Verify Fit with Autodesk Inventor Tolerances13 Jul, 2010 By: Anthony Dull
Avatech Tricks Tutorial: Use a digital prototype to determine whether real-world parts will fit together as they should.
Editor's note: This tutorial courtesy of Avatech Solutions.
Calculating tolerances has always been the hardest part of design in my experience. What happens if "Part A" tolerances go to the high side and "Part B" tolerances go to the low side? Anyone can model something on this magic box we call a computer with exact dimensions where everything fits beautifully together. The defining moment is when you have the parts in your hands and everything goes together the way it should. If not, the solution is not to get a bigger hammer — it is to use your Inventor digital prototype and explore various "what if" scenarios with your tolerances until you are satisfied that parts can be made.
In this example, we are going to enter our tolerances directly to the sketch environment as we place dimensions, as well as inside the assembly file to verify there will be no interferences between parts. As you can see in my skeletal model below, I am using the "multi-body" design concept. To ensure that the design updates correctly as changes are made, consider using any skeletal modeling technique.
Inside the sketch for the door extrusion, let's add a tolerance to the width. To do so, edit the dimension and click on the arrow to the right of the edit dimension dialog box. Then, select the tolerance option.
Apply the appropriate tolerance for your design, close the dialog box, and finish the sketch.
Now let's go and test out our new tolerance to see how it could change our design. Open up the parameter dialog box and find the dimension you just added the tolerance to. (To find parameters more easily, rename them to something that will help you locate them later on.) Under the tolerance column, change the value from nominal to upper, lower, or median and view the changes to the model.
We are now one step closer to verifying that our digital prototype is ready to be manufactured.
Ups and Downs
Now let's look at how we can add assembly tolerances to our design. When constraining parts together, think about how the parts would actually go together in the real world, and use that as a guide to constraining them within Inventor.
With that being said, let's play some "what if" scenarios with the design. What if the door width and hinge location dimensions both go to the high tolerance? Will the doors hit each other when they are opened? Let's take a look and find out. The dimension that needs to have the tolerance applied to it was from a mate constraint that located the hinges for the doors. So find the parameter in the parameter dialog box once again, but this time, select the arrow in the equation cell and choose Tolerance.
Add the appropriate tolerance for your design, then set the tolerance to upper, lower, or median and view the results in your model. Change the tolerances in the part files to see how the assembly will be affected if the assembly tolerances go high or low. Finally, drive the angle constraint for the doors to verify that they will not rub against each other if both tolerances go to the high side.
Test out all of the different scenarios here — not on the shop floor!
The Real Deal
Once our digital prototype passes all of our "what if" tests, it is time to document our design. To save time, we can retrieve dimensions from the part environment and pull them into the drawing environment. Retrieving dimensions will verify that no incorrect tolerances get placed or forgotten. By retrieving the dimensions, you now have the ability to drive the actual model dimensions from the drawing environment.
To retrieve dimensions of a part that was created using the multi-body concept, follow these steps. (If you did not use the multi-body option, skip these steps.)
- Go into the cabinet skeletal model's parameter dialog box and check the export option next to those dimensions.
- Open the door's part file and link those exported dimensions into that file.
- They are now ready to be retrieved in the drawing file.
Right-click on the view, choose Retrieve Dimensions, and select only the dimensions you want to bring to the drawing environment. We now have the intellectual data that drove the design in the drawing environment for documentation.
By utilizing Autodesk Inventor's tolerances to validate form, fit, and function, you can save time, money, and prove that your designs are second to none!