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

[ICEM] Interface meshing at dual zone geometry

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 31, 2012, 11:00
Default Interface meshing at dual zone geometry
  #1
New Member
 
Reza
Join Date: Jun 2011
Posts: 2
Rep Power: 0
hamedi.m.reza is on a distinguished road
Hi guys

I am currently modelling a chemical reactor which has 2 fluid zones. In the first one the reactant will heat up by a heat flux at the wall and in the second one chemical reaction will be happen in a porous zone. I did model the geometry in DM and import it to ICEM via workbench reader. Note that there are 2 interface BC, to be able to define the interface in Fluent.

The problem is that when I merge the two blocks which I created for zones, one of the interfaces will disappear at the final mesh. On the other hand, when two separated blocks was used the mesh quality is awful at the interference. Thank you in advance for your help...

Reza
hamedi.m.reza is offline   Reply With Quote

Old   February 1, 2012, 13:54
Default
  #2
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
The blocks should be in different volume parts... If they are both in FLUID, then merging them will result in a single volume. But if one is in FLUID_A and the other is in FLUID_B, then you will get two volumes that share an interface and mesh distribution...

One other tip... If at all possible, you should try to model both regions at once in the same top down procedure... Just create a new part and move the blocks to that part as needed. One top down procedure results in a simpler index and less issues than working from 2 or more combined topologies.
__________________
-----------------------------------------
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   March 31, 2012, 01:48
Default ICEM Interface
  #3
Senior Member
 
mohamed khedr emam
Join Date: Oct 2011
Location: Egypt
Posts: 121
Rep Power: 5
m5edr is on a distinguished road
Quote:
Originally Posted by PSYMN View Post
The blocks should be in different volume parts... If they are both in FLUID, then merging them will result in a single volume. But if one is in FLUID_A and the other is in FLUID_B, then you will get two volumes that share an interface and mesh distribution...

One other tip... If at all possible, you should try to model both regions at once in the same top down procedure... Just create a new part and move the blocks to that part as needed. One top down procedure results in a simpler index and less issues than working from 2 or more combined topologies.
Hi simon

I had two Fluid zone share an interface (this interface could be twice face until i do "Build topology tolerance") >>>see image

After finished meshing , I set the B.C to this interface as INTERFACE and send it to fluent.

Fluent already create it as interface BUT the "Mesh Interfaces" (ANSYS 13) is not permitted due to it only single interface.

I need the "Mesh Interfaces" to be defined due to it a condition for Multiple rotating frame "MRF"

Any suggestion
thanks
Attached Images
File Type: jpg xc.jpg (54.2 KB, 156 views)
m5edr is offline   Reply With Quote

Old   March 31, 2012, 11:10
Default
  #4
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
Sure... You just need to do one more step before saving your mesh and exporting to your solver...

Edit Mesh (tab) => Split mesh => Split Internal Wall...
__________________
-----------------------------------------
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   March 31, 2012, 12:03
Default
  #5
Senior Member
 
mohamed khedr emam
Join Date: Oct 2011
Location: Egypt
Posts: 121
Rep Power: 5
m5edr is on a distinguished road
Quote:
Originally Posted by PSYMN View Post
Sure... You just need to do one more step before saving your mesh and exporting to your solver...

Edit Mesh (tab) => Split mesh => Split Internal Wall...
Thanks Simon
BUT
1-When i made "split Internal Wall" with checked "create volume cells" button option ,ICEM create one other internal wall " back...." and what called "thermal shell"

2-if I didn't check "create volume cells" Icem told me (There are no internal faces) and create new part with "back....."

3- After all ,the problem also is "split meh" cause (bad periodic problem>>>>shell has node which has no twin) that appear when i do a "check mesh" before send the mesh to fluent and Fluent NOT accept the mesh

Thanks in advance for your help...

Last edited by m5edr; April 1, 2012 at 03:53.
m5edr is offline   Reply With Quote

Old   April 4, 2012, 07:50
Default
  #6
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
Split internal wall works by looking for shell elements with volume material on both sides...

If you select the operation and ask for "create volume cells", it automatically splits the nodes and then inserts a new volume element between them. That is a very specific need and not something you probably want to do...

But once you do this operation, you no longer have an internal wall, so if you run it again, it won't detect anything. You need to go back to before you split with create volume cells. If you didn't save your mesh, this may require remeshing, but hopefully you just need to load an earlier version.

Lets sort out this problem with split mesh first and see if the periodic problem just goes away... If it was periodic before split mesh, it should still be after.
__________________
-----------------------------------------
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 4, 2012, 08:05
Default
  #7
Senior Member
 
mohamed khedr emam
Join Date: Oct 2011
Location: Egypt
Posts: 121
Rep Power: 5
m5edr is on a distinguished road
Thanks simon and i'm really missed your recommendations

Quote:
Originally Posted by PSYMN View Post
If you select the operation and ask for "create volume cells", it automatically splits the nodes and then inserts a new volume element between them. That is a very specific need and not something you probably want to do....

Forget split internal wall with "create volume cells" .. i just ask this to know if this will make the difference

Quote:
Originally Posted by PSYMN View Post
Lets sort out this problem with split mesh first and see if the periodic problem just goes away... If it was periodic before split mesh, it should still be after.
No, Before "splitting the wall" periodic looks Good and Fluent accept it perfectly

thanks in advance
m5edr is offline   Reply With Quote

Old   April 10, 2012, 17:28
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
I am not sure what else I can say to this...

