13.3.2. Using the Ungrouped Macro Heat Exchanger Model

The heat exchanger model settings may be written into and read from the boundary conditions file (Reading and Writing Boundary Conditions) using the text commands, file/write-settings and file/read-settings, respectively. Otherwise, the steps for setting up the ungrouped macro heat exchanger model is as follows:

  1. Read the mesh and make sure that the inlet and outlet for the heat exchanger are two separate zones.

  2. Enable the calculation of energy in the Energy Dialog Box.

     Setup → Models → Energy   ON

  3. Enable the Ungrouped Macro Model option and click the Define... button in the Heat Exchanger Model Dialog Box (Figure 13.12: The Heat Exchanger Model Dialog Box) to access the Ungrouped Macro Heat Exchanger dialog box.

     Setup → Models → Heat Exchanger   Edit...

    Figure 13.12:  The Heat Exchanger Model Dialog Box

    The Heat Exchanger Model Dialog Box

  4. Specify the heat exchanger inputs in the Ungrouped Macro Heat Exchanger dialog box.

    Figure 13.13:  The Ungrouped Macro Heat Exchanger Dialog Box Displaying the Model Data Tab

    The Ungrouped Macro Heat Exchanger Dialog Box Displaying the Model Data Tab

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

    2. Under the Model Data tab, choose Fixed Heat Rejection or Fixed Inlet Temperature, as required (Figure 13.13: The Ungrouped Macro Heat Exchanger Dialog Box Displaying the Model Data Tab).

    3. Specify the Heat Transfer Model as either the default ntu-model or the simple-effectiveness-model. See step 3 in Choosing a Heat Exchanger Model for details about the differences between these two models.

    4. Specify the Core Porosity Model if you want ANSYS Fluent to use the pressure loss coefficient function to automatically compute (and update) the porous media coefficients in the cell zones condition dialog box, as described in Streamwise Pressure Drop in the Theory Guide. More information is available in Setting the Pressure-Drop Parameters and Effectiveness.

    5. If the ntu-model is chosen, a Heat Transfer Data... button will appear under Heat Exchanger Performance Data. Clicking the Heat Transfer Data... button will open the Heat Transfer Data Table Dialog Box, where you will enter experimental data that defines how heat transfer values relate to the fluid flow rates (Figure 13.8: The Heat Transfer Data Table Dialog Box). See Specifying Heat Exchanger Performance Data more details.

      Figure 13.14:  The Heat Transfer Data Table Dialog Box for the NTU Model

      The Heat Transfer Data Table Dialog Box for the NTU Model

    6. Enter the Auxiliary Fluid Temperature and the Primary Fluid Temperature for the ntu-model. These are the fixed inlet temperatures at which the test was performed to obtain the heat transfer data.

    7. If the simple-effectiveness-model is chosen, then clicking the Velocity Effectiveness Curve... button, under the Heat Exchanger Performance Data, allows you to set the velocity and corresponding effectiveness for each point. More information is available in Specifying Heat Exchanger Performance Data.

    8. In the Geometry tab, define the heat exchanger macros using the Number of Passes, the Number of Rows/Pass, and the Number of Columns/Pass fields. The Number of Rows/Pass is along the auxiliary flow direction (height) and the Number of Columns/Pass is defined in the pass-to-pass (width) direction. Also, enter the Auxiliary Fluid Inlet Direction and Pass-to-Pass Direction. You may want to snap the plane tool to either the inlet or outlet of the heat exchanger using the Update from Plane Tool. Note that the plane tool must be attached exactly and oriented so that its green arrow points in the auxiliary flow direction, and its blue arrow points in the pass-to-pass direction.


      Important:  To attach the plane tool exactly, exact coordinates (printed in the console by probing) of the three corner nodes must be entered in the plane tool (x0, x1, x2) in a specific order. Also, note that x0 to x1 is the auxiliary flow direction and x1 to x2 is the pass-to-pass direction.


      More information is available in Specifying the Auxiliary Fluid Inlet and Pass-to-Pass Directions and Defining the Macros.

