Unwanted bias while meshing a tube with sweep and inflation
 

Hello,

I want to mesh the inner space of half a tube in ANSYS Meshing. For simulating turbulence and heat transfer I need to inflate the inner tube wall. I have used an o-blocking strategy to generate sweepable bodies. The surface mesh normal to the flow direction looks quite fine. But in flow direction there is an unintended condensation of cell size, for which I don´t know the reason. I even applied local edge sizing controls with both soft or hard behaviour and different bias types and factors but it did not resolve the problem. Has anyone any idea or hint what is going wrong?

Thanks in advance!

sorry, forgot a picture... here it is

First of all, you should apply a "structured mesh" to all the surfaces.
This will eliminate the unstructured mesh at the inlet faces.

In the second step, you could try to reset your mesh data (right-click on the mesh, choose "clear generated data")
This often helps when the Ansys mesher seems to ignore your input when
creating the mesh.
Additionally, you should deactivate the "use advanced size functions" option.
Afterwards, you can generate the mesh anew.

When applying sizing on edges, you should always choose "hard" as behaviour. Otherwise the ansys mesher does whatever it wants, but won't create the mesh you have in mind.

Hope this helps.

BTW: the biasing in wall-normal direction looks a bit hard. The volume jump is definitely too high.

Hello Alex,
thank you very much for your suggestions!

The disabling of advanced size functions solved the described problem but unfortunately at some costs. First of all the surface meshes at the interface between tube and flow now do not match at all (see figure). Even if this point is not so bad it still isn't the optimum. The worse disadvantage is that the bodies around the tube (which I omitted before for simplicity) seem not to be meshable without the usage of advanced size functions (curvature). Even if I could still first mesh the tube, turn the functions on and then mesh the exterior it´s a little annoying... but still, better than before;-)

Regarding the structured mesh: I have tried to achieve it by using local mesh controls with sweep method and free face mesh type set to "All Quad" but still the outcome is the same unstructured surface mesh. Only when I disable the inflation controls (they are attached to the inlet sides) I get a structured mesh. Did you meet a conflict like this before?

Thanks for the additional hints! I am already always clearing the generated data because I got this suspicion too;-)
I wanted to handle the resolution of the boundary layer afterwards or do you think this could also be a reason for the unstructured meshing?

I wasn't aware that you use the automatic inflations.
Switch them off if you want to control the outcome of the mesh.
Use edge sizing with biasing instead.

In my opinion, there are two options when meshing with the ansys mesher. Either you push the button, close your eyes and use the mesh you get.
Or you switch off all the "features" of the mesher like the advanced size functions and handle EVERYTHING yourself.

About the hanging nodes: did you "form a part" of the (frozen) pieces of your geometry in the design modeler?

Well, yes and no: I formed one part out of the 4 pieces for the tube interior while the tube itself is still a seperate piece. I thought this is the appropriate way to form a solid and a fluid part contained in the same model... Or am I wrong?

But anyway, if I do it as you suggested, switch off the inflation controls entirely and use edge sizing instead (also in flow direction with bias factor 1 to avoid again an unintended bias:rolleyes:), it all works out quite fine. I can then even use advanced size functions and therefore mesh all bodies at once. So thank you again for your help! I will be more cautious with advanced functions in the future...

You can do it this way, but it will most certainly result in a non-conformal interface.
Only if the pieces are merged in one part, the ansys mesher will match the nodes at the edges.

Afterwards, you can still define seperate volume regions (fluid and solid) with the named selections in the ansys mesher.

Isn't it working with the "no bias" option?

That is what I initially wanted to have. Tried it and it works (of course...), thanks again! Learned a lot new stuff from just a few posts:)


Ahh, indeed, it is!