When developing products, it’s important that engineers make informed design decisions. Factors like material, weight, and safety factor are typically key inputs that drive the design process. It’s an iterative process that can require hundreds of different configurations to be tested to see which performs the best and still satisfies the required criteria. Fortunately, the Inventor Stress Analysis environment has a tool called Parametric Study that quickly generates, analyzes, and sorts variations of models to help guide the designer.
Let’s use a bicycle crank arm as an example of parametric study. There are elements of the arm that might not change significantly (e.g. thread sizing, material, length). However, there are thousands of different thicknesses that could potentially work. Additionally, there are thousands of cutout shape and sizes that could be used to reduce the weight of the arm. Here are some potential arm designs with varying thickness and cutout dimensions:
Before jumping into a Parametric Study it’s best to name your key parameters in your model. For the crank arm, let’s focus on the thickness, slot depth, and slot length. Those elements will have a significant impact on the weight of the design and are easy to change.
To start a new study, click on the Environments tab in Inventor and choose “Stress Analysis.” Then click on "Create Study." In the dialogue box – use the drop-down menu to change the Design Objective to “Parametric Dimension.” Then select “OK” to begin the new stress analysis study.
Next, build a Linear Static load study in the typical fashion. This will involve assigning materials, defining loads, constraining faces, and generating assembly contacts. For the crank arm and pedal assembly, the threaded sections are assigned a bonded contact. The side faces of the pedal and crank arm are assigned a separation contact.
Both parts are assigned the material Aluminum 6061. The mesh is reduced to a global size of 3% the bounding box length. This will produce a converged and reliable result.
The square faces where the arm will attach to the crank assembly are constrained as Fixed. This means that the nodes on those faces cannot translate or rotate along any axis. A 100 lbf load is applied to the two horizontal faces of the pedal in the orientation shown below. This position of the crank arm and force value represents the maximum load scenario.
To setup the input parameters, begin by right-clicking on the model name below the analysis name in the Study browser. Then, choose “Show Parameters.”
From the dialogue box, choose the parameters that will be changing during the study. Click the check box in the “Model Parameters” column to add to the study. This will create the varying configurations for the solver. It’s best to start simple and only choose 2-4 parameters. Click “OK” to finish.
Next, click on Parametric Table from the analysis ribbon. Right-click in the Design Constraints table and select “Add Design Constraint.” The design constraints are the result values that are critical to the success of the design. These include things like Mass, Safety Factor, Von Mises Stress, Displacement, etc.
There’s list of design constraints to choose from. Highlight the constraint and select “OK” to add it to the study. For this study – Von Mises Stress (Maximum) and Mass will be used.
After you’ve selected the required design constraints, limits and criteria can be set in the table. This allows for the results to be filtered and sorted based on key values. For example – finding which configuration yields the lowest mass while still satisfying a safety factor of 2.
Parameter values can be configured in the lower table. Discreet values can be entered with commas in between. This method was applied for the thickness because the stock material will likely come in a standard size. A range of values can be entered with a dash in between. Adding a colon with an additional value specifies how many points in the range. (e.g. 2-4:5 would yield 2, 2.5, 3, 3.5, 4)
It’s recommended to create all the configurations prior to running the analysis. This will confirm that none fail and will improve the run-time of the study. Right-click in the lower table and select Generate All Configurations. Depending on how many values you’ve entered, this could take 5-10 minutes. Take a coffee break.
After generating all the configurations, it’s time to run the study. Click on Simulate from the ribbon to begin. From the drop-down menu – choose to run either an Exhaustive Set or Smart Set of configurations. Exhaustive Set will run a study on every single configuration. The Smart Set will solve the base configuration and each parameter change to the base – then interpolates the other results.
Now for the fun part! Once the study is finished, open back up the Parametric Table. For Max Von Mises Stress, I’ve entered an Upper limit of 35 ksi (the yield strength of AL6061) and a Safety Factor of 1.5. For Mass I’ve entered “Minimize” which will produce the configuration that satisfies the other criteria and minimizes mass. If the constraint is satisfied with the configuration – a green circle or checkmark will appear next to the result value.
To satisfy a safety factor of 1.5 – the study recommends a 0.5” thick crank arm with a 6” long and 0.25” deep cutout. This will produce a design that weighs 0.91 lb.
Let’s say that the design team wants to be more conservative and achieve a safety factor of 3. Simply change the constraint limit and the results will be sorted to find the correct configuration! As shown below, to achieve a safety factor of 3, the study recommends a 0.625” thick crank arm with a 5.2” long and 0.25” deep cutout. This adds some weight, but not much.
Once a satisfactory configuration has been identified it can be promoted to the model. Right-click in the lower table and select “Promote configuration to model.”