Viewing applied temperatures

If you are concerned about thermally induced stresses in your design, you will want to run a thermal analysis to determine the temperature distribution. Then, map the temperature results to a subsequent structural analysis.

Mechanical Event Simulation (MES) allows a user to apply such temperatures automatically, whether from a steady-state or transient heat transfer analysis.

If you have previously run a transient thermal analysis, you may want to ensure that the mapping algorithm used for transferring the temperatures to an MES analysis has worked as expected. After all, you could be using different mesh sizes for each analysis type, and the nodal temperatures may not map one-to-one from a transient thermal analysis to an MES analysis.

So how do you check if the mapping was done correctly?

Here is how:

In this example, the FEM file is located in the following folder (C:\FEA\Bracket.fem)

Let’s say that, in Design Scenario 1, you conducted a Transient Heat Transfer analysis on an Assembly using a 100% mesh size. 

Then, you created a second Design Scenario as an MES analysis and meshed it with a 50% mesh size. You then applied the thermal loads within the Thermal tab of the Analysis Parameters dialog. 

Before running the MES analysis, simply perform a “Check Model” operation. This action creates the solid mesh and decodes the geometry, loads, and constraints. If you look in the Design Scenario 2 folder (C:\FEA\Bracket.ds_data\2), you will now see a file named “ds_map.tto”, which is a transient temperature output file mapped from Design Scenario 1 to Design Scenario 2.

At this point, change the analysis type from MES to Transient Thermal, creating a 3^rd Design Scenario. Keep the same mesh size (50%) as used in the MES analysis.

Using Windows Explorer, copy the file “ds_map.tto” from “C:\FEA\Bracket.ds_data\2” to “C:\FEA\Bracket.ds_data\3”.  Then, rename the copied file “ds.tto” (deleting “_map” from the name).

Within Simulation Mechanical perform a “Check Model” operation for the 3^rd design scenario, which is the second transient thermal analysis, without applying any loads or constraints. 

In the Results environment for design scenario 3, you will now be able to see the temperature results that were mapped from Design Scenario 1 (utilizing a 100% mesh size) to Design Scenario 2 (utilizing a 50% mesh size).   

How to Determine the Factor of Safety

When evaluating the results of a linear static stress analysis, one can specify allowable stress values and then display factor of safety contours to see where stresses in the model are below and above those allowables. Viewing factor of safety contours can help one decide whether a design needs modification or is acceptable and is ready for manufacturing.

To display factor of safety contours, choose the "View" command in the "Safety Factor" dropdown of the “Stress” panel in the “Results Contours” tab of Autodesk Simulation (see Figure 1).

Figure 1: In the "Safety Factor" dropdown, choose the "View" command to display factor of safety contours.

When this command is activated, color-coded contours of the factor of safety for the selected stress contour will be shown (see Figure 2).

Figure 2: In the Results environment, one can specify allowable stress values and then display factor of safety contours. This contour shows a color-coded graphical display of where stresses in the model are below and above the specified allowables.

The factor of safety is the ratio of the allowable stress to the actual stress:

• A factor of safety of 1 represents that the stress is at the allowable limit.
• A factor of safety of less than 1 represents likely failure.
• A factor of safety of greater than 1 represents how much the stress is within the allowable limit.

The allowable stresses can be assigned on a per part basis by choosing the "Set Allowable Stress Values" command in the "Safety Factor" dropdown (see Figure 3).

Figure 3: Choose the "Set Allowable Stress Values" command in the "Safety Factor" dropdown to specify allowable stress values.

The "Allowable Stress Values" dialog will appear and each part will be listed in a separate row. One can specify a value in the "Allowable Stress" column or press the "Load Yield Stress" or "Load Ultimate Stress" buttons to load the values from the material library (see Figure 4). Any parts for which the allowable stress is set to 0 will be excluded from the factor of safety calculations.

Figure 4: In the "Allowable Stress Values" dialog, one can enter a value for a part in the "Allowable Stress" column or press the "Load Yield Stress" or "Load Ultimate Stress" buttons to load the values from the material library.

Thus, the ability to view factor of safety contours helps engineers determine what the results say about the adequacy of a design. For example, examining these contours can help you properly exercise engineering judgment when balancing between material cost reduction and ensuring a safe product.

How to sum reaction forces

The summation of reaction forces in a model is often used to verify input loading, validate model behavior or determine floor load distributions. In the Results environment, the "Inquire: Results" dialog can be used to sum the reaction forces of selected nodes.

Another typical application of summing reaction forces is to determine the total force of a pressure load when the area of pressure is unknown and cannot be readily calculated. As shown in Figure 1, the cutting frame has a pressure load applied to two surfaces of unknown area and is fully constrained at the bottom of each of the four legs. The total force of the pressure can be calculated by summing the vertical reactions of all of the constrained nodes.

Figure 1: Note the locations of the pressure loads and constraints in this display of the vertical reaction forces in the cutting frame.

To sum the reaction forces in the Results environment for a Static Stress Analysis:

• Select and display the desired reaction (X, Y or Z) using the "Results Contours” tab,  “Other Results” panel, “Reactions” pull-down menu “Reaction Force (Negative) ” pull-out menu;
• Select the nodes that will be used in the summation;
• Right click anywhere in the working area;
• In the pop-up menu that appears, select "Inquire Results"; and
• In the "Inquire: Results" dialog (Figure 2), click on the "Summary" pull-down menu and select "Sum".

Figure 2: The "Inquire: Results" dialog displays information about the selected nodes and the calculated "Summary" value.

The summary of the reaction forces of all selected nodes will now be displayed in the "Inquire: Results" dialog. If desired, the area could be calculated since the pressure and force values are now known.