CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > ANSYS Meshing & Geometry

How to export 2-D mesh from ICEM CFD for CFX

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree3Likes
  • 1 Post By PSYMN
  • 2 Post By PSYMN

Reply
 
LinkBack Thread Tools Display Modes
Old   December 22, 2009, 07:54
Default How to export 2-D mesh from ICEM CFD for CFX
  #1
New Member
 
Join Date: Dec 2009
Posts: 2
Rep Power: 0
karimakhtar is on a distinguished road
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
karimakhtar is offline   Reply With Quote

Old   December 23, 2009, 23:54
Default Extrude to 3D...
  #2
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
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.
star_mir likes this.
PSYMN is offline   Reply With Quote

Old   December 24, 2009, 14:50
Default
  #3
New Member
 
Join Date: Dec 2009
Posts: 2
Rep Power: 0
karimakhtar is on a distinguished road
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
karimakhtar is offline   Reply With Quote

Old   May 27, 2010, 10:44
Default
  #4
Member
 
Neil Duffy
Join Date: Mar 2010
Posts: 34
Rep Power: 7
neilduffy1024 is on a distinguished road
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
Attached Images
File Type: jpg ICEM hexa mesh.jpg (36.8 KB, 139 views)
File Type: jpg Geometry named selections.jpg (28.9 KB, 116 views)

Last edited by neilduffy1024; May 27, 2010 at 11:04.
neilduffy1024 is offline   Reply With Quote

Old   May 27, 2010, 14:48
Default
  #5
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
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.)
Odysseus and leoly like this.
PSYMN is offline   Reply With Quote

Old   May 28, 2010, 09:41
Default 2.5D meshing methods
  #6
Member
 
Neil Duffy
Join Date: Mar 2010
Posts: 34
Rep Power: 7
neilduffy1024 is on a distinguished road
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

Attached Images
File Type: jpg Geometry inlet mesh issue2.jpg (81.9 KB, 61 views)
neilduffy1024 is offline   Reply With Quote

Old   April 13, 2011, 12:30
Default other way around ;-)
  #7
New Member
 
Evren
Join Date: Mar 2010
Posts: 20
Rep Power: 7
pbe_cfd is on a distinguished road
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
pbe_cfd is offline   Reply With Quote

Old   April 13, 2011, 13:14
Default
  #8
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
@ 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.
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   April 13, 2011, 13:16
Default
  #9
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
@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.
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   April 14, 2011, 05:48
Default *.msh icem-cfd or Fluent
  #10
New Member
 
Evren
Join Date: Mar 2010
Posts: 20
Rep Power: 7
pbe_cfd is on a distinguished road
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
pbe_cfd is offline   Reply With Quote

Old   April 14, 2011, 09:43
Default Doc links...
  #11
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
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.
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   April 14, 2011, 12:38
Default different msh formats
  #12
New Member
 
Evren
Join Date: Mar 2010
Posts: 20
Rep Power: 7
pbe_cfd is on a distinguished road
@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.
Attached Files
File Type: txt fluent.msh.txt (1.9 KB, 36 views)
File Type: txt icemcfdForCfx.msh.txt (11.7 KB, 26 views)
pbe_cfd is offline   Reply With Quote

Old   November 2, 2011, 07:30
Default
  #13
New Member
 
@p N
Join Date: Jan 2010
Location: United States
Posts: 27
Rep Power: 7
yvonne is on a distinguished road
Quote:
Originally Posted by PSYMN View Post
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 is offline   Reply With Quote

Old   November 3, 2011, 10:36
Default
  #14
New Member
 
@p N
Join Date: Jan 2010
Location: United States
Posts: 27
Rep Power: 7
yvonne is on a distinguished road
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!
yvonne is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Export Msh fron ICEM CFD 11 to Star-CD4.06 hamoudi STAR-CD 3 June 12, 2009 14:31
----------------2D mesh with ICEM CFD Abir FLUENT 2 September 12, 2008 23:55
ICEM CFD: Tri MEsh Farid CFX 5 February 29, 2008 07:32
Quality of extruded mesh in ICEM CFD Andrew CFX 1 December 28, 2006 11:35
ICEM mesh export Twiti CFX 0 August 8, 2004 22:40


All times are GMT -4. The time now is 09:46.