[davidrobinson50]

Not sure that you quite understood what I meant. I've attached some images to clarify. The stationary region should be hollowed out (like a ring or doughnut shape) and should surround rotating region. This will give you two separate parts, each with it's own interface surface.

Also, it looks like your rotating region has a smaller height that your stationary region. This is fine, but be aware that you will also need to set up interfaces at the top and bottom of the inner cylinder (as well as the curved surface).

[Volumeoffluid]

Hi all,
i have the 'same' problem. It was created two lines one for one surface and one for the other surface. I have two cell zones as well, but when i go to panel
mesh--->info--->zones--->

Zone sizes on domain 1:
249 mixed cells, zone 3.
145 quadrilateral cells, zone 4.
458 2D interior faces, zone 1.
265 2D interior faces, zone 2.
6 2D wall faces, zone 7.
18 2D wall faces, zone 8.
12 2D wall faces, zone 9.
18 2D wall faces, zone 10.
4 2D wall faces, zone 11.
18 2D wall faces, zone 12.
12 2D wall faces, zone 13.
32 2D wall faces, zone 14.
451 nodes.

But i have 2 cell zones, and it said domain 1...why did it do that???why one domain??
thank you in advance!

[davidrobinson50]

I presume that this is a 2D model that you have set this up with Ansys meshing and Fluent?

In Fluent, a domain and zone are not the same thing. The domain is the complete assembly of all your meshes combined together. A zone is a line, surface or volume component of the domain.

First, make sure that you 'freeze' each 2D surface that you create in Ansys Design modeler. This will create a separate part for each surface (rather than letting the 2D surfaces combine to form one part).

Next, make sure that you set up each boundary and 2d region as a 'named selection' in Ansys Mesh.

Finally, in Fluent, your named selections will appear as zones. If you select 'Cell Zone Conditions'/'Boundary Conditions' your zones should appear as you have defined them. Then, to set up you interface, you should be able to find your two interface zones if you select 'Create/Edit...' under 'Mesh Interfaces'.

If this doesn't help then you're going to have to provide me with more detail as to how you've gone about setting up you geometry, mesh, etc..

[Vidyanand Kesti]

Defining the interface in FLUENT if it any spell mistake if you define it AMP or DM,it read it as wall in FLUENT,so check in boundary condition

[Volumeoffluid]

Thank you both for your clarifications. I am trying now this and i ll inform you!

[Volumeoffluid]

Originally Posted by davidrobinson50

I presume that this is a 2D model that you have set this up with Ansys meshing and Fluent?

In Fluent, a domain and zone are not the same thing. The domain is the complete assembly of all your meshes combined together. A zone is a line, surface or volume component of the domain.

First, make sure that you 'freeze' each 2D surface that you create in Ansys Design modeler. This will create a separate part for each surface (rather than letting the 2D surfaces combine to form one part).

Next, make sure that you set up each boundary and 2d region as a 'named selection' in Ansys Mesh.

Finally, in Fluent, your named selections will appear as zones. If you select 'Cell Zone Conditions'/'Boundary Conditions' your zones should appear as you have defined them. Then, to set up you interface, you should be able to find your two interface zones if you select 'Create/Edit...' under 'Mesh Interfaces'.

If this doesn't help then you're going to have to provide me with more detail as to how you've gone about setting up you geometry, mesh, etc..

Hi and thank you for advices,
so still have a problem...i created different sketches for every line and i cannot make surface for different sketches...it told me no closed profiles..
Otherwise when i have surfaces frome edges, there is no option to be 'freeze' or not.
I dont know what i should do.
Do you want to send you my geom to your email??
My email is jimromanas@hotmail.com
Thank you in advance!

