Adding Tolerances to an Autodesk Inventor Model Sketch (Avatech Tricks Tutorial)1 Sep, 2008 By: Kevin Keene
The more information that's stored in your model, the more robust the model becomes.
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Editor's note: This tutorial courtesy of Avatech Solutions.
Many of you may already use the model iProperties to automatically fill in your title blocks and Vault/Productstream databases, but you might not be taking advantage of using tolerances in the model. The more information that's stored in the model, the more robust the model becomes. By taking the time and effort to add tolerances to your model, you can gain many advantages down the road. In this article, I will be discussing two of them: interference checking and drawing dimensions. I will place a tolerance on a shaft diameter, change the model to maximum material condition to see what effect that will have on my assembly, and then bring that pre-defined tolerance into the drawing.
Adding Tolerances to a Model Sketch
Dimensional tolerances can be added while placing a dimension or when editing a dimension. To add a tolerance to a dimension, bring up the Edit Dimension dialog box and click on the arrow pointing to the right, then select Tolerance.
In the Tolerance dialog box, chose the type of tolerance that you require. In my example, I have chosen the Deviation method with an upper limit of 0.005 and a lower limit of 0.000.
Click OK to exit the Tolerance dialog box and click the green checkmark to exit the Edit Dimension dialog box. In order to see the tolerances while in your sketch, right-click in the graphics area and select Dimension Display, then Tolerance.
Using the Model Tolerances to Create Min/Max Material Conditions
Once a tolerance has been added to a dimension, use the Parameters dialog box to change the physical size of the model. In the dialog box, use the individual toggles to set the size of each dimension individually or the global toggles to set all of the dimensions at once.
Your choices are upper, median, nominal, or lower. In my example, there is only one dimension with a tolerance associated to it, so I choose to set the global tolerances to upper. After setting the tolerances to the desired settings, click OK to exit the dialog box. In order to make the tolerance changes take effect, the model must be updated. If the tolerances are big enough, you should be able to visually see your model change size. After the model has been updated, bring the Parameters dialog box back up to see what happened. In my example, even though the nominal dimension is 0.984, the model value is 0.989 due to being set to the upper limit.
Using the Part Tolerances in an Assembly
After adjusting the physical size of the model, the assembly can now be tested for interference. When running an interference check between the shaft and the bearing in my assembly, I can see how much interference there is with the 0.005 upper limit and determine if that fits my design intent.
Placing the Tolerances in the Drawing
Once the model is fully dimensioned and tolerances have been added, it is necessary to place the part into a drawing and detail it. After the desired views have been created, the dimensions must be pulled from the model using the Retrieve Dimensions command located on the right-click menu when a view is selected. With the Retrieve Dimensions dialog box open, select the needed dimensions and click OK. The dimensions will require some adjustment so they are positioned correctly. Note: if you see a line under the dimensions in the drawing, this means the model is currently at a non-nominal state. To adjust the model back to the nominal state, use the global tolerance options in the Parameters dialog box. This will make the lines disappear in the drawing, letting you know that the model is now at the nominal state. It is desirable to always save Inventor part files in the nominal state.
In conclusion, by adding tolerances to your models you come closer to a master model concept where all the information (description, part number, custom properties, material, mass, tolerances, and more) about the part is stored with the model. All of this information can then be leveraged during the design, manufacture, and data management processes.
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