# OS-HM-T: 5010 Linear Transient Heat Transfer Analysis of an Extended Surface Heat Transfer Fin

This tutorial outlines the procedure to perform a linear transient heat transfer analysis on a steel extended-surface heat transfer fin attached to the outer surface of a system generating heat flux (for example, an IC Engine).

Before you begin, copy the file(s) used in this tutorial to your working directory.
1. Install the latest versions of Altair HyperMesh, Altair HyperView, and Altair HyperWorks Solvers.
2. For more information, refer to the OptiStruct Linear Transient Heat Transfer Analysis User Guide.
The extended surface heat transfer fin analyzed in this tutorial is one of many from an array of such fins connected to the system. The fins draw heat away from the outer surface of the system and dissipate it to the surrounding air. The process of heat transfer out of the fin depends upon the flow of air around the fin (free or forced convection). In the current tutorial, the focus is on transient heat transfer through heat flux loading and free convection dissipation. An extended surface heat transfer fin made of steel is illustrated in Figure 1. To meet certain structural design requirements, the fin is bent at 90° at approximately a quarter of its length.
Note: A free convection analysis is conducted in this tutorial. However, if forced fluid flow (forced convection) is allowed over the outer surface of the system, offsetting the fins from each other periodically interrupts the growth of a thermal boundary layer and a reduction in flow velocity occurs due to form drag, resulting in a higher heat transfer rate.

The extended surface heat transfer fin is meshed with CHEXA elements in HyperMesh and a transient heat transfer analysis is performed in HyperMesh using the OptiStruct solver. A typical heat flux load of 100 KW/m2 is applied to the face connected to the outer surface of the system. An ambient temperature of 25°C is assumed and all material properties are assumed to remain constant with temperature and time. Free (Natural) convection is assumed over the entire surface of the material, wherein heat transfer between the surface of the fin and the surrounding air occurs due to a complex mechanism of density differences resulting from temperature gradients.

Checkpoint:

Steady-state heat transfer analysis is generally sufficient for a wide variety of applications. However, in situations where the system properties vary significantly over time and this variation needs to be captured for the intended application, the transient nature of heat transfer must be considered. Some examples are the relatively slow heating of airplane gas turbine compressor disks compared to the turbine casing leading to aerodynamic issues during takeoff, or the analysis of the time taken for the onset of frostbite in fingers or toes.

The following exercises are included:
• Create the thermal material and the solid property for the given component
• Assign the material and property to the component
• Create flux and convective loads and boundary conditions for the model
• Submit the job to OptiStruct
• Post-process the results using 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 heat_transfer_fin.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 Thermal Material and Properties

The imported model only contains the component and predefined element sets for boundary condition creation. Create a thermal material that can be assigned to this component.

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.
4. In the Create Material window, enter the following values for the material, steel:
1. [K] Thermal conductivity = 7.3 x 10-2 W/mm °C
2. [CP] Heat capacity at constant pressure = 508 J/Kg °C
3. [RHO] Material density = 7.9 x 10-6 Kg/mm3
4. [H] Heat transfer coefficient = 4 x 10-5 W/mm2 °C
5. Click Close.
This is purely a heat transfer analysis, so structural properties (for example, the MAT1 card) are not required. It is assumed that the thermal material properties (MAT4) are temperature independent.
A new material, steel, is created with thermal properties necessary for a transient heat transfer analysis. Next, create the solid property for this model referencing the PSOLID entry and connect the material, steel, to this property; the property can then be assigned to the existing component.
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 steel fin is 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 auto1 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.

### Create Time-steps for the Transient Heat Transfer Analysis

A transient analysis captures the behavior of the system over a specific period of time. Therefore, a time period of interest for your system is defined. A time period of 500 seconds (8 minutes, 20 seconds) is defined with results output every 10 seconds. A load collector is created for this purpose and the TSTEP entry is referenced.

1. In the Model Browser, right-click and select Create > Load Collector.
2. For Name, enter Time Steps.
3. For Card Image, select TSTEP.
4. For TSTEP_NUM, enter a value of 1.
5. For the number of time steps (N), enter 50
6. Set each time increment (DT) to 10.
This encompasses a total time period of 500 seconds in which to capture the behavior of the system.
7. Click Close.

