Hello and welcome! In this workshop we will demonstrate how to generate a poly-hexcore volume mesh in an electronics enclosure, using
the Watertight Geometry Workflow in Ansys Fluent Meshing, for a conjugate heat transfer analysis. During the workshop, we will explore
how to add local size controls such as BOI, curvature, and face sizing. We will also demonstrate how to add boundary layer mesh
and improve the volume mesh quality. Let’s get started!
Launch Ansys Fluent in Meshing mode and select the watertight geometry workflow. Begin with importing the CAD geometry of the PCB
enclosure while keeping the units in mm, which is the same units in which the geometry was created. To be able to see the inside of the
enclosure, select the fluid surface and click on ‘Transparency’. The geometry we have here is that of a Printed Circuit Board placed inside an
enclosure. The model also consists of fans and heat sinks which are used to facilitate an effective thermal management of the PCB. To
analyze the air flow within the PCB enclosure, the fluid volume has been extracted during the CAD creation phase. The CAD geometry has
been prepared using ANSYS Spaceclaim and all the necessary operations such as adding of Bodies of Influence around heat sinks are
performed to make it ready for meshing in watertight geometry workflow. In the Add Local Sizing task, select ‘yes’ to add
local mesh size controls. First let’s assign the Body of Influence size control to the two BOI regions that enclose the two heat sinks.
Change the ‘Target Mesh Size’ to 1.5mm and keep all other settings as default and click ‘Add Local Sizing’. Notice that the BOI regions
disappear once the BOI local sizing is applied. This is because, the BOIs are not a part of the geometry to be simulated, and are instead
used to demarcate a local region, in which mesh of a specific size is created. Generally, the mesh in BOI is of a finer size than the
surrounding, to accurately capture the flow physics in that region. Next, apply curvature size control to capacitor, hub walls, inlet and
outlet surfaces to accurately resolve the curved surfaces of these geometrical features. Enter the ‘Local Min Size’, ‘Max Size’ and ‘Curvature
Normal Angle’ values as shown. Finally, face sizing is applied to the fans with a target mesh size of 1mm to ensure that fan geometry is well
captured. The next step is to generate the surface mesh for the model. The minimum and the maximum sizes are changed to 0.5mm and
4mm respectively while the ‘Cells per Gap’ is set to 2 and the Proximity size function is scoped to ‘faces and edges’. This ensures that
thin regions in the model, such as the fins of the heat sink and the thickness of the enclosure are filled with atleast 2 cells across
their thickness, which allows to better capture the thermal gradients when simulating the model. Once satisfied with the inputs, execute
the task to create surface mesh. Once the surface mesh has been generated, we need to inform the workflow the type of geometry we
are working with. The geometry here consists of solid, fluid and void regions. There is no need to cap openings to extract fluid regions
and to apply share topology, however we will change any fluid-fluid interfaces to the type ‘internal’. There are no changes to be made in
the ‘Update Boundaries’ task because the Watertight workflow correctly identifies the appropriate boundary conditions that need to
be employed on the boundary surfaces based on their labels assigned during the CAD creation phase. In the ‘Create Regions’ task,
change the ‘Estimated Number of Fluid Regions’ from 2 to 1, as it is known that there is only one fluid region which is occupying the
empty space within the solid enclosure. The console reports a warning which says that 2 fluid regions were identified instead of one.
This is because, in this case, the workflow identifies the enclosure also as a fluid region. The enclosure can be changed to solid region
type in ‘Update Regions’ task. Also, the workflow automatically detects the void region which is assigned the ‘dead’ region type. Since
our aim is to generate a mesh to perform a conjugate heat transfer analysis of the model, it is generally recommended to add boundary
layer mesh even in the solid region, in addition to the walls in the fluid region of the model, to avoid large cell jumps across solid-fluid
interfaces. Using the ‘Add Boundary Layers’ task, let’s add 10 layers of boundary layer mesh in the fluid region on all the wall-type
boundaries, with last-ratio as the ‘Offset Method Type’ and 0.05mm as the height of the first layer. We will further add three layers of the
boundary layer mesh in the solid regions at solid-fluid interfaces with the same settings as fluid region boundary layer mesh. Execute the
task and move to the ‘Generate the Volume Mesh’ task. We will use the poly-hexcore ‘Fill With’ method to fill the volumetric regions. This
model supports the use of poly-hexcore ‘Fill With’ method for two reasons, firstly because the model consists of structured quad shapes
and secondly, the dominant direction of the fluid flow is expected to be along one of the coordinate axes. Leave the rest of the settings
to default and generate the volume mesh. After the volume mesh has been generated, it can be inspected by using the clipping plane.
Notice the boundary layer mesh is created along the walls in the fluid region, and along the solid-fluid interface in the solid regions. The
orthogonal quality of the mesh, as reported in the console, is 0.09. Since the recommended quality is 0.1 or greater, it is recommended to
improve the mesh quality. For this, the workflow provides the ‘Improve Volume Mesh’ task which can be accessed by right-clicking on the
‘Generate the Volume Mesh’ task. Retain the default settings and click on ‘Improve Volume Mesh’. Notice that the orthogonal quality has
now improved to a value of 0.15. The mesh is now ready to be exported to the Fluent solver for CFD analysis. That brings us to the end of
the workshop.