# OS-HM-T: 5005 Linear Steady State Heat Convection Analysis

In this tutorial, a heat transfer analysis is performed on a steel pipe.

Before you begin, copy the file(s) used in this tutorial to your working directory.
The temperature on the inside surface of the pipe is 60 °C. The outside surface is exposed to the surrounding air, which is at 20 °C. The temperature distribution within the pipe can be determined by solving the linear steady state heat conduction and convection solution.
The following exercises are included:
• Create the thermal material and property
• Create and apply the thermal boundary conditions on the model
• Submit the job to OptiStruct
• Post-process the results in HyperView

## Launch HyperWorks

1. Launch Altair HyperWorks.
2. In the New Session window, select HyperMesh from the list of tools.
3. For Profile, select OptiStruct.
4. Click Create Session.
This loads the user profile, including the appropriate template, menus, and functionalities of HyperMesh relevant for generating models for OptiStruct.

## Import the Model

1. On the menu bar, select File > Import > Solver Deck.
2. In the Import File window, navigate to and select thermal.fem you saved to your working directory.
3. Click Open.
4. In the Solver Import Options dialog, ensure the Reader is set to OptiStruct.
5. Accept the default settings and click Import.

## Set Up the Model

### Create the Thermal Material Properties

1. In the Model Browser, right-click and select Create > Material.
A default MAT1 material displays in a Create Material window.
2. For Name, enter steel.
3. Select the check box next to MAT4.
The MAT4 card image appears below MAT1 in the material information area. The MAT1 card defines the isotropic structural material. The MAT4 card is for the constant thermal material. MAT4 uses the same material ID as MAT1.
4. In the Create Material window, enter the following values for the material, steel:
1. [E] Young’s modulus = 2.1 x 1011 Pa
2. [NU] Poisson’s ratio = 0.3
3. [RHO] Material density = 7.9 x 103 Kg/m3
4. [A] Thermal expansion coefficient = 1 x 10-5 / °C
5. [K] Thermal conductivity = 73W / (m * °C)
6. [H] Heat transfer coefficient = 40W / m2 °C
5. Click Close.
A new material, steel, is created with both structural and thermal properties.
6. In the Model Browser, right-click and select Create > Property.
A default PSHELL property displays in a Create Property window.
7. For Name, enter solid.
8. For Card Image, select PSOLID from the drop-down menu.
9. For Material, click Unspecified.
10. Click .
11. In the Advanced Selection window, select steel and click OK.
12. Click Close.
The property of the solid steel pipe has been created as 3D PSOLID. Material information is linked to this property.

### Link the Material and Property to the Existing Structure

Once the material and property are defined, they need to be linked to the structure.

1. In the Model Browser, double click Components to open the Components Browser.
2. Click on the pipe component.
The component template displays in the Entity Editor.
3. For Property, click Unspecified.
4. Click .
5. In the Advanced Selection window, select solid and click OK.

## Apply Thermal Loads and Boundary Conditions

In this exercise, the thermal boundary conditions are applied on the model and saved in a predefined load collector spc_temp. A predefined node 4679 specifies the ambient temperature. A predefined node set node_temp contains the nodes on the inside surface of the pipe.

### Create Temperatures on the Inner Surface of the Pipe

1. From the Analyze ribbon, select Constraints.
2. For Entities, select Nodes > .
3. In the Advanced Selection window, select By Set from the drop-down menu.
4. Select node_temp and click OK.
5. Clear the check boxes for DOF1, DOF2, DOF3, DOF4, DOF5, and DOF6.
6. For Load Type, select SPC.
7. Click Create and Close.
This applies the temperature 0.0 on the inside nodes. In the next step, the temperature value is updated to 60.
8. In the Model Browser, in Loads, double-click SPC.
9. Right-click and choose Select > All from the context menu.
10. For D, enter 60.0.

### Create Ambient Temperature

1. In the Model Browser double-click on Load Collectors.
2. In the browser tab, right-click spc_temp and select Make Current from the context menu.
3. From the Analyze ribbon, select Constraints.
4. For Entities, select Nodes > .
5. In the Advanced Selection window, select By ID from the drop-down menu.
6. In the text box, enter 4679 and click OK.
Node 4679 is highlighted.
7. Clear the check boxes for DOF1, DOF2, DOF3, DOF4, DOF5, and DOF6.
8. Click Create and Close.
9. In the Model Browser under Loads, double-click SPC.
11. For D, enter 20.0.

### Create Heat Convection Surfaces

1. From the Analyze ribbon, select Convection.
2. For Type, select Convection from the drop-down menu.
3. For ELSETID, select > Create.
4. For Elements, select Faces from the drop-down menu.
5. Select the ourter faces as shown in Figure 16.
6. For PCONID, select > Create.
7. For Material, click to open Advanced Selection.
8. Select Steel.
9. For TA1, click Nodes > .
10. In the Advanced Selection dialog, select By ID from the drop-down menu and enter ID 4679.
11. Click Close.

### Create a Heat Transfer Load Step

An OptiStruct steady state heat convection load step is created, which references the thermal boundary conditions in the load collector spc_temp. The gradient, flux, and temperature output for the heat transfer analysis is also requested.

1. In the Model Browser, right-click and select Create > Load Step.
2. For Name, enter heat_transfer.
3. For Analysis type, select Heat transfer (steady state) from the drop-down menu.
4. For SPC, click to open Advanced Selection.
5. Select spc_temp and click OK.
6. Select the Output check box.
7. Under Output, select the FLUX and THERMAL check boxes.
8. For both outputs, for FORMAT select H3D.
9. For both outputs, for OPTION select ALL.
10. Click Close.

## Submit the Job

Run OptiStruct.

1. From the Analyze ribbon, click Run OptiStruct Solver.
A browser window opens.
2. Select the directory where you want to write the OptiStruct model file.
3. For File name, enter thermal_complete.
The .fem filename extension is the recommended extension for Bulk Data Format input decks.
4. Click Save.
5. Click Export.
6. For run options, toggle analysis.
7. Click Run.
If the job is successful, you should see new results files in the directory in which thermal_complete.fem was run. The thermal_complete.out file is a good place to look for error messages that could help debug the input deck if any errors are present.

## View the Results for Heat Transfer Analysis

A "Process completed successfully" message appears in the HyperWorks Solver View window.

1. In the HyperWorks Solver View window, click HyperView.
HyperView is launched and the results are loaded. A message window appears to inform model and results files were successfully loaded.
2. Close the message window, if one appears.
3. Click Contour .
4. In the first pull-down menu below Result type, select Grid Temperatures (s).
5. Click Apply.
A contour plot of grid temperatures is created. You may have to use the Edit Legend function to get the contour.
6. In the first pull-down menu below Result type, select Element Fluxes (V).
7. Click Apply.
A contour plot of fluxes is created. You may have to use the Edit Legend function to get the contour.