Maybe a checklist...

1) Does your mesh actually have internal walls? These would be defined as shell elements with volume mesh on both sides. If you meshed the regions separately then it should have started with two sets of surface mesh, one connected to each volume, and you don't need to split anything.

2) So after confirming 1 above, use split internal wall without the option to create volume elements. Does it tell you that you don't have internal walls or does it work?

3) Assuming 2 works, what does Prism tell you exactly? Does it give an element number where the problem is? Can you check that element (use subsets)?
__________________
-----------------------------------------
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 10, 2012, 18:32
Default
  #9
Senior Member
 
mohamed khedr emam
Join Date: Oct 2011
Location: Egypt
Posts: 121
Rep Power: 5
m5edr is on a distinguished road
Thanks simon

Quote:
Originally Posted by PSYMN View Post

1) Does your mesh actually have internal walls? These would be defined as shell elements with volume mesh on both sides. If you meshed the regions separately then it should have started with two sets of surface mesh, one connected to each volume, and you don't need to split anything.
I'm just did the mesh the two region seperatly but it cause various problem (like mesh found holes , single edge), this kind of errors wasn't appear before (I think i made it in a wrong way) ..Could you told me specific method to mesh regions separately (I choose compute mesh >>> Input >>> select geometry >>> select by parts) !!

Quote:
Originally Posted by PSYMN View Post
2) So after confirming 1 above, use split internal wall without the option to create volume elements. Does it tell you that you don't have internal walls or does it work?
If the model meshes directly (without meshing seperatly ) AFTER after splitting internal wall , Icem create the "same face name _back" but told me (There are no internal faces)


Finally, I know you are so busy BUT Could I ask you to check my model files
I had sent you the files before

Thanks in advance
m5edr is offline   Reply With Quote

Old   April 10, 2012, 20:10
Default
  #10
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
OK, I didn't want to download it before because I had to sign up to the site, but I did it now for you anyway...

You don't need to mesh this separately, but select by parts is one way, but you must be careful to select all the parts associated with each region. A more common method is to save a copy of the tetin file with "visible parts" or just save a copy and then delete the parts you don't need. You mesh the partial copies, then load back the original model and the partial meshes... You could even mesh the parts separately and re-assemble within your solver (never load all the sub components at once in ICEM CFD).

Looking at your mesh, it looks like you meshed it all at once. No problem.

WHen you first go to Split internal wall, it says "Found 1 internal wall part(s)". Then after you apply it says "New parts created:" just as it should. I guess it is a bit confusing that it then says "There are no internal faces", it should be saying "there are no more internal faces". It is just because the command is iterative in ICEM CFD. I will put in a request to fix that so no one else stumbles. Then it says "Done Split Internal Wall".

That all worked perfectly fine...

Then I tried the checks... Periodicity check failed, so I checked its subset and see that it included triangles near the split wall. I checked for the usual suspects (such as line elements in one part but not the periodic pair), but didn't find any issues... I did the manual operation of rotating the one periodic part to fall directly on the other, I couldn't see any difference.

So now I am thinking it looks like a defect... (it might still be my user error). I tried a few other tricks like renumbering the nodes and elements, etc. But no luck.

I will submit a defect on your behalf and get back to you if I figure out the answer.
__________________
-----------------------------------------
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 10, 2012, 23:19
Default
  #11
Senior Member
 
mohamed khedr emam
Join Date: Oct 2011
Location: Egypt
Posts: 121
Rep Power: 5
m5edr is on a distinguished road
Many thanks Simon and I'm appreciate your efforts

I'm wait the answer

Thanks again
m5edr is offline   Reply With Quote

Old   April 22, 2012, 18:15
Default
  #12
Senior Member
 
mohamed khedr emam
Join Date: Oct 2011
Location: Egypt
Posts: 121
Rep Power: 5
m5edr is on a distinguished road
Hi simon

Any news

thanks in advance
m5edr is offline   Reply With Quote

Old   May 6, 2012, 00:38
Default NeW Technique
  #13
Senior Member
 
mohamed khedr emam
Join Date: Oct 2011
Location: Egypt
Posts: 121
Rep Power: 5
m5edr is on a distinguished road
Dear / Simon


Since Im waiting you replay, I thought in another direction as following
Now, I changed my technique, now Im able to make two duplicated wall between the two fluid zones (using original geometry in solidworks ) and no need to use Split internal wall option.
BUT when ICEM meshing completed, I found one wall is meshed and the other is not.
Could you please see the New case after the modification , this is the link
http://www.4shared.com/rar/IierXH9h/Project.html

Finally, i'm sorry for disturbance but as you know before my phd pending
Please I need you help
Thanks in advance
m5edr is offline   Reply With Quote

Reply

Tags
icem cfd, interface, multi zone

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
Problem in running ICEM grid in Openfoam Tarak OpenFOAM 6 September 9, 2011 17:51
[ICEM] Meshing on a Complicated Geometry tav98f ANSYS Meshing & Geometry 2 August 17, 2011 11:15
Segmentation Fault in fluent3DMeshToFoam cwang5 OpenFOAM Bugs 23 April 13, 2011 15:37
RPM in Wind Turbine Pankaj CFX 9 November 23, 2009 05:05
IGES/IGS format geometry file for icem meshing littlelz Main CFD Forum 0 May 27, 2008 18:24


All times are GMT -4. The time now is 22:58.