CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [ICEM] Proper way to name boundaries on 2D model for use in CFX? (http://www.cfd-online.com/Forums/ansys-meshing/79815-proper-way-name-boundaries-2d-model-use-cfx.html)

RossFS September 5, 2010 08:20

Proper way to name boundaries on 2D model for use in CFX?
 
I'm trying to mesh a fairly simple structure in 2D (2.5D for CFX) for use in ANSYS CFX in ICEM CFD as the mesher in ANSYS workbench is not giving me the control I need when refining the mesh.

PSYMN has suggested that the easiest way to generate a 2.5D model in ICEM CFD for ANSYS CFX is to generate a 2D mesh and export it in Fluent format. To name locations of the boundaries you just convert the curves (edges) of the mesh into parts. The name and locations of the parts are carried through to ANSYS CFX when importing the mesh file. The problem with doing this however is that it will not give me a part/location for the front *and* rear plane of symmetry (I need to set up symmetry bocos on the "front" and "back" of the mesh in CFX right?) in CFX setup. Is there a work around for this?

-----------
Otherwise, I tried making a 2D mesh and extruding it 1 cell thick. I then made parts out of all the nodes in the relevant locations. This however generates warnings about having parts made up of 2D and 3D elements which isn't allowed in CFX 5. The mesh will import into CFX and the locations I want turn up, but a bunch of stuff I didn't intend to generate seems to come through as well.
What is a better way of setting up the locations (parts) for bocos ?
Generating a surface in the same location as the edges of the nodes I want to select and generating a part from this doesn't appear to generate a location that will transfer into CFX.

zeitistgeld September 5, 2010 09:58

Definitely when you import fluent type mesh into cfxpre, you will find some primitive 2D regions, that's what you need to set them as symmetry pairs.

RossFS September 9, 2010 05:29

Just to clarify for anyone that ends up getting this thread in a search:

1) Create parts out of the curves before creating a surface or doing any premeshing.
2) Create premesh via blocking
3) file -> mesh -> load from blocking
4) export mesh as 2D Fluent file.

Front and rear faces can be selected in CFX by clicking on the "..." box when picking a location and Primitive A and B are your front and rear surfaces.

yvonne November 2, 2011 10:31

I made 2D geometry of a pump (with multiple rotating domains) in GAMBIT, exported it in the .msh format to ICEMcfd(v12.1). Extruded the surface mesh in the z-direction. When I create the .def file and solve it in the solver I get the following error:

+--------------------------------------------------------------------+
| ERROR #002100048 has occurred in subroutine SU_BNEXT. |
| Message: |
| All vertices for a fluid domain lie on boundaries. This is |
| considered to be a fatal error because control volume gradients |
| cannot be calculated, leading to serious discretization error. |
| |
| A common cause for this error is a mesh which is only one |
| element thick, without symmetry or 1:1 periodicity on the lateral |
| boundaries. If you have this situation, and the domain is |
| two-dimensional, please change the lateral boundary conditions |
| to symmetry or 1:1 periodicity. Alternatively, for |
| three-dimensional simulations, please ensure that your mesh |
| has at least two elements across. |
| |
| Execution is terminating. This error message can be bypassed by |
| setting the expert parameter 'boundary vertex check = f', but |
| be aware that doing so may lead to sigificant solution error. |
+--------------------------------------------------------------------+


I cant make anything of it. Kindly help. Where do I specify symmetry?

zeitistgeld November 10, 2011 03:38

Quote:

Originally Posted by yvonne (Post 330446)
I made 2D geometry of a pump (with multiple rotating domains) in GAMBIT, exported it in the .msh format to ICEMcfd(v12.1). Extruded the surface mesh in the z-direction. When I create the .def file and solve it in the solver I get the following error:

+--------------------------------------------------------------------+
| ERROR #002100048 has occurred in subroutine SU_BNEXT. |
| Message: |
| All vertices for a fluid domain lie on boundaries. This is |
| considered to be a fatal error because control volume gradients |
| cannot be calculated, leading to serious discretization error. |
| |
| A common cause for this error is a mesh which is only one |
| element thick, without symmetry or 1:1 periodicity on the lateral |
| boundaries. If you have this situation, and the domain is |
| two-dimensional, please change the lateral boundary conditions |
| to symmetry or 1:1 periodicity. Alternatively, for |
| three-dimensional simulations, please ensure that your mesh |
| has at least two elements across. |
| |
| Execution is terminating. This error message can be bypassed by |
| setting the expert parameter 'boundary vertex check = f', but |
| be aware that doing so may lead to sigificant solution error. |
+--------------------------------------------------------------------+


I cant make anything of it. Kindly help. Where do I specify symmetry?


You should first add different mesh parts into name parts after extrusion. The volume mesh should be added into fluid domain name(or names if you have more than one). Then the error should be excluded(All vertices for a fluid domain lie on boundaries!!!). And those surface mesh parts should be named as what you want, eg. sym01, sym02, inlet, outlet etc. easy to set boundary conditions for them. Check the mesh in ICEM to make sure it is error free. Then export it and import to cfxpre. For symmetric interface pair, you should first set them as interfaces then you can set them as a symmetry pair. Have a try! Good luck!


All times are GMT -4. The time now is 04:05.