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/)
-   -   How to export 2-D mesh from ICEM CFD for CFX (http://www.cfd-online.com/Forums/ansys-meshing/71262-how-export-2-d-mesh-icem-cfd-cfx.html)

karimakhtar December 22, 2009 07:54

How to export 2-D mesh from ICEM CFD for CFX
 
Hi every body,

Can any one tell me how to export simple 2-D mesh from ICEM CFD to CFX. I am new to icem and spend a lot of time on this problem..Thanks

PSYMN December 23, 2009 23:54

Extrude to 3D...
 
CFX doesn't support solving in 2D... Rather you must make your model 2.5D.

Do this by extruding your model by one cell in the Z direction... Usually, by a distance approximately equal to your average cell size.

The Extrude tool (under Edit Mesh) will give you options to name the top. Leave the sides set to inherited so they will inherit the names of the curves (for bocos).

Then go to output and select ANSYS CFX (not one of the other pre ANSYS CFX variants...) in other words, the list is alphabetical, so look under "A" not "C".

The rest should be fairly obvious and is the same as 3D output.

karimakhtar December 24, 2009 14:50

Thanks Simon Pereire

I was using gambit, in gambit we were doing 2-D. CFX automatically gave extrusion to 2D model, I made now the Geometry. I also converted the mesh into .mesh extension readable for both fluent and cfx. The only problem now I have is how to define region and boundary condition. I am still looking for it

neilduffy1024 May 27, 2010 10:44

2 Attachment(s)
Hi,

I'm having a similar problem. I want to do a 2.5D simulation of a combustion chamber in CFX. When I did this using CFX-Mesh I created the geometry by extruding a sketch a small amount - so I did the same here and also created named selections in DM and then imported into ICEM. I then created a 2D planar structured hexa mesh (see attachment). It might be worth noting that I just switched on premesh to do this and did not select the separate compute mesh option as it meshed up the hexa parameters I had laid out. Is this correct?

Following the ICEM tutorial (hexa meshing in a grid fin) I set up periodicity and assigned the periodic vertices. The surface mesh was projected to the opposite periodic face but it's hard to tell if there is a volume mesh (as the geometry thickness is of the order of the mesh elements). However, I can't seem to import the mesh into cfx (or save it as a .cfx file)?

I've seen suggestions on some of the posts about converting to an unstructured mesh and then extruding it by one element. The main reason I didn't do this is because many of the named selections (parts in ICEM) I set up are in the face normal to the original 2D planar block (on the very thin surface created by extrusion - highlighted and circled in attached pic) and I was hoping to use these to set up boundary conditions in CFX pre as I did in previous simulations using the CFX-Mesh. Is there a way to do this and still keep the named selections? I just figured the nodes would not match. I have since tried to convert the periodic structured mesh to unstructured but still can't import.

Any suggestions would be great because ICEM is a tough nut to crack for people new to it. Thanks.

Neil

PSYMN May 27, 2010 14:48

Hello,

The info above was a bit out of date. The current easiest way to get a 2.5D mesh for CFX is to create a 2D mesh and then output it in Fluent Format. When a 2D Fluent mesh is read into CFX, it automatically extrudes it a bit...

Then people ask "what about bocos". Well, you just put the curves into parts (or named selections) so that when the line elements are extruded into shells, they will be in the correct part name. Note, that it is important to associate all the perimeter edges to the perimeter curves, other wise you will not get line elements on those boundaries and will end up with an unbounded model.

Now specific to your situation... if you wanted to do it with an actual 1 element thick hexa blocking... You seem to be on the right track. Use translational periodic to make sure that your mesh is a 2.5 D model and not 3D... Yes, you will have volume cells (no worries). You can not export premesh. you must convert it to Unstructured mesh. Once it is unstructured mesh, you can run your checks, etc. Then go to output and write it out to "ANSYS CFX".

Now here is the kicker... ANSYS CFX is not the same as a native CFX pre file. So when you go into CFX Pre, you can't just "Open" it. Instead, you must got to "New" and then "Import" the mesh from ICEM CFD... It is a bit unintuitive, but it works.

But like I said, the 2D method is easiest... It is also easier to block (<half the associations, etc.)

neilduffy1024 May 28, 2010 09:41

2.5D meshing methods
 
1 Attachment(s)
Thanks Simon,
both methods of creating the 2D mesh and then either extruding it or exporting to Fluent seem easier than setting up periodic vertices. I just have a couple questions related to these:

  • If I wanted the mesh to remain very thin (say 0.01 mm), would setting the mesh to have a thickness be sufficient for a 2.5D simulation, rather than extruding it by one element (~5-10 mm)?
  • To create a 2D mesh for export to Fluent, would you still have to import a 3D geometry into ICEM, then go about the usual business of creating 2D blocks, associating part names to curves for bocos etc to generate a purely 2D mesh? It's just I tried importing a 2D .STEP file (created in SW) and it didn't seem to like it (no surfaces I fear). Not that there is any issue drawing it, but would discrepancies between mesh and geometry cause issues (at least when extruding you can force it to match the geometry)?
I just have one more question, related to the mesh around one of the inlets (circled in red in attached jpeg). I could not get the mesh to propagate fully despite matching parameters on both opposing edges. Is there a reason for this or should I just fix it with mesh editing tools?

Thanks for all the help


pbe_cfd April 13, 2011 12:30

other way around ;-)
 
1) Is it possible to import mesh from CFX files as, *.def, *.res or *.cfx ?

