PDF
Convective Flow in a Heat Exchanger Plate
Introduction
An evenly distributed flow is necessary to achieve good thermal performance in plate heat exchangers. The flow distribution can be controlled by the design of the inlet and outlet manifolds that connect the plate channels.
Modeling the detailed flow within the channels of a plate heat exchanger can be computationally costly, or even prohibitive. However, it is often sufficient to describe the flow with a lumped pipe flow model. This way the computational time and memory requirements can be significantly reduced. The model presented here shows such an approach where a Pipe Flow interface, solving for the velocity and pressure in the plate channels, is coupled to a Laminar Flow interface, that solves for the 3D flow and pressure in the inflow and an outflow manifolds.
Figure 1: Plate heat exchanger assembly with stacked plates. Image courtesy of Varem S.p.a.
Model Definition
Figure 2 shows the model geometry. The inlet and outlet manifolds are 2 mm wide, 1 mm high, and 85 mm long. The microchannels have a square cross section with a side of 1 mm. They are drawn as edges in the 3D geometry.
Figure 2: Five microchannels, inlet and outlet manifold.
Domain equations
The fluid properties of water are used in both interfaces.
Inlet and Outlet Manifolds
The laminar flow in the manifolds is described by the equations in 3D, set up by the Laminar Flow interface.
Microchannels
The 1D flow in the channels is modeled using the Pipe Flow interface, that calculates the pressure drop over a pipe and the continuity equation according to:
(1)
Where dh is the mean hydraulic diameter (m), given by:
where A is the pipe cross section area (m2) available for flow, and Z is the wetted perimeter (m).
The right hand side of Equation 1 describes the pressure drop due to internal viscous shear and contains the Darcy friction factor, fD. The Pipe Flow interface provides a library of built-in expressions for fD covering laminar and turbulent flow regimes, as well as Newtonian and non-Newtonian fluids.
Boundary conditions
Coupling the 3D flow in the manifolds to the 1D flow in the channels is easily done with the multiphysics coupling Pipe Connection.
An fully developed flow boundary condition with average velocity of 5 cm/s is set at the manifold inlet. On the manifold outlets, facing the microchannel inlets, a pipe connection multiphysics feature sets up appropriate conditions automatically.
Figure 3: The connection between the pipe segment and the 3D flow domain is easily done with the multiphysics coupling Pipe Connection.
Results and Discussion
Figure 4 shows the pressure distribution in the model. The microchannels contribute to the major part of the pressure drop.
Figure 4: The main pressure drop occurs the microchannels.
Figure 5 shows the velocity in the microchannels. The velocity is lower in the central channels, reducing the heat exchange efficiency in this region. A change in the manifold design would be necessary for a more uniform flow distribution in the plate channels.
Figure 5: Flow velocity magnitude in the microchannels.
Application Library path: Pipe_Flow_Module/Tutorials/heat_exchanger_plate
Modeling Instructions
From the File menu, choose New.
New
In the New window, click  Model Wizard.
Model Wizard
1
In the Model Wizard window, click  3D.
2
In the Select Physics tree, select Fluid Flow>Single-Phase Flow>Pipe Flow (pfl).
3
Click Add.
4
In the Select Physics tree, select Fluid Flow>Single-Phase Flow>Laminar Flow (spf).
5
Click Add.
6
Click  Study.
7
In the Select Study tree, select General Studies>Stationary.
8
Click  Done.
Geometry 1
Insert the prepared geometry sequence from file. You can read the instruction for creating the geometry in the appendix.
1
In the Geometry toolbar, click  Insert Sequence.
2
Browse to the model’s Application Libraries folder and double-click the file heat_exchanger_plate_geom_sequence.mph.
3
In the Geometry toolbar, click  Build All.
Definitions
Add Material
From the Home menu, choose Add Material.
Add Material
1
Go to the Add Material window.
2
In the tree, select Built-in>Water, liquid.
3
Click Add to Component in the window toolbar.
4
Click Add to Component in the window toolbar.
