Modeling Dual-Stream Heat Exchangers

To use the dual-stream heat exchanger option, you must define the interface between two streams using a common mesh and separate physics continua. One physics continuum represents the hot stream, and the other represents the cold stream.

To model dual-stream heat exchangers:
  1. Import the heat exchanger geometry and define a region topology with six regions that conform to the following structure (actual shapes are determined by the real geometry):


    The diagram shows only one inlet and one outlet for each stream, but you can also specify multiple inlets and outlets for a heat exchanger. The figure below shows a heat exchanger with three inlets and two outlets on the cold stream.


    1. Multi-select all the parts within the Geometry > Parts node, right-click and select Assign Parts to Regions.
    2. In the Assign Parts to Regions dialog, select Create a Region for Each Part and select one of the following in-place interface types:
      • Create Boundary-mode Interfaces From Contacts
      • Create Contact-mode Interfaces From Contacts
      You define internal interfaces between the common boundaries of the regions equivalent to [cold-in] and [cold-core], [cold-core] and [cold-out], [hot-in] and [hot-core], and [hot-core] and [hot-out].




  2. Generate the volume mesh.
  3. Select the Regions > [core] region node, then copy and paste the region.
    You have two overlapping regions with the exact same mesh. The heat transfer occurs in these two regions. For maximum accuracy, ensure that the mesh for the core region is constructed of uniform cells.
  4. Create two physics continua that represent the hot stream, [hot-continuum], and the cold stream fluids, [cold-continuum], and select the following models for each:
    Group Box Model
    Space Three Dimensional
    Material
    • Gas
    • Liquid
    • Solid
    • Multi-Component Gas
    • Multi-Component Liquid
    • Multiphase
    Multiphase Model Volume of Fluid (VOF)—only this multiphase model is compatible with heat exchanger simulations
    Flow Any
    Equation of State Any
    Time
    • Steady
    • Implicit Unsteady
    Energy
    • Segregated Fluid Enthalpy (if you selected the Segregated Flow model)
    • Segregated Fluid Temperature (if you selected the Segregated Flow model)
    • Coupled Energy (if you selected the Coupled Flow model)
    • Segregated Multiphase Temperature (if you selected the Volume of Fluid (VOF) model)
  5. Associate the regions with their corresponding physics continua:
    1. Select the [cold-in], [cold-core], and [cold-out] regions that represent the cold stream and set Physics Continuum to [cold-continuum].
    2. Select the [hot-in], [hot-core], and [hot-out] regions that represent the hot stream and set Physics Continuum to [hot-continuum].
  6. To define the heat exchanger interface, multi-select the [cold-core] and the [hot-core] regions, right-click and select one of the following:
    • Create Interface > Region-Mode Direct Region Interface—use this option if you created boundary-based in-place interfaces between the heat exchanger geometry parts.
    • Create Interface > Contact-Mode Direct Region Interface—use this option if you created per-part contact-based in-place interfaces between the heat exchanger geometry parts. A single heat exchanger interface can represent several part contacts, each of which is treated as a separate heat exchanger, transferring heat between the two parts that constitute the part contact.
    The Interfaces > [heat exchanger] node is created. For more information on the properties, see Heat Exchanger Interface Reference.


  7. Depending on whether you are simulating a single phase or multiphase dual stream heat exchanger, set the heat exchanger method as follows:
    Flow Type Steps
    Single phase Select the Interfaces > [heat exchanger] > Physics Conditions > Heat Exchanger Method node and set Option to one of the following:
    • Inactive—This option indicates that the source terms of the energy equation are not affected.
    • Basic Dual Stream —Unavailable with Contact-Mode Direct Region Interface.
    • Actual Flow Dual Stream

    See The Basic and Actual Dual Stream Heat Exchanger Options for guidelines on choosing between them.
    Volume of Fluid (VOF)
    1. Select the Regions > [cold-core] > Physics Conditions > Energy Source Option node and set Energy Source Option to Volumetric Heat Source.
    2. Select the Physics Values > Volumetric Heat Source node and specify positive volumetric heat flux values for the [cold-core] region.
    3. Select the Regions > [hot-core] > Physics Conditions > Energy Source Option node and set Energy Source Option to Volumetric Heat Source.
    4. Select the Physics Values > Volumetric Heat Source node and specify negative volumetric heat flux values for the [hot-core] region.
  8. Set the heat transfer rate.
    1. Select the Physics Conditions > Heat Exchanger Data Specification node.
    2. Set the Method property. See Heat Exchanger Data Specification Reference for guidelines on choosing the method.
  9. Set target heat rejection, if necessary.
    1. Select the Interfaces > [heat exchanger] > Physics Conditions > Hot Stream Inlet Temperature Specification node (unavailable with Contact-Mode Direct Region Interface).
    2. Set Hot Inlet Temperature to Inferred if you do not want to use the default setting of Specified. See Target Heat Rejection for guidelines on choosing between them.