In this lesson you will perform the following tasks:

In this lesson you will construct a model with two separate radiation enclosures: one for gray body radiation and the other for wavelength-dependent radiation. No material (e.g., air) will be defined in the enclosure; therefore, only Radiation heat transfer can transfer heat energy across the enclosures. In the enclosure where it is assumed that the surfaces are gray, the emissivity will be constant regardless of the surface temperatures. The other enclosure will incorporate wavelength-dependent radiation which is a significant extension of the gray body theory. Normal radiosity is divided into discrete frequency bands with emissivity and transmissivity assumed to be gray within these frequency bands.

Before creating the next piece of the model set the Display Lines to zero.

To create the next region of the model change the Vector Coordinate List to <0.5, 0.5, 0> click in the Origin Coordinate List, and select Point 4 in the viewport.

Using the above construction technique complete the remaining portion of the model’s geometry.

Your completed patch geometry should look similar to that shown below.

Click on the Finite Elements Toggle in the main form. Change the Object to Mesh. Specify a Global Edge Length of 0.16666 for the QUAD 4 elements. The completed Finite Elements form and meshed model are shown below for your reference.

To simplify the visual image of your model, turn off all entity labels. Your model should now look like the one shown below.

To thermally represent the participating medium, create a Node within the enclosure. Use 1000 as its ID and create the node so that it is not associated with the model’s geometry. Use the Select a Screen Position option in the select menu to select a point inside Enclosure 2. Your completed Finite Elements form should look similar to the one shown below.

To better visualize the Node locations, set their radius to 6 pixels. Your model should now look like the one shown below.

Click on the Loads/BCs toggle in the main form. In the Loads/Boundary Conditions form enter, Temp_Participating_medium, as the New Set Name and then click on the Input Data… button. In the Input Data form, assign a fixed temperature of 200 (remember TID=-1). Click on the OK button to close the Input Data form. In the Loads/Boundary Conditions form click on the Select Application Region… button. In the Select Application Region form, change the Geometry Filter to FEM and then click in the Select Nodes databox. Select Node 1000 from the viewport. This node will represent the Participating Medium temperature. The completed forms are shown below for your reference.

Next, assign fixed temperatures of 1500°C and 0°C respectively to the top and bottom geometry edges of the model. Use T_top and T_bottom for their respective New Set Names. The completed forms are shown below for your reference.

To create the viewfactor boundary conditions for the two enclosures you will first supply geometric information in the Patran Loads/BCs form and then enter data concerning the Emissivity and Transmissivity values in the template.dat file.

In the Loads/Boundary Conditions form, change the Action, Object, and Type option menus respectively to Create, Viewfactor (P/THERMAL), and Element Uniform. Change the Target Element Type to 2D. Use the diagram and Table E‑1 and Table E‑2 to determine the required geometric information for the eight viewfactors which define the two enclosures.

 

You will now complete the Viewfactor definitions by entering the Emissivity and Transmissivity information into the template.dat file. Create a separate x-window shell and make a subdirectory in the directory you are running Patran. Use your current Patran database name for this subdirectory name. Change to that subdirectory, open and edit a file named template.dat. Next, enter the required VFAC commands to define the Emissivity and Transmissivity for Enclosures 1 and 2. The syntax of the command is:

Each term of the command is defined in Chapter 3 of the MSC Patran Thermal User’s Guide. Shown below is a table that lists the required information for the two VFAC commands and the template.dat file created with this information for your reference.

Your model with its applied boundary conditions should now look like the one shown below.

To do this, click on the Element Props toggle in the main form. When the form appears set its Action, Dimension, and Type option menus respectively to Create, 2D, and Thermal 2D. Enter Iron, for the New Set Name and then click on the Input Properties… button. Enter 18 in the Material Name databox and then click on the OK button to close the form. Next, click in the Select Members box and select all the models Patches in the viewport. Finally click on the Apply button in the Element Properties form. The completed forms are shown below for your reference.

Click on the Analysis toggle in the main form. When the Analysis form appears check that the Action, Object, and Method option menus are respectively set to Analysis, Full Model, and Full Run.

Click on the Solution Type… button. When the P⁄THERMAL Solution Type form appears specify a Steady State Thermal Analysis. To cause Viewfactor to calculate the viewfactor for both enclosures click on the Perform Viewfactor Analysis button. In the Select Viewfactor Solution frame, select the 0, Viewfactors --> Resistors option. Click on the OK button to close the form.

In the Analysis form, click on the Solution Parameters… button. In the P⁄Thermal Solution Parameters form, set the Calculation Temperature Scale to Celsius and select 0, Standard Solution for the Solver Option. Click on the OK button to close the P/Thermal Solution Parameters form.

In the Analysis form, click on the Output Requests… button. In the P⁄Thermal Output Request form, set the Units Scale for Output Temperatures to Celsius. Click on the Print Intervals Controls… button. When the P⁄Thermal Print Intervals Control form appears, set the Initial Print Interval to 5. This will cause P/Thermal to print out solution information every 5 intervals. Click on the OK button in both forms.

Submit the analysis run by clicking on Apply in the Analysis form.

As expected the temperature distribution is not horizontally symmetrical due to the different radiation boundary conditions in each enclosure.

To do this, set the Action and Object, to Create and Contour, respectively. Click on the Results Selection… button and select 1.1 Temperature, (nodal) from the Contour Results List Box. Click on the OK button to close the from. Click on the Apply to create the Temperature Contours. Your model should now look similar the one shown below.

To create Cursor tool change the Object to Cursor and then click on the Results Selection… button. Again select 1.1-Temperature, (nodal) in the Cursor Results list and click on OK to close the form. Click on the Apply button to create the Cursor Tool. When the Cursor Tool form appears click on the Apply button. Next, click somewhere on the model. You should see the temperature of the Node nearest to the mouse cursor printed on the model and in the Cursor Results form. Your model should now look similar to the one shown below.

An example Cursor Results form and its corresponding temperature locations are shown below for your reference.

Finish this exercise by quitting Patran.