5
From the Home menu, choose Add Material.
Materials
Water, liquid 1 (mat2)
1
In the Settings window for Material, locate the Geometric Entity Selection section.
2
From the Geometric entity level list, choose Edge.
3
From the Selection list, choose Array 1.
Pipe Flow (pfl)
1
In the Model Builder window, expand the Component 1 (comp1)>Definitions node, then click Component 1 (comp1)>Pipe Flow (pfl).
2
In the Settings window for Pipe Flow, locate the Edge Selection section.
3
From the Selection list, choose Array 1.
Fluid Properties 1
No settings are needed for the fluid properties because these are retrieved from the material.
Pipe Properties 1
1
In the Model Builder window, click Pipe Properties 1.
2
In the Settings window for Pipe Properties, locate the Pipe Shape section.
3
From the list, choose Square.
4
In the wi text field, type 1[mm].
Laminar Flow (spf)
Now set up the Laminar Flow interface. Again, the fluid properties are taken from the material.
1
In the Model Builder window, under Component 1 (comp1) click Laminar Flow (spf).
Inlet 1
1
In the Physics toolbar, click  Boundaries and choose Inlet.
2
Select Boundary 43 only.
3
In the Settings window for Inlet, locate the Boundary Condition section.
4
From the list, choose Fully developed flow.
5
Locate the Fully Developed Flow section. In the Uav text field, type 5[cm/s].
Outlet 1
1
In the Physics toolbar, click  Boundaries and choose Outlet.
2
Select Boundary 5 only.
3
In the Settings window for Outlet, locate the Pressure Conditions section.
4
Select the Normal flow check box.
Multiphysics
Pipe Connection 1 (plc1)
In the Physics toolbar, click  Multiphysics Couplings and choose Global>Pipe Connection.
Mesh 1
1
In the Model Builder window, under Component 1 (comp1) click Mesh 1.
2
In the Settings window for Mesh, locate the Physics-Controlled Mesh section.
3
From the Element size list, choose Finer.
4
Click  Build All.
Size
Right-click Component 1 (comp1)>Mesh 1 and choose Edit Physics-Induced Sequence.
Size 2
1
In the Settings window for Size, locate the Element Size section.
2
From the Predefined list, choose Normal.
Study 1
1
In the Model Builder window, click Study 1.
2
In the Settings window for Study, locate the Study Settings section.
3
Clear the Generate default plots check box.
4
In the Home toolbar, click  Compute.
Create the result plots shown in Figure 4 and Figure 5 following these steps:
Results
3D Plot Group 1
In the Home toolbar, click  Add Plot Group and choose 3D Plot Group.
Volume 1
1
Right-click 3D Plot Group 1 and choose Volume.
2
In the Settings window for Volume, locate the Expression section.
3
In the Expression text field, type p2.
4
Click to expand the Range section. In the 3D Plot Group 1 toolbar, click  Plot.
Pressure
1
In the Model Builder window, under Results click 3D Plot Group 1.
2
In the Settings window for 3D Plot Group, type Pressure in the Label text field.
Line 1
1
Right-click Pressure and choose Line.
2
In the Settings window for Line, locate the Expression section.
3
In the Expression text field, type p-1[atm].
4
In the Pressure toolbar, click  Plot.
5
Locate the Coloring and Style section. Clear the Color legend check box.
6
From the Line type list, choose Tube.
7
In the Tube radius expression text field, type 0.5.
8
Select the Radius scale factor check box.
9
From the Color table list, choose RainbowLight.
10
Click the  Show Grid button in the Graphics toolbar.
11
In the Pressure toolbar, click  Plot.
12
Click the  Zoom Extents button in the Graphics toolbar.
Velocity
1
Right-click Pressure and choose Duplicate.
2
In the Settings window for 3D Plot Group, type Velocity in the Label text field.
Line 1
1
In the Model Builder window, expand the Velocity node, then click Line 1.
2
In the Settings window for Line, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1)>Pipe Flow>pfl.U - Velocity magnitude - m/s.
