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

[ICEM] ICEM problem

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 5, 2010, 01:42
Default ICEM problem
  #1
Senior Member
 
MASOUD
Join Date: Mar 2009
Posts: 102
Rep Power: 7
MASOUD is on a distinguished road
Hi guys,
I have created a project in ICEM but when i save it (including geometry, block, mesh , etc) and try to read the mesh in to the Ansys Fluent 12.0, it doesn't appear. the extension of the mesh file is: *.*uns.
What's wrong?
thanks
MASOUD is offline   Reply With Quote

Old   March 5, 2010, 09:28
Default
  #2
Super Moderator
 
Ryne Whitehill
Join Date: Aug 2009
Posts: 313
Rep Power: 8
rwryne is on a distinguished road
The files that are created when you hit save are ICEM files, not Fluent files.

Go to the output tab of ICEM and do the following:

1. select Fluent as your solver using the red toolbox button
2. set up your BCs with the BC button
3. click the final button to output your mesh in a Fluent format
rwryne is offline   Reply With Quote

Old   March 5, 2010, 16:14
Default
  #3
Senior Member
 
MASOUD
Join Date: Mar 2009
Posts: 102
Rep Power: 7
MASOUD is on a distinguished road
Thanks for reply.

But still I come across a fatal error when I read the mesh file in Fluent.
Attached is the geometry of a 2D molten carbonate fuel cell with 6 zones (Gas channels, anode, cathode and electrolyte.
I'm not that much familiar with ICEM comparing to Gambit.
Could please help me know how can I generate the mesh for this geometry?
Many thanks
Attached Images
File Type: gif geometry.gif (26.5 KB, 32 views)
MASOUD is offline   Reply With Quote

Old   March 8, 2010, 01:53
Default
  #4
Senior Member
 
Rikio
Join Date: Mar 2009
Location: SH, China
Posts: 182
Blog Entries: 1
Rep Power: 7
rikio is on a distinguished road
Send a message via Skype™ to rikio
Could you show the details of the error message?
Follow the three steps as Ryne show will lead to a successful transfer from ICEM to FLUENT. Maybe you do not set the boundary conditions correctly.Have a check.
rikio is offline   Reply With Quote

Old   March 8, 2010, 11:59
Default
  #5
Senior Member
 
MASOUD
Join Date: Mar 2009
Posts: 102
Rep Power: 7
MASOUD is on a distinguished road
Thanks Rikio.

Here is the error detail:

Error:
FLUENT received fatal signal (ACCESS_VIOLATION)
1. Note exact events leading to error.
2. Save case/data under new name.
3. Exit program and restart to continue.
4. Report error to your distributor.
Error Object: #f

You are right about the BCs. But I don't know how to set the BCs in ICEM. here is the path I'm trying to use:

output>boundary condition>mixed/unknown>GEOM>create new>....

Then I don't know how to find zone ID...what is that?

Thanks
MASOUD is offline   Reply With Quote

Old   March 8, 2010, 14:37
Default
  #6
Senior Member
 
MASOUD
Join Date: Mar 2009
Posts: 102
Rep Power: 7
MASOUD is on a distinguished road
And I need all the curves shown in the attached picture in Fluent to be shown separately because I wanna set different BCs for eachone. But what I can see in Fluent when read the mesh, is a grouped curves not individual curves. So I can't set different Bcs for eachone.
MASOUD is offline   Reply With Quote

Old   March 8, 2010, 15:38
Default
  #7
Super Moderator
 
Ryne Whitehill
Join Date: Aug 2009
Posts: 313
Rep Power: 8
rwryne is on a distinguished road
Quote:
Originally Posted by MASOUD View Post
And I need all the curves shown in the attached picture in Fluent to be shown separately because I wanna set different BCs for eachone. But what I can see in Fluent when read the mesh, is a grouped curves not individual curves. So I can't set different Bcs for eachone.
It sounds like you need to separate your geometry into various parts.

In the tree menu, right click on the "Parts" entry and select Create New Part, then select the geometry corresponding to the first part. Rinse and repeat for all parts.
rwryne is offline   Reply With Quote

Old   March 8, 2010, 15:42
Default
  #8
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,650
Blog Entries: 1
Rep Power: 33
PSYMN will become famous soon enoughPSYMN will become famous soon enough
Boundary conditions are based on part names... If you know you will need different bocos for each curve, you must put each one in its own Part.

If this is a 2D model, Bocos should be applied to the boundary curve parts. if it is a 3D model, then bocos are applied to the surfaces.

As for the Zone ID's, don't worry about that. I usually just leave those all zeros. (they are all in the same zone, zone 0.)
PSYMN is offline   Reply With Quote

Old   March 8, 2010, 16:19
Default
  #9
Senior Member
 
MASOUD
Join Date: Mar 2009
Posts: 102
Rep Power: 7
MASOUD is on a distinguished road
Thank you for reply.