      Figure 13.15:  The Ungrouped Macro Heat Exchanger Dialog Box Displaying the Geometry Tab

      The Ungrouped Macro Heat Exchanger Dialog Box Displaying the Geometry Tab

      Figure 13.16:  The Ungrouped Macro Heat Exchanger Dialog Box Displaying the Auxiliary Fluid Tab

      The Ungrouped Macro Heat Exchanger Dialog Box Displaying the Auxiliary Fluid Tab

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

    10. 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. If user-defined-enthalpy is selected as the Auxiliary Fluid Properties Method, you will need to specify the Inlet Quality and the Pressure Drop. More information is available in Specifying the Auxiliary Fluid Properties and Conditions.

    11. Click Apply in the Ungrouped Macro Heat Exchanger dialog box to save all the settings. Once you click the Apply button, the NTU matrix will be computed from the raw data. Therefore, make sure you click Apply at the very end of your setup.


      Important:  When you click Apply, look for any error or warning message in the ANSYS Fluent console. Some of the common errors you may see displayed are due to the NTU computations not converging. In such cases, check that

      • you have entered the data correctly

      • the values of the data are reasonable

      • the operating condition for the auxiliary fluid flow rate is not too far from the range of the heat transfer data

      Other error messages you may encounter may be due to macros not getting any cells assigned to it. In such cases, make sure that

      • the heat exchanger core is rectangular

      • the directions are correct

      • you are using uniformly spaced cells in both directions

      • the mesh is either a hexahedra or wedge and is structured


    12. Repeat steps (a)–(k) 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 Using the Grouped Macro Heat Exchanger Model.

For additional information, see the following sections:

13.3.2.1. 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.

13.3.2.2. 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.

  • ntu-model: For the ntu-model you will provide the heat transfer for different primary and auxiliary fluid flow rates. Click the Heat Transfer Data... button to open up a tabular dialog box. Set the number of auxiliary flow rates and primary fluid flow rates. The dialog box will resize itself accordingly. You will need to provide various primary fluid flow rates and auxiliary fluid flow rates and the corresponding heat transfer values. You may write this data to a file that can be read later.

  • simple-effectiveness-model: For this model, you will need to provide velocity versus effectiveness data. To provide this you can click the Velocity Effectiveness Curve... button. This will open up a tabular dialog box. In this dialog box, you can set the number of points in the curve, then you can provide velocities and corresponding effectiveness values (note that the effectiveness values must be within the range of 0–1). This data can be written to a file and read back.

13.3.2.3. 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 13.17: 1x4x3 Macros 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 Initializing the Plane Tool 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 the Update from Plane Tool button in the Ungrouped Macro Heat Exchanger dialog box. 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.)

13.3.2.4. Defining the Macros

As discussed in The Macro Heat Exchanger Models, 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 13.17: 1x4x3 Macros). Macros are numbered from to () in the direction of auxiliary fluid flow, where is the number of macros.

Figure 13.17:  1x4x3 Macros

1x4x3 Macros

In the Ungrouped Macro Heat Exchanger dialog box, 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.


Important:  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. For example, if you have 50 cells in the auxiliary flow direction, you can use 25 for the Number of Rows/Pass, but you should not use 26 or 24. If you have 51 cells in that direction, you can only use 51 for the Number of Rows/Pass. The same holds true for the other direction.


13.3.2.4.1. 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 dialog box, then click the View Passes button to display it. The path of the auxiliary fluid is color-coded in the display: macro is red and macro is blue.

For some problems, especially complex geometries, you may want to include portions of the computational-domain mesh 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 enabling the Draw Mesh option. The Mesh Display Dialog Box will appear automatically when you enable the Draw Mesh option, where you can set the mesh display parameters. When you click the View Passes button in the Ungrouped Macro Heat Exchanger dialog box, the mesh display, as defined in the Mesh Display dialog box, will be included in the macros plot (see Figure 13.18: Mesh Display With Macros).

