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

[ICEM] How to Define a Line separating two Meshes/Regions to not show up as "wall" in Fluent

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 25, 2009, 23:48
Default How to Define a Line separating two Meshes/Regions to not show up as "wall" in Fluent
  #1
New Member
 
Join Date: Mar 2009
Posts: 21
Rep Power: 8
enigma is on a distinguished road
Good Day Everybody,

My name is Martin and I would like to kindly ask you for your technical expertise concerning an ICEM meshing issue I could not solve despite having invested a considerable effort.

I use ICEM to create a mesh which consists of two parts/regions allowing me to assign different pressures to these regions. The problem is that the boundary between these two meshes (the quarter of the elliptical curve on the left hand side at the bottom) always shows up as a "hard line" (called hotedge in the screenshots) when importing the mesh in Fluent which means that I have to assign a boundary condition to that line which is "wall", or "outflow" or whatsoever.

Is there any possibility to tell Fluent / ICEM that this curve is just an interior curve doing nothing else than seperating the meshes? I do have another grid where this line simply shows up as "Type/Interior" in the boundary condition menue. This mesh however was created using Gambit by another person. I would like to find a way to do the same thing in ICEM.

Thank you very much for your help,







enigma is offline   Reply With Quote

Old   March 26, 2009, 01:23
Default
  #2
Senior Member
 
Rikio
Join Date: Mar 2009
Location: SH, China
Posts: 182
Blog Entries: 1
Rep Power: 8
rikio is on a distinguished road
Send a message via Skype™ to rikio
Hi, engima,

You can get this by following steps:
1). Create a separate part to include the line named Hotedge. And assign other curves into parts as many as you want.
2). Mesh the domain in quar or tri.
3). If mesh obtained by blocking, get mesh by "Load From Blocking" which can be accessed via File/Mesh/.
4). Save the mesh as a project.
5). Output. Select Fluent as the solver, then specify BC for the curves. As you want, assign "interior" to Hotedge, and wall & inlet & outlet to others. At last, write input file for the solver you chose.
6). So far, msh file generated.

Something you should pay attention to are: a). create a part for the geometry that will be assigned different BC, such as Hotedge in this case; b). If the solver is Fluent, you have to specify BCs in ICEM Output, and not for CFX (I do not know other solvers' requirement).
rikio is offline   Reply With Quote

Old   March 26, 2009, 04:06
Default
  #3
New Member
 
Join Date: Mar 2009
Posts: 21
Rep Power: 8
enigma is on a distinguished road
Dear Rikio,

First of all, I would like to say thank you for your reply and your support to solve this issue. I did not know that you can assign the BC "interior" inside of ICEM but cannot do that in Fluent. Unfortunately, assigning "interior" to this part (hotedge) which consists of a curve only, would be changed back to "wall" by fluent (this can be seen in the screenshot, with Ansys and Fluent open, there's also the BC menue and the Ansys tree in the image).

1) Whenever one creates a mesh in ICEM (Mesh/Compute Mesh/Surface Mesh Only/Input/Select Geometry from Screen) in a certain region, ICEM automatically adds the mesh to one of the parts (in this example there are 3 lines, hence 3 parts for the small mesh and 5 lines, hence 5 parts to create the large mesh). The line on the left hand side of the problem is divided into "Sym1" and "Sym2". ICEM automatically adds the small mesh to "Sym1" and the large mesh to "Sym2". Is there any way to tell ICEM to create a NEW part whenever a mesh is created? The mesh should be an independent part, shouldn't it? This is why in the BC field ICEM classifies Sym1 and Sym2 as "Mixed/Unknown".

2) It appears to me as if this line/part "hotedge" is attached to both meshes. When looking at the Fluent error (screenshot), one can see that Fluent tries to break that line/part ("hotedge") down into two components. They both look exactly the same. I assume one belongs to the small mesh, the other one belongs to the large mesh.

