[Fluent Inc. Logo] return to home search
next up previous contents index

7.25.3 Using the Heat Exchanger Model

The heat exchanger model settings may be written into and read from the boundary conditions file (Section  4.6) using the text commands, file/write-bc and file/read-bc, respectively. Otherwise, the steps for setting up the heat exchanger models are as follows:

1.   Enable the calculation of energy in the Energy panel.

Define $\rightarrow$ Models $\rightarrow$ Energy...

2.   Specify the inputs to the heat exchanger model, using the Heat Exchanger Model panel (Figure  7.25.2).

Define $\rightarrow$ User-Defined $\rightarrow$ Heat Exchanger...

Figure 7.25.2: The Heat Exchanger Model Panel Displaying the Model Data Tab
figure

(a)   In the Fluid Zone drop-down list, select the fluid zone representing the heat exchanger core.

(b)   Under the Model Data tab, choose Fixed Heat Rejection or Fixed Inlet Temperature, as required (Figure  7.25.2).

(c)   Specify the heat exchanger model as either the default ntu-model or the simple-effectiveness-model.

(d)   Specify the Core Porosity Model if needed.

(e)   If the ntu-model is chosen, a Heat Transfer Data... button will appear under Heat Exchanger Performance Data. Clicking on the Heat Transfer Data... button will open up the Heat Transfer Data Table panel with information on the fluid flow rates and heat transfer data (Figure  7.25.3).

Figure 7.25.3: The Heat Transfer Data Table Panel for the NTU Model
figure

(f)   Enter the Auxiliary Fluid Temperature and the Primary Fluid Temperature for the ntu-model.

(g)   If the simple-effectiveness-model is chosen, then clicking on the Velocity Effectiveness Curve... button, under the Heat Exchanger Performance Data, allows you to set the velocity vs effectiveness curve.

(h)   Under the Geometry tab, define the macro grid using the Number of Passes, the Number of Rows/Pass, and the Number of Columns/Pass fields.

Figure 7.25.4: The Heat Exchanger Model Panel Displaying the Geometry Tab
figure

(i)   In the Auxiliary Fluid tab, specify the auxiliary fluid properties and conditions ( Auxiliary Fluid Flow Rate, Inlet Temperature, and Auxiliary Fluid Specific Heat).

Figure 7.25.5: The Heat Exchanger Model Panel Displaying the Auxiliary Fluid Tab
figure

(j)   In the Auxiliary Fluid tab, specify the Auxiliary Fluid Properties Method, either as a constant-specific-heat or as a user-defined-enthalpy.

(k)    Auxiliary Fluid Flow Rate, Heat Rejection, Inlet Temperature, and Inlet Pressure can be provided as a constant, polynomial or piecewise-linear profile that is a function of time.

(l)   Click Apply in the Heat Exchanger panel to save all the settings.

(m)   Repeat steps (a)-(l) for any other heat exchanger fluid zones.

To use multiple fluid zones to define a single heat exchanger, or to connect the auxiliary fluid flow path among multiple heat exchangers, see Section  7.25.4.



Selecting the Zone for the Heat Exchanger


Choose the fluid zone for which you want to define a heat exchanger in the Fluid Zone drop-down list.



Specifying Heat Exchanger Performance Data


Based on the heat transfer model you choose in the Model Data tab, some performance data must be entered for the heat exchanger.



Specifying the Auxiliary Fluid Inlet and Pass-to-Pass Directions


To define the auxiliary fluid direction and flow path, you will specify direction vectors for the Auxiliary Fluid Inlet Direction and the Pass-to-Pass Direction in the Geometry tab. Figure  7.25.6 shows these directions relative to the macros.

For some problems in which the principal axes of the heat exchanger core are not aligned with the coordinate axes of the domain, you may not know the auxiliary fluid inlet and pass-to-pass direction vectors a priori. In such cases, you can use the plane tool as follows to help you to determine these direction vectors.

1.   "Snap'' the plane tool onto the boundary of the heat exchanger core. (Follow the instructions in Section  27.6.1 for initializing the tool to a position on an existing surface.)

2.   Translate and rotate the axes of the tool appropriately until they are aligned with the principal directions of the heat exchanger core. The depth direction is determined by the red axis, the height direction by the green axis, and the width direction by the blue axis.

3.   Once the axes are aligned, click on the Update From Plane Tool button in the Heat Exchanger Model panel. The directional vectors will be set automatically. (Note that the Update from Plane Tool button will also set the height, width, and depth of the heat exchanger core.)



Defining the Macros


As discussed in Section  7.25.1, the fluid zone representing the heat exchanger core is split into macros. Macros are constructed based on the specified number of passes, the number of macro rows per pass, the number of macro columns per pass, and the corresponding auxiliary fluid inlet and pass-to-pass directions (see Figure  7.25.6). Macros are numbered from $0$ to ( $n-1$) in the direction of auxiliary fluid flow, where $n$ is the number of macros.

