Map the heat distribution of a solar panel

Practice to create a mapping solution on the target structural model, mapping the temperature results for a specific time step, from a source thermal model, and run a structural analysis.

Download and extract the part files.

Open the thermal Simulation file

Open the Simulation file and reset the dialog box settings.

  1. Choose File→Open and open panel/panel_s_thermal.sim.
  2. Choose File→Preferences→User Interface and on the Dialog and Precision page, reset the dialog box memory.
  3. In the Simulation Navigator, expand and explore all nodes.
  4. Choose File→Open and open panel/panel_s_structural.sim.
    Notice that tetrahedral type elements are used.

Display the thermal results

Display the temperatures at 5000 seconds, which you will be mapped onto the structural model later.

  1. Click the (Simulation) panel_s_thermal.sim tabbed window.
  2. In the Simulation Navigator, under the Thermal solution node, double-click the Results node.
  3. In the Post Processing Navigator, expand the Thermal→Increment 18, 5000 sec nodes and double-click the Temperature - Nodal node.
  4. Expand the Post View 1→panel_f_thermal.fem→2D Elements nodes and hide Black Side Panel Collector.

Create the mapping solution

Create a mapping solution on the structural Simulation file, which you will open first. The mapping solution will point to the thermal solution results.

  1. Click the (Simulation) panel_s_structural.sim tabbed window.
  2. In the Simulation Navigator, right-click the panel_s_structural.sim node and choose New Solution.
  3. In the Solution group, from the Solver list, select one of the following options: Simcenter 3D Thermal/Flow, Simcenter 3D Electronic Systems Cooling, Simcenter 3D Space Systems Thermal, or Simcenter 3D Multiphysics.
    Note that for this activity the Simcenter 3D Space Systems Thermal solver is selected.
  4. From the Analysis Type list, select Mapping.
  5. Click Create Solution.
  6. On the Mapping Details tab, in the Data Source and Destination group, click Browse and select the panel_s_thermal-Thermal_solution.bun file.
  7. In the Transient Times group, in the Select Output Times box, type 5000.
  8. On the Optional Output tab, in the Output Format group, select the Create Nastran Solution check box.
  9. Click OK.

Solve the mapping solution

Solve the mapping solution you just created on the structural model.

  1. In the Simulation Navigator, right-click the Solution 1 node and choose Solve.
  2. In the Solve dialog box, click OK.
  3. Wait for the mapping solve to end, before proceeding.
  4. In the Analysis Job Monitor dialog box click Cancel.
  5. Close the Information window.

Display mapped thermal results

Display the mapped thermal results on the structural panel simulation file at time 5000 sec.

  1. In the Simulation Navigator, under the Solution 1 node, double-click the Results node.
  2. In the Post Processing Navigator, expand the Thermal→Increment 1, 5.000E+03s nodes and double-click the Temperature – Nodal node.
  3. Expand the Post View 2→panel_f_structural.fem→2D Elements and hide Black Side Panel Collector.
    You mapped temperatures at a specific time: 5000 seconds. The temperature is approximately 55 °C and uniform.
  4. Right-click the (Simulation) panel_s_structural.sim tabbed window and choose Layout→2 Tabbed Groups .
  5. Choose Results tab→View Layout group→Synchronize Views .
  6. Select both graphics windows.
  7. In the View Settings dialog box, click OK.
  8. Choose Results tab→Context group→Return to Home .

Constrain the panel

Apply a fixed constraint at one of the sides of the satellite panel.

  1. Click the (Simulation) panel_s_structural.sim tabbed window.
  2. In the Simulation Navigator, double-click the Mapping Nastran node.
  3. Expand the Subcase1→Loads→Temperature Set – Temperature1 nodes.
  4. Notice the Temperature1 load, which was created by the mapping process.
  5. Choose Home tab→Loads and Conditions group→Constraint Type list→Fixed Constraint .
  6. On the Top Border bar, from the Type Filter list, select Polygon Edge.
  7. Select the following two polygon edges on the model.
  8. Click OK.

Solve the structural solution

Solve the structural model with the temperature preload.

  1. In the Simulation Navigator, right-click the Mapping Nastran node and choose Solve.
  2. Click OK.
  3. Wait for the solve to end, before proceeding.
  4. In the Review Results dialog box, click No.
  5. In the Analysis Job Monitor dialog box, click Cancel.
  6. Close the Information window.

Display the structural results

Animate displacement results to compare the deformation between top and bottom sides.

  1. In the Simulation Navigator, expand the Mapping Nastran node and Results nodes.
  2. Right-click the Structural node and select Specify.
  3. In the Results File Name group, click Browse and select panel_s_structural-mapping_nastran.op2.
  4. Click OK twice.
  5. In the Post Processing Navigator, double-click the Structural node→Displacement Nodal node.
    The average displacement is approximately 0.110 mm.
  6. Choose Results tab→Animation group→Play.
You have completed this lab.