### Create Initial Conditions for the Transient Heat Transfer Analysis

Since the temperature profile of the system varies over time, the initial grid point temperature profile must be set to specify the starting point for the analysis. Assume that the temperature of the entire system is equal to 25°C at T = 0 seconds; the TEMPD Bulk Data Entry sets the initial temperatures.

1. In the Model Browser, right-click and select Create > Load Collector.
2. For Name, enter Initial Conditions.
3. For Card Image, select TEMPD.
4. For T1, enter 25.
5. Click Close.

## Apply Ambient Temperature Boundary Conditions

Ambient temperature thermal boundary conditions are applied on the model by creating specific load collectors for each. The ambient temperature is controlled using an SPCD entry, as this allows an ambient temperature variation over time to help mimic such physical requirements (if any).

### Create the SPCD Entry for Time-variant Ambient Temperature

A time-variable ambient temperature can be created by referencing an SPCD entry via a TLOAD1 load step input data entry. The time variable nature of the ambient temperature can be captured using a TABLED1 entry also referenced by the TLOAD1 data.

1. In the Model Browser, right-click and select Create > Load Collector.
2. For Name, enter Ambient SPCD.
3. For Card Image, select None.
The newly created Ambient SPCD load collector becomes the current load collector.
4. Click Close.

### Create the Amplitude

Create the amplitude (constant part) of the time variant ambient temperature using an SPCD data entry.

1. From the Analyze ribbon, select Constraints.
2. For Entities, select Nodes > .
3. In the Advanced Selection window, select By ID from the drop-down menu.
4. In the text box, enter 5672 and click OK.
6. Clear the check boxes for DOF1, DOF2, DOF3, DOF4, DOF5, and DOF6.
7. Click Create and Close.
8. From the Constraints tool group, select the BCs Browser satellite icon.
10. For the SPCD constraint, D field, enter 25.0.
This creates an SPCD referencing the ambient node specifying a temperature of 25°C.

### Create a Curve

Create a curve to define the time variant nature of the ambient temperature. This is done by creating a TABLED1 entry.

1. In the Model Browser, right-click and select Create > Curve.
A new Curve Editor window opens.
2. For Name, enter Ambient SPCD Table.
3. In the table, enter the following values:

x(1) = 0.0

y(1) = 1.0

x(2) = 500.0

y(2) = 1.0

4. Close the editor.
5. In the Model Browser, double-click on curves to open the Curves Browser.
6. Select Ambient SPCD Table.
7. In the Entity Editor, change the card image from TABDMP1 to TABLED1.
Note: In this tutorial, a constant ambient temperature (the values of y(1) and y(2) are the same leading to a constant temperature distribution over the first 500 seconds) is defined; this demonstrates the procedure to use a TABLED1 entry to specify a time variant ambient temperature as well. To do this, specify different values for the y# fields and depending on the type of variation required, select from LINEAR or LOG options.

1. In the Model Browser, right-click and select Create > Load Step Inputs.
2. For Name, enter Ambient SPCD TLOAD1.
3. For Config Type, select Dynamic Load - Time Dependent.
The SPCD and its corresponding TABLED1 table are linked to the TLOAD1 entry.
5. For EXCITEID, select the Ambient SPCD load collector.
6. For TYPE, select DISP,
7. Click TID and select the Ambient SPCD Table from the curve menu.
8. Click Close.

### Create SPC Data Entries

All entities referenced by SPCD entries should also be constrained by SPC data entries. The value of the corresponding SPC referencing an ambient point controlled via an SPCD by TLOAD1/TLOAD2 entries should be equal to zero (0.0).

1. Create a new load collector named Ambient SPC.
2. For Card Image, select None.
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 5672 and click OK.
7. Clear the check boxes for DOF1, DOF2, DOF3, DOF4, DOF5, and DOF6.
8. Click Create and then Close.