1. Can I do this separation in Fluent as well? (Mesh>separate>...)

2. And what is the SHADOW in Boundary Condition panel?

3. How can I separate the zones? As you see in the attached file, I need to have 6 different zone (some as fluid and some as solid) but in the preliminary geometry which I've created in ICEM i have just one zone.

4. What's the point of BLOCKing??? What we used to do in GAMBIT was: building a geometry>generating a grid network>defining BCs and zones, that's it. So what is the Blocking?
MASOUD is offline   Reply With Quote

Old   March 8, 2010, 16:34
Default questions...
  #10
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,650
Blog Entries: 1
Rep Power: 33
PSYMN will become famous soon enoughPSYMN will become famous soon enough
1) I guess you could do it in Fluent, but then you would be selecting elements, etc. I have never done it that way. It is much easier to setup the Geometry Parts in ICEM CFD.

2) You have one boundary between two regions, but Fluent needs to have boundaries all around each region. So it autmatically creates a "shadow" boundary, which is essentially just a way to select a boundary already used for another region. Don't worry about it, it is just a Fluent book keeping thing...

3) separating the zones is as easy as breaking up the boundaries. Just right click on "Parts" branch in the model tree and "create new part"... For that new Part (say SOLID or INLET)), select the corresponding entity on the screen. For 2D models, surfaces are zones and curves (lines) are boundaries. The points don't matter much unless you are planning to do something special... I usually just put the points in the same part as the adjacent curve.

4) In Gambit, you had to subdivide the actual geometry. This is risky since geometry changes can cause problems, and it was difficult if not impossible to edit those subdivisions later and you would have to start over with each new geometry. Blocking solves these problems by giving you a separate data layer to subdivide, etc. You don't need to damage your original geometry and you don't need to conform to it either (patch independent). It is also very flexible and allows for easy creation of topologies that would be a nightmare in Gambit. You can edit blocking easily. You can also load a previous blocking topology and quickly fit it to a new but topologically similar geometry.

In your case, you have a very simple model so you don't really see the advantages. You just want to extract one block from each surface so use the 2D surface blocking method and it can block it for you automatically... This is the most like Gambit but it is still a separate layer that you can edit, etc.

But you could also just use a quad meshing algorithm and generate unstructured mesh directly without blocking...
PSYMN is offline   Reply With Quote

Old   March 8, 2010, 21:14
Default
  #11
Senior Member
 
MASOUD
Join Date: Mar 2009
Posts: 102
Rep Power: 7
MASOUD is on a distinguished road
Many thanks for the comprehensive answer.

I could create five rectangular zones in PART section from the scratch. But still I don't know how can I have four Curves from each rectangular?

By the way could you help me know what's the difference between:
Patch independant
Patch dependent
Auto block
Shirinkwrap

Would you provide me with any online reference?

Thanks
MASOUD is offline   Reply With Quote

Old   March 9, 2010, 08:11
Default
  #12
Super Moderator
 
Ryne Whitehill
Join Date: Aug 2009
Posts: 313
Rep Power: 8
rwryne is on a distinguished road
Quote:
Originally Posted by MASOUD View Post
Many thanks for the comprehensive answer.

I could create five rectangular zones in PART section from the scratch. But still I don't know how can I have four Curves from each rectangular?

By the way could you help me know what's the difference between:
Patch independant
Patch dependent
Auto block
Shirinkwrap

Would you provide me with any online reference?

Thanks
The help menu will help explain the difference in these (Help->User Manual)
rwryne is offline   Reply With Quote

Old   March 9, 2010, 09:49
Default
  #13
Senior Member
 
MASOUD
Join Date: Mar 2009
Posts: 102
Rep Power: 7
MASOUD is on a distinguished road
how about for creating 4 curves from a rectangular part?
MASOUD is offline   Reply With Quote

Old   March 9, 2010, 10:19
Default No problem...
  #14
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,650
Blog Entries: 1
Rep Power: 33
PSYMN will become famous soon enoughPSYMN will become famous soon enough
You could try "Geometry Tab => Repair => Build Diagnostic Topology". This will create curves around all your surfaces... If you leave the "inherit part" checkbox (near the top above the other icons) on, it will create curves in the names of the surfaces. If you turn that option off, it will put all the created curves into a new part (CURVES). Either way, you can then create parts for each of the new entities.
PSYMN is offline   Reply With Quote

Old   March 9, 2010, 11:18
Default
  #15
Senior Member
 
MASOUD
Join Date: Mar 2009
Posts: 102
Rep Power: 7
MASOUD is on a distinguished road
Could you please let me know for the other check boxes, which one must be on and which one off? Because I did what you wrote leaving all other check boxes as default but I didn't any new part in the PART section. (or even a subtree)
MASOUD is offline   Reply With Quote

Old   March 10, 2010, 01:58
Default
  #16
Senior Member
 
Rikio
Join Date: Mar 2009
Location: SH, China
Posts: 182
Blog Entries: 1
Rep Power: 7
rikio is on a distinguished road
Send a message via Skype™ to rikio
You can refer to the Help Manual first, that may help you out. If you still have some problems in understanding, just post here. :-)
rikio is offline   Reply With Quote

Old   March 11, 2010, 16:57
Default Hands on help...
  #17
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,650
Blog Entries: 1
Rep Power: 33
PSYMN will become famous soon enoughPSYMN will become famous soon enough
So the first thing I noticed was that you had no surfaces, just curves. It is possible to mesh like this, but then it becomes a hassle because you have to select the area (material) elements and put them in a separate part from the boundaries (or use a separate blocking material if you use Hexa Blocking).

