[bboynido]

Hey
I posted a thread last week asking about how to chose a good domain when meshing a helicopter.After careful research I found that for a helicopter it's better to chose a spherical domain.So I did the mesh with a spherical enclosure and I applied a sphere of influence and a wake box into the mesh along with 5 layers of inflation.
Everything looks good but when I loaded the mesh into Fluent I did not know how to chose my inlet and outlet for the boundary conditions.

Do I have to set a velocity direction as a boundary condition,or should I go back and set the inlet and outlet before loading the mesh into Fluent?

Please help me

This is my mesh for the helicopter

[scipy]

It's always a good idea to split your domain walls into zones before going into Fluent. This can be done either in DesignModeler (if you've used it to create the enclosure or do some geometry preparation) or in ANSYS Meshing. I usually opt for the ANSYS Meshing because it's much easier and less time consuming (it's enough to right mouse click a face zone and create named selection, while in DM you have to create a named selection feature, then select faces then click generate).

As far as your question goes: if your half-sphere face zone is already split from the rest of the walls in the domain (the helicopter walls and the symmetry plane) then it doesn't really matter where the "inlet/outlet" name is assigned - it can be done in Fluent or in ANSYS Meshing. But you don't seem to have "carefully researched"

The appropriate boundary condition for a half-spherical domain is a "pressure far-field". There is no inlet/outlet per say... the flow direction is specified as components of X/Y/Z (cosine of angle of attack for example.. if you had an angle of attack or helicopter pitch of 2° then X component would be cos(2°) and Y (or Z, depending on your orientation) component would be sin(2°)). The flow can be entering or exiting through the whole far-field zone depending on the direction. So, the first half (quater) of the half-sphere is the "inlet", while everything behind the "zero meridian" is the outlet. The velocity is specified as a Mach number. That's about it.

[bboynido]

Good evening Scipy

I'm so grateful for your help.Actually I did watch the "Ahmed car body" series and a lot of other videos during my research and they were really helpful.the problem is that I did not find a single tutorial that shows how to do a CFD simulation for a helicopter using Ansys meshing. I am used to work on a rectangular domain where I create named selections for faces and then Fluent recognize them as boundary conditions.Your response was very helpful because you corrected a wrong thought that I used to think of.I thought that Fluent needs a specific face as a starting point for the calculation.
So when I loaded the mesh in Fluent, I only found symmetries, walls and interior solid and all of those are fixed and doesn't allow modifications,I had in mind that I will be setting a flow direction but I did not know where to do that.
So I did split the domain into zones,the body of the helicopter ,the symmetry,and the face of the sphere as a symmetry-side in order to eliminate any wall reactions so it's not a real symmetry it's just for Fluent to optimize the simulation as I saw in most of the simulations ...
Thanks a lot for helping me.
It's my second month since since I started using Ansys and I don't know if my meshing is good or not, it contains about 5 million elements and 900000 nodes ,the radius of the domain is 4 times the length of the helicopter ... so do you think that I can improve it?

[scipy]

You can leave the symmetry-side name but you have to change the type of the boundary condition in FLUENT to pressure far-field. I think FLUENT would automatically assign this type of BC if you named it "farfield" or something. Doesn't really matter though, as long as we understand that it's not really a symmetry BC any more and that it's actually the only inlet/outlet you need.

Domain size sounds OK to start with, you may investigate a larger domain later on to see if it influences the results in any way. Mesh size also sounds reasonable for a symmetric case of external aero but the economy of the mesh could probably be improved. It seems overly refined at the front for example, and you might not need the details such as the shaft hole on the rear vertical fin etc. Also, check if your y+ is within a reasonable range for the usage of wall functions and then maybe refine the areas that need refinement so it's within 30-300 range.

[bboynido]

I did change the type of boundary for the symmetry-side to pressure fare-field in FLUENT as shown in the pictures(I set the mach number to be 3 and an angle of attack of 2°).

I eliminate the mesh size in the front ( these are the statistics as shown in the picture below).

for the shaft hole on the rear vertical fin, it is actually the shaft itself and not just a hole , that's why I thought that it can affect the aerodynamic body as it is a 3D detail.(below you find a picture of the conception that shows all the details).

After setting all the parameters and doing a hybrid simulation ,I ran calculations but it stopped and an error pop up saying that pressure far-fields only works for ideal gazes even though I am using air as a fluid(as you can see in the picture below).
What do you think is the reason for this error?

[scipy]

I don't really know. It should work. Chances are you screwed up somewhere in the setup. Make sure material air is assigned to your fluid zone, you don't really need to use ideal gas law, since helicopters fly at relatively low Ma you can treat the whole simulation as incompressible.

[bboynido]

I checked the fluid material twice and made sure that it is setting to be air.Then I ran a hybrid initialization and nothing came up all the 10 iterations brought zeros ,and again I ran the calculation and the message popped out!
I went back and changed the fluid material to be ideal gas and this time it worked for the hybrid simulation and i got preliminary meaningful values, So I ran the whole calculation using ideal gas.

Would this change the results dramatically ?

[scipy]

It shouldn't change the results in any noticeable way (since effects of compressibility don't really come into play at ).

[bboynido]

That make sense since the actual Ma=0.18 in my case , and I chose to ran it with Ma=0.3 to ensure that the values are in the margin of safety for my case.Based on that it won't change the values as you said