## Apply a Heat Flux Load

Ambient temperature thermal boundary conditions are assigned to the model and heat flux load from the outer surface of the engine (to which the fin is attached) is applied next on the model. A time-varying heat flux load of 0 to 0.1 W/mm2 from 0 to 500 seconds is used for the analysis of this fin. This load is applied on the model by creating specific load collectors for the corresponding TLOAD1, QBDY1 and TABLED1 entries similar to the procedure used for the ambient temperature SPCD definition.

### Create the QBDY1 Entry for Time-variant Heat Flux Load

A time variable heat flux load can be created by referencing an QBDY1 entry via a TLOAD1 load step input data entry. The time variable nature of the heat flux load can be captured using a TABLED1 entry also referenced by the TLOAD1 data.

1. In the Model Browser, right-click and select Create > Load Collector.
2. For Name, enter Heat Flux QBDY1.
3. For Card Image, select None.
4. Click Close.

### Create the Heat Flux Load

1. From the Analyze ribbon, click Heat Flux.
2. In the Create Load window, next to ELSETID, click > Create.
You can create a SURF SET on which the heat flux is applied.
3. For Name, enter flux_surf.
4. For Elements, select 0 Elements then switch to Faces in the drop-down menu.
5. Hover over and select the faces automatically highlighted in the short end of the fin.
With this method, you can easily select the faces on which heat flux is applied.
6. Once the faces are selected, click .
7. For QBDY1 Option, Q0 field, enter 0.1.
8. Click Close.

### Create a Curve

Create a curve to define the time variant nature of the heat flux load. This is done by creating a TABLED1 entry.

1. In the Model Browser, right-click and select Create > Curve.
A new Curve Editor window opens.
2. For Name, enter Heat Flux Table.
3. In the table, enter the following values:

x(1) = 0.0

y(1) = 0.0

x(2) = 500.0

y(2) = 1.0

4. Close the editor.
5. In the Model Browser, double-click on curves to open the Curves Browser.
6. Select Heat Flux Table.
7. In the Entity Editor, change the card image from TABDMP1 to TABLED1.
Note: In this tutorial, a linearly incremental heat flux load is defined (the values of y(1) and y(2) are 0 and 1 leading to a linearly increasing heat flux distribution over the first 500 seconds).

1. In the Model Browser, right-click and select Create > Load Step Inputs.
2. For Name, enter Heat Flux TLOAD1.
3. For Config Type, select Dynamic Load - Time Dependent.
The QBDY1 and its corresponding table are linked to the TLOAD1 entry.
5. For EXCITEID, select the Heat Flux QBDY1 load collector.
7. Click TID and select the Heat Flux Table from the curve menu.
8. Click Close.

Free convection is assigned in a similar manner to the procedure used for the creation of the conduction interface. Free convection is, however, automatically assigned to all heat transfer subcases and the PCONV and CONV entries should refer to the material, steel, and the ambient temperature. The difference between the ambient temperature and the structural surface temperature allows for calculation of the amount of heat transferred through free convection.

Surface elements are created to simulate the heat exchange between the fin surface and the surrounding air.

1. In the Model Browser, right-click and select Create > Load Collector.
2. For Name, enter free convection.
3. For Card Image, select None.
4. Click Close.
5. From the Analyze ribbon, click Convection.
6. For ELSETID, select > Create.
You can create a SURF SET which contains the faces participating in free convection heat transfer.
7. For Name, enter convection_surf.
8. For Elements, select 0 Elements then switch to Faces in the drop-down menu.
9. Hover over and select all faces that are not part of the previously defined heat flux input surface.
10. After the required faces are selected, click .
The convection surface elements are displayed in blue and the conduction heat flux surface elements are displayed in orange in this model as seen in the image below (the colors are arbitrary based on the assigned color of the SURF entries, and may differ in your model).
11. Next to PCONID, select > Create.
12. For Name, enter convection.
13. For Material, click Unspecified > to open Advanced Selection.
14. Select Steel and click OK.
15. For TA1, click Unspecified > to open Advanced Selection.
16. Select By ID from the drop-down menu and enter node ID 5672 in the text box.
This sets the convection boundary condition by identifying the convection ambient point for free convection ambient temperature definition.
17. Click Close.

Two different TLOAD1 entries are defined and since they are to be referenced in the same subcase, they should be combined using a DLOAD Bulk Data Entry.