It is much easier and more intuitive to simply create surfaces from your curves (geometry tab => Create curves => from surfaces). I left the inherited part name on so. This just took about 2 seconds per surface and now the elements will know what part to be created in, the part of the underlying surface.


Masoud_02_Surfaces.jpg



Next I set sizes. I set all curve sizes to 0.0002, but you could have been fancy and set things up much more carefully.


Masoud_03_CurveNodeSpacing.jpg



Next, I starting creating new parts for the curves in the top two sections (you can complete the rest on your own). I also created an assembly and put all the parts for each section into that assembly. I also put all the points into a POINTS part… It is not necessary, but it makes the boundary conditions a little clearer because there are no points mixed in there.


Masoud_03_BreakIntoParts.jpg



Next, I went to Compute mesh and hit the “compute” button. 2 seconds and no effort later, I have a mapped quad mesh.

Masoud_04_ComputeMesh.gif



You can see from the colors of the quads that they match the materials parts. The colors of the boundaries match the boundary parts…


Masoud_05_Mesh.jpg



To be continued with boundary conditions…
PSYMN is offline   Reply With Quote

Old   March 11, 2010, 17:00
Default Hands on help... Continued
  #18
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,650
Blog Entries: 1
Rep Power: 33
PSYMN will become famous soon enoughPSYMN will become famous soon enough
Ok, above we sorted out the geometry prep and meshing. Now we look at setting Bocos. I Chose FLUENT as my solver and have expanded some branches of the tree.



Masoud_06_Bocos.jpg



If I had volume elements, they would be in the volume section. For surface elements, it groups them into “one sided” (surface elements with volume on one side) or “two sided” (surface elements with volumes on 2 sides). We don’t have any volume elements, so our shells don’t fit either of these and end up in “mixed unknown”.

Here I have clicked on the “Create New” under the ANODE-GAS_CHANNEL_Material and you can see that I could select fluid, etc.

Further down in the boco tree, under “edges” you can see the ones I separated out. You would add bocos to these for Inlet, outlet, walls, etc. (wall is the default, internal walls are also taken care of by default). Further down, under Nodes, you can see the POINTS part I created., At the very bottom under “Mixed/Unknown” are the other parts. These are “mixed dimension” because they contain curves and surfaces (shells and lines” in the same part. This makes it more difficult to apply bocos that are “dimension specific”. In practice, you will need to break those up appropriately also.

(Note, it is ok to have edges in with your shells if they are internal and of no concern (such as the internal edges due to the surface topology rather than edges due to boundaries where you will need at least wall bocos… If you assign these mixed/unknown a boco, it will only apply it to the elements that make sense. If you applied a fluid property to the bottom part, it would apply to its shells, and the lines would be ignored. But in this case, Fluent would complain because the part had no boundary to hang bocos on...)

Have fun.

Simon
PSYMN is offline   Reply With Quote

Old   March 11, 2010, 22:22
Default
  #19
Senior Member
 
Rikio
Join Date: Mar 2009
Location: SH, China
Posts: 182
Blog Entries: 1
Rep Power: 7
rikio is on a distinguished road
Send a message via Skype™ to rikio
I have to say that Simon is a great advisor. :-)
One question about the zone ID. Generally, I left the zone IDs to default because no effect to meshing and solving. Why we need this option to be involved? It seems that zone ID would be used in UDF in Fluent. Is it the only case that we need this ID?
rikio is offline   Reply With Quote

Old   March 12, 2010, 08:49
Default Maybe someone else knows?
  #20
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,650
Blog Entries: 1
Rep Power: 33
PSYMN will become famous soon enoughPSYMN will become famous soon enough
That option was put in before I took over the product.

Most of these features are driven by customer demand... I have never needed to use that Zone ID because Fluent assigns it for me.

Perhaps there is some good reason for some users to have wanted it (udfs as you mention) or perhaps the reason is historical and no longer necessary.

Maybe someone else on CFD-Online can tell us?
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
ICEM - strange linking problem RodriguezFatz ANSYS Meshing & Geometry 3 October 25, 2011 03:25
[ANSYS Meshing] Problem with Icem Script Krish ANSYS Meshing & Geometry 0 October 18, 2011 12:10
[ICEM] Problem while improting Solidworks Part file or Acis File into ICEM CFD venki1130 ANSYS Meshing & Geometry 0 October 13, 2011 13:04
ICEM boundary condition problem Martin_D ANSYS Meshing & Geometry 2 February 14, 2011 10:20
Icem to FLUENT problem Babak FLUENT 0 June 10, 2010 17:14


All times are GMT -4. The time now is 17:55.