3
Click to expand the Range section. Locate the Coloring and Style section. Select the Color legend check box.
4
In the Velocity toolbar, click  Plot.
Volume 1
1
In the Model Builder window, right-click Volume 1 and choose Disable.
2
Click the  Zoom Extents button in the Graphics toolbar.
Creating the Geometry
The previously inserted geometry can be created from scratch like this:
Add Component
In the Home toolbar, click  Add Component and choose 3D.
Global Definitions
Parameters 1
1
In the Model Builder window, under Global Definitions click Parameters 1.
2
In the Settings window for Parameters, locate the Parameters section.
3
In the table, enter the following settings:
Name
Expression
Value
Description
Lp
190[mm]
0.19 m
Pipe length
Geometry 1
1
In the Model Builder window, under Component 1 (comp1) click Geometry 1.
2
In the Settings window for Geometry, locate the Units section.
3
From the Length unit list, choose mm.
Work Plane 1 (wp1)
1
In the Geometry toolbar, click  Work Plane.
2
In the Settings window for Work Plane, locate the Plane Definition section.
3
In the z-coordinate text field, type 0.5.
Work Plane 1 (wp1)>Plane Geometry
In the Model Builder window, click Plane Geometry.
Work Plane 1 (wp1)>Line Segment 1 (ls1)
1
In the Work Plane toolbar, click  More Primitives and choose Line Segment.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
From the Specify list, choose Coordinates.
4
Locate the Endpoint section. From the Specify list, choose Coordinates.
5
Locate the Starting Point section. In the yw text field, type 0.5.
6
Locate the Endpoint section. In the xw text field, type Lp.
7
In the yw text field, type 0.5.
8
Click  Build Selected.
9
Click the  Zoom Extents button in the Graphics toolbar.
Create an array of the curve and enable Create selections to facilitate selection later on in the physics settings.
Array 1 (arr1)
1
In the Model Builder window, right-click Geometry 1 and choose Transforms>Array.
2
Select the object wp1 only.
3
In the Settings window for Array, locate the Size section.
4
In the y size text field, type 5.
5
Locate the Displacement section. In the y text field, type 20.
6
Locate the Selections of Resulting Entities section. Select the Resulting objects selection check box.
7
From the Show in physics list, choose Edge selection.
Create the inlet and outlet manifolds using blocks.
Block 1 (blk1)
1
In the Geometry toolbar, click  Block.
2
In the Settings window for Block, locate the Size and Shape section.
3
In the Width text field, type 2.
4
Locate the Position section. In the x text field, type -2.
5
Click  Build Selected.
6
Click the  Zoom Extents button in the Graphics toolbar.
Block 2 (blk2)
1
Right-click Block 1 (blk1) and choose Duplicate.
2
In the Settings window for Block, locate the Position section.
3
In the x text field, type Lp.
4
Click  Build Selected.
Array 2 (arr2)
1
In the Geometry toolbar, click  Transforms and choose Array.
2
Select the objects blk1 and blk2 only.
3
In the Settings window for Array, locate the Size section.
4
In the y size text field, type 5.
5
Locate the Displacement section. In the y text field, type 20.
6
Click  Build Selected.
Block 3 (blk3)
1
In the Model Builder window, under Component 1 (comp1)>Geometry 1 right-click Block 2 (blk2) and choose Duplicate.
2
In the Settings window for Block, locate the Size and Shape section.
3
In the Depth text field, type 85.
4
Locate the Position section. In the x text field, type -4.
5
Click  Build Selected.
Block 4 (blk4)
1
Right-click Block 3 (blk3) and choose Duplicate.
2
In the Settings window for Block, locate the Position section.
3
In the x text field, type Lp+2.
4
In the y text field, type -4.
5
Click  Build Selected.
Form Composite Domains 1 (cmd1)
1
In the Geometry toolbar, click  Virtual Operations and choose Form Composite Domains.
2
On the object fin, select Domains 1–12 only.
3
In the Geometry toolbar, click  Build All.