1. In the Model Browser, right-click and select Create > Load Step Inputs.
2. For Name, enter Combined Flux and Convection.
3. For Config Type, select Dynamic Load Combination.
4. For S, enter 1.0.
5. As only a simple linear addition of the two TLOAD1 entries is required, for DLOAD_NUM, enter 2 and press Enter.
6. Click .
7. In the pop-up window, enter S(1) = 1.0 and S(2) = 1.0.
8. For L(1), select Ambient SPCD TLOAD1.
9. For L(2), select Heat Flux TLOAD1.
10. Click Close twice.

### Create a Transient Heat Transfer Load Step

An OptiStruct transient heat transfer load step is created which references the time steps in the Time Steps load collector, the initial conditions in the Initial Conditions load collector, the heat flux and free convection setup in the Combined Flux and Convection load collector, and the SPC boundary condition in the Ambient SPC load collector. The gradient, flux, and temperature output for the heat transfer analysis are also requested.

1. In the Model Browser, right-click and select Create > Load Step Inputs.
2. For Name, enter transient heat transfer.
3. For Analysis type, select Heat transfer (transient) from the drop-down menu.
4. For SPC, select Unspecified > Loadcol.
5. In the Advanced Selection dialog, select Ambient SPC as the SPC and click OK.
6. For TSTEP, select Time Steps.
7. For DLOAD, select Combined Flux and Convection.
8. In the SUBCASE OPTIONS, select the IC check box.
10. Click on Unspecified and select Initial Conditions.
11. Select the Output check box.
12. On the sub-list, select the THERMAL and FLUX options.
13. For both options, set the FORMAT field to H3D.
14. For both options, set the OPTION field to ALL.
15. Click Close.

## Run OptiStruct

1. On the Analyze ribbon, under the Analyze tool group, select Run OptiStruct Solver.
2. In the File Explorer, save the model as heat_transfer_fin_complete to your working directory.
The .fem filename extension is the recommended extension for OptiStruct input decks.
3. Click Save.
4. In the Solver Export Options window, for Export, select All and accept all other default settings.
5. Click Export.
6. In the Altair Compute Console, for Options, add the following run options:
7. Click Run.
8. Once the job completes successfully, the ACC Solver View window opens and an ANALYSIS COMPLETE message is printed in the Message log.
9. Click Close.
If the job is successful, you should see new results files in the directory in which heat_transfer_fin_complete.fem was run. The heat_transfer_fin_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 Transient Heat Transfer Analysis Results

1. When the message Process completed successfully is received in the command window, click Results.
HyperView is launched and the results are loaded.
2. For Result type, in the first drop-down menu, select Grid Temperatures(s).
3. Click Apply.
4. From the Results Browser, select Time = 5.0000000E+02.
A contour plot of grid temperatures at the final time step is created.
This is the grid point temperature plot after 500 seconds. The system is input a linearly increasing heat flux from 0 to 0.1 W/mm2 from 0 to 500 seconds respectively. Therefore, a physical correlation can be the effect of starting an IC engine to full capacity wherein the flux transmitted to the outer surface linearly increases with time.
Note: The flux patterns in actuality may be different and may fluctuate based on the duration of the power cycles. The maximum temperature of 80.32°C predictably occurs at the elements closest to the heat flux loading site and the minimum temperature of 25.0°C occurs at elements farthest from the heat source.
5. From the Results Browser, select Time = 4.6000000E+02.
A contour plot of grid temperatures is created.
6. For Results type, first drop-down menu, select Element Fluxes (V).
7. Click Apply.
8. From the Results Browser, select Time = 5.0000000E+02 to view the element flux results after 500 seconds.
In a practical setting, you can also see the effect of free convection in the reduction of temperature at the outer surface of the system. Convection (due to the extended surface area) allows a larger amount of heat to be drawn out of the system when compared to the absence of an extended surface fin. This is evident in the temperature of the outer surface of the system after 500 seconds in the absence of convection heat loss.

The maximum temperature at the outer surface of the heat source system is 125.3°C, which decreases by around 45°C to 80.3°C when free-convection is included. Therefore, using an extended surface fin is a very effective way to reduce the temperature of a system.