[davidrobinson50]

This link will hopefully explain how to create a frozen surface from a sketch http://www.kxcad.net/ansys/ANSYS/wor...ches3dmod.html

Make sure that your sketch is closed and not self-intersecting, otherwise you won't be able to extrude it or create a surface from it! To create a frozen surface, just select "add frozen" instead of "add material" before you generate the geometry. If you're having trouble getting your head around this then I suggest going through some of the ANSYS tutorials - they'll probably explain this better than I can.

If you really need me to look at your geometry I'm happy to do it - but I'd prefer it if you upload it to dropbox (or something similar) for me to download it from.

[Volumeoffluid]

Hi david,

so i really want to see my geometry and tell me my 'errors'..
the file is too small and i can to send you in mail...
but i need an email of you...(for dropbox).
Plz send me your mail in jimromanas@hotmail.com
or send mt your mail in private message here

Regards
Dimitris

[Elio]

Hello John and David

I am modeling a a Vertical axis wind turbine where I have to breakdown the model into several rotating domains.
I am facing the same problem. Any new on the subject? How did you manage to solve it

[Elio]

Hello John and David,

I am modeling a Vertical Axis wind turbine which requires several rotating domains in a stationary domain.
I am facing the same problem.
Any new on the topic? How did you manage to solve it?

Thanks

[aptahaney]

Hi,

I understand that this thread is quite old, but I would really appreciate any guidance you could provide as my problem is almost the exact same as has been described.

I am modelling a 2D VAWT. My geometry consists of a large rectangle with a 2m circle removed from the middle (Part 1). In this 2m hole, I have imported a circle with a 2m diameter (containing 3 airfoils) (Part 2) which shall rotate.

I have done everything that previous posters have suggested to achieve a good interface between the 2 parts, which has worked and which is great.

However, when I go into Fluent, and open the "Create/Edit Mesh Interface", only one interface appears (I get a similar message as shown in the picture posted David on October 10,2012). I have tried the suggestions that previous posters have given, such as freezing the part, naming the selections (faces) etc. but I am still getting no-where and I cannot find my error.

Can you provide advice as to what I may be doing wrong?

(I will outline the steps that I have taken in brief below)

Thanks for your help,

Aidan
_ _ _ _ _ _ _ _ _ _ _ _ _ _ _ _ _ _ _ _ _ _ _ _ _ _ _ _ _ _ _ _ _ _ _ _ _

DESIGN-MODELLER:
Imported rectangle section (with circle removed) (i.e. Part 1). Pressed "Add Frozen", Generate. Named Selections (Inlet, Outlet, Interface 1, Face1).
Imported rotational section, (Part 2). Pressed "Add Frozen", Generate. Named Selections (Airfoils, Interface 2, Face2).
Created New Part called "Total".
ICEM:
Opened geometry. Blocking ->2D Surface Blocking, Associated Edges to Curves. Viewed Pre-mesh.
Outlined Boundary Conditions - at this section, only 1 of the interfaces appears. Then pressed "Write Input" to Fluent, in the hope that the zones would be recognized as mentioned in an earlier post.
FLUENT:
Opened geometry, Viewed "Cell Zone Conditions" and the 2 zones appear (i.e. Face 1 and Face 2) - note, these are different to Parts 1 and 2, but are as defined by "named selection".
Pressed Mesh Interface -> Create. At this point, I can only see one of the interfaces and herein lies my problem.

I have checked for interference between Parts, renamed selections, tried to name just one interface etc. but nothing has worked to date. Therefore, I would really appreciate any assistance and guidance on the problem.

Apologies if the description is a bit brief, but if you need more detail, I'd be happy to provide it. Thanks again.
Aidan

[davidrobinson50]

Hi Aidan, this is a little puzzling, because it sounds like you have set up the named selections correctly...

My guess is that ICEM is meshing your stationary and rotating zones as one part, with a shared interface (rather than a unique interface for each zone). I'm not very familiar with ICEM so I'm not sure why this would be occurring.