Figure 7.25.6: $1 \times 4 \times $3 Macros
figure

In the Heat Exchanger Model panel, in the Geometry tab, specify the Number of Passes, the Number of Rows/Pass, and the Number of Columns/Pass. The model will automatically extrude the macros to the depth of the heat exchanger core. For each pass, the Number of Rows/Pass are defined in the direction of the auxiliary flow inlet direction and the Number of Columns/Pass are defined in the direction of the pass-to-pass direction.

figure   

The Number of Rows/Pass, as well as the Number of Columns/Pass must be divisible by the number of cells in their respective directions.

Viewing the Macros

You can view the auxiliary fluid path by displaying the macros. To view the macros for your specified Number of Passes, Number of Rows/Pass, and Number of Columns/Pass, click the Apply button at the bottom of the panel. Then click View Passes to display it. The path of the auxiliary fluid is color-coded in the display: macro $0$ is red and macro $n-1$ is blue.

For some problems, especially complex geometries, you may want to include portions of the computational-domain grid in your macros plot as spatial reference points. For example, you may want to show the location of an inlet and an outlet along with the macros. This is accomplished by turning on the Draw Grid option. The Grid Display panel will appear automatically when you turn on the Draw Grid option, and you can set the grid display parameters there. When you click on View Passes in the Heat Exchanger Model panel, the grid display, as defined in the Grid Display panel, will be included in the macros plot (see Figure  7.25.7).

Figure 7.25.7: Grid Display With Macros
figure



Selecting the Heat Exchanger Model


You can specify the model for your heat exchanger by selecting the ntu-model or the simple-effectiveness-model from the Heat Transfer Model drop-down list in the Model Data tab.



Specifying the Auxiliary Fluid Properties and Conditions


To define the auxiliary fluid properties and conditions, you will specify the Auxiliary Fluid Flow Rate ( $\dot{m}$) in the Auxiliary Fluid tab. The properties of the auxiliary fluid can be specified using the Auxiliary Fluid Properties Method drop-down list. You can choose a Constant Specific Heat ( $c_p$) and set the value in the Auxiliary Fluid Specific Heat field below, or as a user-defined function for the enthalpy using the User Defined Enthalpy option and selecting the corresponding UDF from the Auxiliary Fluid Enthalpy UDF drop-down list.



Setting the Pressure-Drop Parameters and Effectiveness


The pressure drop parameters and effectiveness define the Core Porosity Model. If you would like FLUENT to set the porosity of this a heat exchanger zone using a particular core model, you can select the appropriate model. This will automatically set the porous media inputs. There are three ways to specify the Core Porosity Model parameters:

If you do not choose a core porosity model, you will need to set the porosity parameters in the boundary conditions panel for the heat exchanger zone(s). To do this, follow the procedures described in Section  7.19.6.

The models you define will be saved in the case file.

Using the Default Core Porosity Model

FLUENT provides a default model for a typical heat exchanger core. To use these values, simply retain the selection of default-model in the Core Porosity Model drop-down list in the Heat Exchanger Model panel. (You can view the default parameters in the Heat Exchanger Model panel, as described below.)

The default-model core porosity model is a list of constant values from the Heat Exchanger Model panel. These constants are used for setting the porous media parameters.

Defining a New Core Porosity Model

If you want to define pressure-drop and effectiveness parameters that are different from those in the default core porosity model, you can create a new model. The steps for creating a new model are as follows:

1.   Click the Edit... button to the right of the Core Porosity Model drop-down list, for which default-model should have been selected. This will open the Core Porosity Model panel (see Section  7.25.3) (Figure  7.25.8).

Figure 7.25.8: The Core Porosity Model Panel
figure

2.   Enter the name of your new model in the Name box at the top of the panel.

3.   Under Gas-Side Pressure Drop, specify the following parameters used in Equation  7.25-2:

Minimum Flow to Face Area Ratio   ( $\sigma$)

Entrance Loss Coefficient   ( $K_c$)

Exit Loss Coefficient   ( $K_e$)

Gas-Side Surface Area   ( $A$)

Minimum Cross Section Flow Area   ( $A_c$)

and the Core Friction Coefficient and Core Friction Exponent ( $a$ and $b$, respectively, in Equation  7.25-3).

4.   Click the Change/Create button. This will add your new model to the database.

Reading Heat Exchanger Parameters from an External File

You can read parameters for your Core Porosity Model from an external file. A sample file is shown below:

("modelname"
  (0.73 0.43 0.053 5.2 0.33 9.1 0.66))

The first entry in the file is the name of the model (e.g., modelname). The second set of numbers contains the gas-side pressure drop parameters:

( $\sigma$ $K_c$ $K_e$ $A$ $A_c$ $a$ $b$)

To read an external heat exchanger file, you will follow these steps:

1.   In the Core Porosity Model panel, click on the Read... button.

2.   In the resulting Select File dialog box, specify the HXC Parameters File name and click OK. FLUENT will read the core porosity model parameters, and add the new model to the database.

Viewing the Parameters for an Existing Core Model

To view the parameters associated with a core porosity model that you have already defined, select the model name in the Database drop-down list (in the Core Porosity Model panel). The values for that model from the database will be displayed in the Core Porosity Model panel.


next up previous contents index Previous: 7.25.2 Heat Exchanger Model
Up: 7.25 Heat Exchanger Models
Next: 7.25.4 Using the Heat
© Fluent Inc. 2006-09-20