Figure 13.18:  Mesh Display With Macros

Mesh Display With Macros

13.3.2.5. Specifying the Auxiliary Fluid Properties and Conditions

To define the auxiliary fluid properties and conditions, you will specify the Auxiliary Fluid Flow Rate () 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 () 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.

The function should return a single value depending on the index:

  • Enthalpy for given values of temperature, pressure, and quality.

  • Temperature for given values of enthalpy and pressure

  • Specific heat for given values of temperature and pressure

The user-defined function should be of type

 DEFINE_SOURCE(udf_name, cell_t c, Thread *t, real d[n], int index). 

where n in the expression d[n] would be 0 for temperature, 1 for pressure, or 2 for quality. The variable index is 0 for enthalpy, 1 for temperature, or 2 for specific heat. This user-defined function should return

 real value; /* (temperature or enthalpy or Cp depending on index). */ 
  • If you want ANSYS Fluent to compute the auxiliary fluid inlet temperature for a specified heat rejection, follow the steps below:

    1. Enable the Fixed Heat Rejection option in the Model Data tab.

    2. Specify the Heat Rejection ( in Equation 6–15 in the Theory Guide) in the Auxiliary Fluid tab.

    3. Specify the Initial Temperature, which will be used by ANSYS Fluent as an initial guess for the inlet temperature ( in Equation 6–11 and Equation 6–13 in the Theory Guide).

  • If you want ANSYS Fluent to compute the total heat rejection of the core for a given inlet auxiliary fluid temperature, follow the steps below:

    1. Enable the Fixed Inlet Temperature option in the Model Data tab.

    2. Specify the Inlet Temperature ( in Equation 6–11 and Equation 6–13 in the Theory Guide) in the Auxiliary Fluid tab.

  • If you enable the User Defined Enthalpy option under the Auxiliary Fluid Properties Method, you must also specify the Inlet Pressure ( in Equation 6–21 in the Theory Guide) and Inlet Quality ( in Equation 6–20 in the Theory Guide).

13.3.2.6. Setting the Pressure-Drop Parameters and Effectiveness

The pressure drop parameters and effectiveness define the Core Porosity Model. If you would like ANSYS 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:

  • Use the values in ANSYS Fluent’s default model.

  • Define a new core porosity model with your own values.

  • Read a core porosity model from an external file.

If you do not choose a core porosity model, you will need to set the porosity parameters in the cell zone conditions dialog box for the heat exchanger zone(s). To do this, follow the procedures described in User Inputs for Porous Media.

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

13.3.2.6.1. Using the Default Core Porosity Model

ANSYS Fluent provides a default model for a typical heat exchanger core. The default-model core porosity model is a list of constant values from the Ungrouped Macro Heat Exchanger dialog box. These constants are used for setting the porous media parameters. To use these values, simply retain the selection of default-model in the Core Porosity Model drop-down list in the Ungrouped Macro Heat Exchanger dialog box. (You can view the default parameters as described below.)

13.3.2.6.2. 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 Dialog Box (Figure 13.19: The Core Porosity Model Dialog Box).

    Figure 13.19:  The Core Porosity Model Dialog Box

    The Core Porosity Model Dialog Box

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

  3. Under Gas-Side Pressure Drop, specify the following parameters used in Equation 6–2 in the Theory Guide:

    • Minimum Flow to Face Area Ratio ()

    • Entrance Loss Coefficient ()

    • Exit Loss Coefficient ()

    • Gas-Side Surface Area ()

    • Minimum Cross Section Flow Area ()

    and the Core Friction Coefficient and Core Friction Exponent ( and , respectively, in Equation 6–3 in the Theory Guide).

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

13.3.2.6.3. 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 (for example, modelname). The second set of numbers contains the gas-side (primary-side) pressure drop parameters:

( )

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

  1. In the Core Porosity Model dialog box, click the Read... button.

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

13.3.2.6.4. 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 dialog box). The values for that model from the database will be displayed in the Core Porosity Model dialog box.


Release 18.2 - © ANSYS, Inc. All rights reserved.