I'd suggest keeping the two zones as separate parts in Design Modeller (i.e.: skip the 'Created New Part called "Total"' step). The two zones should appear as two separate frozen bodies in Design Modeller. And remove any blank space from your named selection names (i.e.: replace 'Interface 1' with 'Interface1').

If that still doesn't work, then I think that you are probably doing something incorrectly with ICEM. If this is the case, then I'm afraid that I won't be of much help.. you'd need to find someone more familiar with ICEM. Alternative, you could try using Ansys Meshing to generate the mesh.

Hopefully that helps!
David.

[aptahaney]

Hi David,
Thanks for your suggestions. Yes, it's very confusing (and frustrating). It is possibly something very small that I am doing wrong, but I have not found it yet.
Unfortunately, when I had two frozen parts instead of combining them as you suggested, the mesh interfaces failed to align. I have tried renaming the parts, and re-drawing them and a combination of other changes this evening without success.
The reason that I have not used Ansys meshing is that my thesis supervisor prefers ICEM, as I can control the mesh to a greater degree. Excellent control may be possible in Ansys meshing, and I have used it on previous work but my knowledge of it is very limited - having said that, I may be forced to use it, if I cannot solve this problem by Sunday. I have been working at solving it for quite some time now and will need to make a call on it soon.

Thanks again for your suggestions.

If anyone else would be able to provide any insight, I'd really appreciate if you could share?

Aidan

[LauPal]

Hello guys,

I just had exactly your problem in a very simple case in 2D: I was trying to manage the interface between two squares 1*1 [m^2] unsuccessfully because the edges between the two surfaced (one for each square) seemed to become one when I opened the meshing part. Thus as posted previously I couldn't name two different edges to define a correct mesh interface in fluent.

I solved this problem in design modeler: when you click on the whole part created thanks to your small parts, you should have an option 'shared topology method' (or something like that, I only have the french version right now) at the very end of the details. My default setting was 'automatic', and I presume that option automatically merged the common edge of my squares, resulting the remaining edge. I set this parameter to 'none' (or 'nothing', whatever this is called), did the same process for each surfaced square (the little parts inside this big one) and I had my two edges in the meshing part.

I tested this method in 3D with your concentric cylinders and it seemed to work.

I hope this will help you.

[mdoberpaur]

Hi huys!
I had exactly the same problem as LauPal simulating a 2-D Gorlov Turbine. The shared-topology option did the trick for me!

[Fadih]

hello guys,

i am simulating a 3D VAWT and i am having the same error (overlapping mesh ) was someone able to solve this problem, please help

[rohit_patil1125]

Hi Simon do you know how to get conformal interface between rotating and stationary domain (Vertical axis wind turbines) in ICEMCFD. I am using hexa mesh in rotating and stationary region.

[PSYMN]

The point of having a rotational domain is that it should be free to move and not be con-formal with the stationary domain.

Now, if you want to make the rotating domain into a stationary domain, then yes, you can merge one domain with another using merge mesh or merge blocking (depending on the type of mesh you have). But when you take that mesh to your solver, it will not be able to rotate the domain anymore.

[rohit_patil1125]

Thanks a lot for your reply. I understood what you suggested but I have separate project files for rotating and stationary domains and have same node distribution on both the domains so the nodes will overlap(but they are not overlapping in ICEMCFD 17). And there will not any kind of numerical error at the interface by using conformal time step. Which is possible with Gambit (unstructured mesh) but I am not able to manage it with ICEMCFD 17.0 (Hexa mesh).

[lcbarreto]

Hi guys,

I am having a similar problem to the one stated on the begining of the post. I am simulating the flow over an aircraft and I want to slice my domain in order to generate different types of mesh (tet for the region close to the airplane and hex for the far regions). I am having problem making the meshs to match.

Simon, the solution that you said before (Creating a new part) used to work for me in design modeler, however it does not seems to work with spaceclaim. Does anyone know how to do it with Spaceclaim?

Thanks in advance.