[Bubble the Tea]

Hey everyone, I'm very new to Ansys and currently trying to create a tetrahedral mesh with a "inflation" of 7 layers and a total thickness of 3.5 mm for CFD (college assignment). I've been struggling to achieve this specific configuration because the resulting mesh's quality appears in red no matter what size I input in "element size" (a couple classmates told me that red means the mesh wont work on simulations). i'm also limited because of my ansys student licence which only allows for meshes with 512k cells/nodes, so my minimum element size seems to be around 250mm. I dont really know what do to and would really appreciate some guidance or tips on how to set up the mesh parameters correctly.

P.s: Someone told me to change the inflation settings but it's mandatory to have those 7 layers and 3.5mm Total thickness
gas 3.JPG
gas 4.JPG

And here are the sketches of the 3d model
gas 1.JPG
gas 2.JPG

[SimulationLearner]

Try to change the method of meshing. You can do this by right-click on the "mesh" icon on the left side of the screen, then "insert", then choose "method.
In the details menu try to change the dominant method to "Hex Dominant". You can also try to cange the method to "MultiZone" but it's a little bit more complicated.

[siw]

Seems like a simple volume to mesh, so it is odd that you're having issues.

MultiZone might not work because of the radii. Hex-dominant is not a recommended method for CFD because the elements at the core of the interior will have low quality, it's really a mesh method for FEA.

Looks like you are going to use Fluent for the CFD. Why do you not use Fluent Meshing? A poly-hexcore mesh will keep the element quantity low for your Student Version, and lower than if you make a tetra-prism mesh based on the same sizings.

There are many very useful Fluent Meshing courses at https://courses.ansys.com/index.php/fluids/. Recommend you watch them all (in order) as this will help with your future CFD.

[siw]

The Ansys 2024 R1 Student Version says you can have up to 1 million nodes for CFD: https://www.ansys.com/academic/students/ansys-student. Not sure where your 250 mm element size comes from, when your image shows the geometry is 200 mm x 200 mm x 500 mm, so I guess it must be a typo.

A first cell height of 0.271 mm gives a total inflation height of 3.5 mm with 7 layers and the default growth rate of 1.2.

Global mesh element size of 3 mm and made about 737,000 nodes / 2.2 million elements. Maximum skewness is < 0.8, so it is good.

Be careful with Element Quality metric, as it is different for different element types. Instead, look at aspect ratio, skewness and orthogonal quality.

Didn't take long to make your geometry in SpaceClaim and a tetra-prism mesh in Ansys Meshing. If it was my simulation, I'd use Fluent Meshing for a poly-hexcore mesh.