reflect the option chosen. Using the Plate_Length (100mm +/- 0.5) dimension as an example and setting the evaluated size to upper will change the model to its maximum value.

Depending on how the dimensions are displayed, we can see that the dimension is underlined in Tolerance view to show that the displayed value has an evaluated size applied, but still shows the nominal value with the tolerance.

We can change the Dimension Display option to Precise to display the evaluated size, in this case, the upper limit value in the sketch.

Changing the evaluated size to lower, changes the actual size to its minimum value.

The median evaluated size will give the mid-range value for the dimension tolerance. Using the 20mm +0.3/-0.1 deviation tolerance we can see the median value of 20.1mm

And the limits value of 29.45 – 30mm gives a value of 29.725mm.

We can also see the actual values, depending on our evaluated size selection, in the parameters window in the model value column.

Summary

Dimension tolerances are a vital part of the design process allowing for precision fits or reducing precision to allow for easier assembly and/or reduce manufacture costs. With the often-overlooked tolerance tools in Inventor, adding tolerances to designs is quick and simple, and opens additional assessment options and workflows downstream, reducing overall costs, simplifying assembly processes and shortening time to market.

If you would like additional information regarding Autodesk Inventor, or any other Autodesk product, please do not hesitate to contact us at customer.services@cadline.co.uk.