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 simulate rising levels of water over time in FEA

In a time based analysis (MES) Hydrostatic pressure is a straight forward load you can apply to any surface within Simulation Mechanical. All you have to do is to;

• pick a surface,
• define the direction of gravity (which will increase the pressure load linearly in that direction) and
• enter the fluid density

But what if you wanted to simulate effects of increase in the amount of water over time?  

Think of heavy rains over a short period of time and its effects on a dam gate like the one shown here.

Hydrostatic pressure load definition does not give you the option to change the water level over time. 

No need to panic J

Instead of increasing the water level, you can simply use prescribed displacements to move the object deeper and deeper in to the water which will increase the pressure acting on the surface.

To accomplish this I recommend creating 2 load curves:

• The 1^st one will be ramp up style and it will control the motion.
• The 2^nd one will be a steady load curve and it will control the hydro static pressure.
• Make sure the hydrostatic pressure you have applied has the “follows displacement” option enabled. 

When you run the simulation you will see that the deformations will increase as your design dips deeper in to the water which represents rising water levels. 

The video on the right shows the increase in stress levels as the pressure builds up