Thank you very much for your input.

enigma is offline   Reply With Quote

Old   March 26, 2009, 09:42
Default
  #4
Senior Member
 
Rikio
Join Date: Mar 2009
Location: SH, China
Posts: 182
Blog Entries: 1
Rep Power: 8
rikio is on a distinguished road
Send a message via Skype™ to rikio
Hi,

I tried the same geometry as you did, it works well.
Do you generate two surfaces for the two portions? If you mesh on these two surfaces, the mesh will be created into these surface parts. Have a try to see whether it works.
rikio is offline   Reply With Quote

Old   March 27, 2009, 01:48
Default
  #5
New Member
 
Join Date: Mar 2009
Posts: 21
Rep Power: 8
enigma is on a distinguished road
Hey mate,

Thanks for your comment. I import the geometry from a step file and create the meshes from there. I have modified the step file to no longer consist of a wireframe, but surfaces, in other words, the imported geometry consists of two surfaces only (screenshot1). When I try to create these surfaces in ANSYS ICEM (from a imported wireframe) it would misalign the edges (screenshot2) since it appears to me as if it could not handle the elliptic curve. Hotedge is now automatically assigned the BC "fluid", which is, I think what I'm after. Unfortunately Fluent would not accept the mesh, when I check the mesh with ICEM (screenshot 3) it would say that all the border elements are "single edge elements". I had a look at other, more complex meshes and ICEM comes up with the same error message when checking the grid, so that cannot be the problem.

I was suggested to not use ICEM in the beginning and I think I should have rather started with Gridgen. Nevertheless I'm not giving up on that issue since I'm pretty sure that there is a way around it.

Rikio, when you say you modelled the problem yourself I assume you created the geometry in ANSYS, is that correct? I also assume you drew the ellipse through previously calculated points since there is no option in ICEM to draw an ellipse.





Last edited by enigma; March 27, 2009 at 02:04.
enigma is offline   Reply With Quote

Old   March 27, 2009, 02:13
Default
  #6
Senior Member
 
Rikio
Join Date: Mar 2009
Location: SH, China
Posts: 182
Blog Entries: 1
Rep Power: 8
rikio is on a distinguished road
Send a message via Skype™ to rikio
It seems there are two curves in the second figure above. If mesh generated on the two, of course they will be single edge elements.
I upload an example for your reference.
Attached Files
File Type: zip Example.zip (63.4 KB, 26 views)
rikio is offline   Reply With Quote

Old   April 5, 2009, 19:31
Default
  #7
New Member
 
Join Date: Mar 2009
Posts: 21
Rep Power: 8
enigma is on a distinguished road
Thanks for that and thanks for the help.

As a matter of fact I found the issue with importing the wireframe into Ansys. The problem is that when one creates the surfaces, they will not be stiched together, hence, when creating the mesh it will regard the boundaries between individual meshes as walls.

Problem solved!
Cheers!
enigma is offline   Reply With Quote

Old   April 6, 2009, 12:20
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: 36
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Right, to mesh it as one part, you need to build topology on the geometry to connect the two parts together. Once the geometry is sharing that curve, the meshers will understand to share that curve also.

ICEM CFD has the same full boco fluent mesh file capability as Gambit. By default, the boundary between two flow regions is called a wall (lines in 2D or surfaces in 3D). If you do not want these as a wall you simply needed to override that default.
PSYMN 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
Robin B.C. Yu FLUENT 3 May 27, 2012 04:19
DEfine NON NEWTONIAN Blood flow in FLUENT jusepina Main CFD Forum 0 January 18, 2009 17:43
OpenFOAM15 installables are incomplete problem with paraFoam tryingof OpenFOAM Bugs 17 December 7, 2008 05:41
Free surface boudary conditions with SOLA-VOF Fan Main CFD Forum 10 September 9, 2006 12:24
Options when running Fluent from the command line An Modh Coinniolach FLUENT 2 January 14, 2003 05:11


All times are GMT -4. The time now is 02:36.