The Immersed Boundary analysis type, identical to the Conjugate Heat Transfer (CHT) analyses types, allows for the simulation of heat transfer between solid and fluid domains by exchanging thermal energy at the interfaces between them.
However, as opposed to the CHT analyses with a body-fitted mesh the Immersed Boundary Method (IBM) is based on a cartesian grid where the geometry gets immersed into. Therefore it is resilient to geometrical details and does not require CAD simplification even for very complex models.
The IBM analysis type is available in SimScale’s analysis type widget:
Since the solved physics are identical for Immersed Boundary and Conjugate heat transfer analyses this page focuses on the differences between the respective analysis types. Please find a detailed setup guide under Conjugate Heat Transfer Analysis.
Differences Between IBM and CHT Analysis Types
The Immersed Boundary analysis type is currently released under a Beta flag. This means the solver was released very early during active development in order to provide value to our user base and allow for early feedback.
You may find the main features not yet supported by the Immersed Boundary analysis type compared to our CHT analysis type but we are constantly working on closing the feature gap between them.
If you face issues with the solver please share your feedback directly with our team either via the chat functionality, the forum or directly via email.
Not all features of the CHT analysis types are yet supported but will become available in the near future.
Currently external, natural convection analyses and internal flow analyses are separated in the user interface (see next section).
Not all features are listed here e.g. some boundary condition settings are not mentioned explicitly. This is rather a top-level overview.
External vs Internal Analysis
There is an analysis type option ‘Internal flow’ that defines which type of a flow domain you want to simulate.
If Internal flow is toggled ‘off’ (default): You run an external flow, natural convection analysis e.g. the passive cooling of an LED fixture.
If Internal flow is toggled ‘on’: You run an internal flow analysis e.g. fan cooling or liquid cooling of an enclosure.
Defining the Flow Domain
For an external flow, natural convection analysis, the only way to define the flow volume is via a geometry primitive box.
Under the Materials tab assign a fluid material of your choice.
Click on the + icon next to Geometry primitives to create a cartesian box with the appropriate domain size for your simulation. Once the cartesian box is successfully prepared it should appear under the Geometry primitives item in the simulation tree (marked with an arrow).
Now within the fluid material settings assign the primitive to your fluid material.
It is currently not possible to simulate an external flow analysis with Immersed boundary if the external flow box is part of your CAD model e.g. after doing an ‘External’ flow volume operation in CAD mode
If you run an external flow, natural convection analysis, the boundary condition section in the navigation tree is missing. This is intentional as all boundaries of the external flow box get assigned natural convection boundary conditions by default representing an open environment.
Did you know?
If you are running an external flow analysis all space in the box domain that is not covered by solid parts will become flow regions with the defined fluid material. This might be the case for internal cavities etc.
Defining the Flow Domain
For an internal flow simulation you can define the internal flow domain in two ways:
Create ‘Internal caps’ in CAD mode. This operation creates cap faces only for the inlet and outlet openings without creating the full flow region.
Create an ‘Internal’ flow region in CAD mode or import the CAD model including the flow region already.
It is currently not possible to simulate multiple flow channels.
If the model contains additional cavities those become enclosed flow domains with the same fluid material as the internal flow region though same as in the External flow workflow.
The Internal caps operation, in CAD mode, creates cap faces for the inlets and outlets of the internal flow domain and groups them into a sheet body.
The operation is faster and much more robust for complex CAD models than the Internal flow volume operation and is therefore recommended.
You can assign the resulting sheet body containing all bounding faces to the fluid material and use the cap faces for boundary condition assignment the same way you would do it with a ‘complete’ flow region.
In the Workbench, the resulting sheet body is listed under the scene tree with the name Flow volume caps. While defining materials the fluid material should be assigned to this sheet body.
Similarly while defining boundary conditions the cap faces resulting from the internal caps operation are available for assignment.
The Immersed Boundary simulations are based on Cartesian meshes. These do not resolve every part separately as in a body-fitted meshing approach, but refine the cartesian grid towards geometrical and topological details and immerse the geometry into it. The detailed treatment is done on the solver level instead.
The above-discussed meshing approach has some strong advantages:
Very flexible mesh sizing from very coarse to very fine for all levels of CAD complexity.
Automatic defeaturing of small geometrical details.
Perfect hexahedral mesh.
Mesh refinements are physics-based instead of geometry-based.
Flow boundary layers can only be resolved using wall functions instead of boundary layer inflations used for body-fitted meshes.
Cartesian Mesh Settings
The mesh settings for the Immersed Boundary analysis type are as follows:
Number of Cells Per Direction
These settings define how many base mesh cells will be distributed in the mesh along the cartesian axes. Base mesh cells are the mesh cells prior to the refinements around the geometrical parts (Level 0 cells). For external flow analyses, the computational domain is defined by the external flow box primitive. For internal flow analyses, the bounding box of all parts is used.
You can usually leave the default settings and mainly work with refinements in case adjustments are needed. It is advantageous to adapt the cells in one direction though if:
The geometry dimensions in this direction are considerably bigger than the others.
There are very thin components oriented in this direction.
Main physical gradients are expected in this direction e.g. the gravity direction in natural convection analyses.
Refinement Strategy and Refinement Control
The refinement strategy defines how the cells adjacent to the geometry surface need to be refined both inside and outside of the geometry. There are two choices available:
Refinement propagation layers (default): The distance from the geometry is defined by the size of the base mesh cells (See Number of cells per direction). The Refinement control specifies the number of base mesh cells that should define this distance. This refinement strategy defines the distance relative to the overall mesh size and therefore doesn’t require a good knowledge of a reasonable absolute distance.
Distance from surface: The distance from the geometry is defined by an absolute distance value for ‘Refinement control’ measured in a respective length unit. Only base mesh cells that have their cell center within this distance will be considered for refinements. It gives you very detailed control but requires a good understanding of a reasonable value for the respective geometry.
Number of Refinement Levels
This setting defines the highest refinement level that will be applied close to the geometrical surfaces. The mesh size will transition from the lowest level 0 to the defined maximum number within the distance defined under Refinement strategy and Refinement control. Note that every refinement creates 8 refined cells out of one lower level cell. So mesh sizes can increase fast with this setting. The maximum allowed value is 10.