structured domains
 

Hello Guys,
How can i create a structured domain for my simple 2D Geometry? How should i define the Domain and mesh it? Left edge is Velocity inlet and right edge is pressure outlet. The circle is wall. I hope that someone can help me.
Thanks!

While this topology is possible with a single O-grid, I prefer to mesh it with 12 domains - as seen in the attached picture. Sounds like a lot more but it doesn't take much effort and you can achieve a much higher quality mesh around the circle and in the wake.

-Chris

Hello Chris,
Thanks for your answer you helped me a lot. My plan was also to create the Domain like the one you created. I am already created a domain around the cylinder. I want to know how you could create 12 Domains in a rectangle.
I appreciate if you could help me.

My general steps are:

1) Create the rectangular box around the circle with 4 connectors (don't worry about dimension and spacings yet)

2) Split the circle connectors (and/or domains) around the circle in 90 deg increments - as shown in mine. Be sure to have the first point 45 deg above the horizontal.

3) Split each of the 4 connectors from step 1 at two locations. The two locations will correspond to the two closet split points on the circle. When splitting a connector, you will notice that the split marker can only slid along the connector however you can still move the cursor unrestricted. Use this to your advantage by moving the cursor to one of the two closest circle split points until the snap circle highlights on your cursor and click on the circle split location. By doing this, the split location on the connector will line up with the split location on the circle.

4) Draw 2-point connectors from each new split location from step 3 to it's corresponding point on the circle.

5) Finally, adjust dimensions and spacing on the new connectors from preceding 4 steps so structured domains can be assembled.

Let me know if you have any more questions, Chris

Hi,

I am also meshing this similar kind of geometry, but it's 3D.
I mesh the geometry with 14 blocks, 4 blocks around each cylinder, another 6 in the upsteam, middle and downstream of the channel.

Now I am a little confused about setting the boundary, exactly the domains on the symmetry plane. Should i see it as boundary or not.
If so, how should i give boundary to the symmetry plane? like interface or something else, but i cannot find it in Gridgen boundary settings.

If I don't set give boundary on the symmetry plane, wrong results will emerge when i do the simulation.

Thanks.

You should not have to nor need to set a CAE boundary condition on the symmetry because it will ultimately be part of the internal mesh, i.e. flow through.

@ Chris , it worked. thank you ever so much!

Thank you, Chris.

Hi jimbean!

Don't be confused by the geometric symmetry. The flow field is not symmetrical so you can't use this plane as a symmetry plane and set BC for symmetry.

boundary conditions
 

Hi
I have a question about boundary conditions.
Now i have 12 domains in Pointwise. in ansys, i get 3 different faces as inlet. I want to determine the inlet boundary condition for faces together. How can i connect these domains into a single boundary conditions?
Thanks!

In pointwise, you can select domains that are adjacent to each other and join them.

You group together multiple domains to form a single, coherent boundary condition in the CAE>Set Boundary Conditions menu. Be sure to set your solver first (CAE>Set Solver) because the BC physical types will be solver specific.

In short, go to the panel I mention, create a BC (click New), select the domains that form the BC you want (e.g. inlet), click in the check box in your new BC's row to assign them. Repeat for remaining BCs.

The same idea applies in 3D for blocks with volume conditions. For some solvers, volume conditions aren't necessary but others the are, e.g. Fluent. Because Pointwise allows one to create multiple 3D mesh regions, called blocks, but often represent a single fluid (or solid) region, blocks can be assigned to a single "volume condition". This is done is similar manner as boundary conditions.

I would not recommend joining domains just to get the boundary conditions you desire in the solver. First, because it's not always possible to join structured domains due to topology. Second, because it can be more difficult to modify you mesh subsequently. Third, because getting the boundary conditions you desire is best accomplish by the above procedure.

Good luck. Let me know if have any more questions.

-Chris

Chris you're right and your help is always invaluable.
This is a simple domain though and that's why I said he could join the three domains together.