Physics Setup

Temperature Boundary Condition

First, under Steady-State Thermal (A5) click Initial Temperature. In the Details window, we can see that the initial temperature is 22 degrees Celsius. We want the temperature change to be 100 degrees Celsius. So, we need to specify a boundary condition of 122 degrees Celsius. Click on to open the Thermal Environment menu in the menu bar. In the Thermal Environment menu, click on to create a temperature essential boundary condition.

Next, we need to select the boundary for the boundary condition. Click the point selection filter and select the right point of the line body. In the Details window, select Geometry > Apply. Now, specify the temperature Magnitude to 122.

Elasticity Boundary Conditions

Now, we have to specify the boundary conditions that will affect the elasticity solution to this simulation. In the Outline window, click on to bring up the structural environment menu bar. In the structural environment, select Supports > Fixed Support. Ensuring that the point selection filter is selected, select the left side of the bar, and in the details window select Geometry > Apply.

Next, we need to specify a displacement constraint to represent the gap in the wall. In the Structural Environment menu, select Supports > Displacement. In the Details window, change the X Component from Free to 0.002 m. Also, select the right point of the bar using the point selection filter, and select Geometry > Apply.

Click here to enlargeVisit page in new window

There should now be 3 boundary conditions on the bar. The left end should be fixed, and the right end should have a temperature boundary condition and a displacement boundary condition.

Go to Step 5: Numerical Solution

Go to all ANSYS Learning Modules

  • No labels