2) I would like to convert *.msh file which is created by icem-cfd to another format which will be used for our in house CFD solver. I need to learn the format of the msh file. I couldn't find much information so far. What I understand form the ascii output of msh file is,

1) No idea about 1. line
2) Info about version
3) Number of vertices and elements, 4 stands for hexahedral elements but the other parameters, no idea....
4) with in the 4'th line coordinates are given
5) Then cells are written with node id
6) Then 3d regions are defined. (I couldn't get the convention. 10 vertices are specified at each line, so most probably 6 faces of a cell is defined at each line???)
8) Then vertices are specified with the local number of face. what's the local numbering for faces?

Could one justify my propositions and give some references?

keep on good work:rolleyes:

PSYMN April 13, 2011 13:14

@ Nielduffy

1) No, the mesh thickness is a property, not actual thickness. However, you could setup thickness and then use the edit mesh option to convert shells to hexas, which uses that thickness property to do its thing... However, both these options are really for FEA solvers. They still wouldn't convert the surrounding line elements to shells (needed for CFD bocos), and you wouldn't have the top and bottom shells, so it wouldn't be acceptable for CFD solvers.

2) Yes, you can bring a 2D geometry into ICEM CFD. I think that a 2D step file doesn't actually have surfaces. I don't use Step much, but I think they always come in with just curves. You don't actually need the surfaces in 2D meshing, but I usually create them anyway.

3) That mesh not propagating suggests that your blocking is not properly connected. If those blocks were sharing an edge, the the mesh would propagate. How did you create that? You can right click on edges to show color by connectivity. You can merge the end nodes (which may appear aligned, but are probably still separate); if both end nodes are merged, the edge between them is also merged and the mesh will propagate thru.

PSYMN April 13, 2011 13:16

@pbe_cfd

You can read CFX *.def or *.res files into ICEM CFD.

Fluent *.msh is a very well documented format. Check the customer portal for all that info.

pbe_cfd April 14, 2011 05:48

*.msh icem-cfd or Fluent
 
As far as I see from ascii output of both icem-cfd and fluent, the formats are different. Fluent *.msh seems to be more complicated and containing more information. where as, icem-cfd has a simpler *.msh format. And what I need is icem-cfd *.msh file format. Could one supply some information on icem-cfd *.msh format, please ?
cheers;)

PSYMN April 14, 2011 09:43

Doc links...
 
Here is the table of output interfaces...

http://www.ansys.com/Products/Other+...Interfaces+TOC

If you click on the Fluent V6 one, you get specifics...

http://www.ansys.com/staticassets/AN...georampant.htm

Is this enough? Maybe you could compare this with the fuller doc on the Fluent customer site.

pbe_cfd April 14, 2011 12:38

different msh formats
 
2 Attachment(s)
@PSYMN
Thanks, it's totally irrelevant. The format in the scope is not the Fluent's msh format. It's the msh format which is generated by icem-cfd in order to be imported by CFX. May be, you compare the attached files to see the difference ;)


All the best,
Evren
PS. There are oder msh formats, as gid, gmsh, ...
PPS. The attached files are just samples, some part of the mesh files. If you are interested I can send the complete mesh files.

yvonne November 2, 2011 07:30

Quote:

Originally Posted by PSYMN (Post 260562)
Hello,

The info above was a bit out of date. The current easiest way to get a 2.5D mesh for CFX is to create a 2D mesh and then output it in Fluent Format. When a 2D Fluent mesh is read into CFX, it automatically extrudes it a bit...

Then people ask "what about bocos". Well, you just put the curves into parts (or named selections) so that when the line elements are extruded into shells, they will be in the correct part name. Note, that it is important to associate all the perimeter edges to the perimeter curves, other wise you will not get line elements on those boundaries and will end up with an unbounded model.

Now specific to your situation... if you wanted to do it with an actual 1 element thick hexa blocking... You seem to be on the right track. Use translational periodic to make sure that your mesh is a 2.5 D model and not 3D... Yes, you will have volume cells (no worries). You can not export premesh. you must convert it to Unstructured mesh. Once it is unstructured mesh, you can run your checks, etc. Then go to output and write it out to "ANSYS CFX".

Now here is the kicker... ANSYS CFX is not the same as a native CFX pre file. So when you go into CFX Pre, you can't just "Open" it. Instead, you must got to "New" and then "Import" the mesh from ICEM CFD... It is a bit unintuitive, but it works.

But like I said, the 2D method is easiest... It is also easier to block (<half the associations, etc.)

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

yvonne November 3, 2011 10:36

Hi All!
I am trying to create a 2.5 D geometry of a centrifugal pump in ICEMcfd. following is the algorithm use:

* Create the geometry
* add parts: As Ill be using frozen rotor scheme, Ill need three domains--> Inlet(stationary), Rotating domain, Outlet(stationary). Corresponding to 3D setup, where we add surfaces to parts for creating bocos, Im adding curves for this 2.5D simulation.
* I then add 2 interfaces (to separate the moving domain from the two stationary ones)
* I mesh this.
* Extrude the mesh in z-axis by one layer.
* Export in CFX format
After meshing generally (for 3D geometries) the domains will get created automatically, as ICEM will recognise the interface boundary. But this is not happening in my 2D case.
In CFX-pre when I open the geometry it shows only one domain with 'interface' as a boco.
Im not doing pre-mesh or blocking as Im very new to ICEM. Is that the solution?

Also If i make 2D mesh and export in Fluent format and see this in CFX-pre, I get the following error message:

ERROR The importing process reported the following warning(s) while importing
the mesh from the requested file:
Failed to construct all elements.
There was a problem importing the mesh from the requested file.
The importing process reported the following problem:
Unable to import mesh: No 3D elements are present.

Kindly help!:(


All times are GMT -4. The time now is 07:04.