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

[ICEM] Icem cfd 13.0

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

Like Tree2Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   July 16, 2012, 17:41
Default Icem cfd 13.0
  #1
Member
 
Ehab
Join Date: Nov 2011
Posts: 30
Rep Power: 5
Ehab44 is on a distinguished road
Dear All,


I am using ICEM CFD for meshing instead of Ansys meshing as I was not able to obtain consistent mesh from Ansys meshing.

I am new to ICEM and I need help .... I new tutorials, videos, ...


I hope someone can help me
Ehab44 is offline   Reply With Quote

Old   July 17, 2012, 18:08
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: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
At ICEM CFD 13.0, the tutorials are under Help => Tutorial Manual...

There are others on the Customer Portal, but the built in ones should get you started...
__________________
-----------------------------------------
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   July 18, 2012, 04:19
Default Icem cfd 13
  #3
Member
 
Ehab
Join Date: Nov 2011
Posts: 30
Rep Power: 5
Ehab44 is on a distinguished road
Dear Sir,


Thank you for your reply.

I started working but I am receiving strange errors.

Sometimes the program works well, one time it hangs while it is writing loading prism.uns. Another time, while exporting to fluent I received an error about cell connectivity.

Also, one time after computing the mesh I found a new part added (created faces) and when I repeated compute mesh, it disappears.

Also, I do not know why the number of cells decreases when I export the mesh to fluent.

I am sorry for any inconvenience.



Yours,
Ehab
Ehab44 is offline   Reply With Quote

Old   July 19, 2012, 13:16
Default Icem cfd 13
  #4
Member
 
Ehab
Join Date: Nov 2011
Posts: 30
Rep Power: 5
Ehab44 is on a distinguished road
Dear Sir,


I hope you can reply to my post soon.

I am sorry for any inconvenience.


Yours,
Ehab
Ehab44 is offline   Reply With Quote

Old   July 19, 2012, 13:45
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
Hey Ehab44, I will answer what I can...


Quote:
Sometimes the program works well, one time it hangs while it is writing loading prism.uns.
Not enough info here... Hanging usually suggests that the mesh exceeds your hardware. Could it be that really large problems are failing to load on your system?

Quote:
Another time, while exporting to fluent I received an error about cell connectivity.
Being more specific about the error would help me guess more specifically at the problem... But generally, these are real errors and they are usually your fault . For instance some new users don't realize that the volume meshing step gives them surface mesh and they separately create or import surface mesh... Or the generate a new mesh but don't replace the old one, so the two are not connected. Or perhaps you have two adjacent volumes that you did not properly merge... To find the problems, run the mesh checks (under the Edit Mesh tab).

Quote:
Also, one time after computing the mesh I found a new part added (created faces) and when I repeated compute mesh, it disappears.
Depending on your mesh sizes, etc. you may have had some leakage or something like that, which it fixed for you with some created faces... If you meshed it again, with slightly different sizes, it may not have had that same problem...

Quote:
Also, I do not know why the number of cells decreases when I export the mesh to fluent.
It doesn't decrease. However, there are lots of ways you could make this mistake. For instance, are you comparing numbers of nodes to numbers of elements? Or perhaps you are comparing number of volume elements to total number of elements (volume plus surface)... Or perhaps you are comparing the mesh loaded in ICEM CFD with the other UNS file that you selected to send to Fluent (the conversion works of a saved file, so perhaps your current mesh was not saved)...
amin_gls likes this.
__________________
-----------------------------------------
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   July 19, 2012, 17:50
Default Icem cfd 13
  #6
Member
 
Ehab
Join Date: Nov 2011
Posts: 30
Rep Power: 5
Ehab44 is on a distinguished road
Dear Sir,

First of All, I really appreciate your help as I am in a critical condition to finish my PhD.

Let me explain in details what I do starting from the beginning:

1- After I open ICEM, I use the workbench reader to import my geometry which is created in Ansys Design Modeler. But I don't know if I should check the option "create material point" or not.

2- I open the global mesh parameters, then I define the global element seed size as 2, 1, 0.5,.... (different cases) and I left the scale factor as 1.

3- In the global mesh parameters, I open the global prism settings and I select the following:
- growth law: linear
- initial height: 0.0
- height ratio: 1.2
- number of layers: 1, 3, 5, 10 (different cases)
- total height: 0.0

4- I open compute mesh and I select the following:
- mesh type: Tetra/mixed
- mesh method: octree
- I checked the option "create prism layers"

5- I click "compute mesh".

As I told you before, some of the cases work and others faced the problems I explained previously knowing that I always change two parameters only:
- global element seed size
- number of layers in global prism settings

Finally, I want to know if I am doing something wrong or there is something missing.

Note: I tried to attach the geometry but it was refused for its size. If you need it, please send me your email in a private message.


I am sorry for any inconvenience ....



Yours,
Ehab
Ehab44 is offline   Reply With Quote

Old   July 21, 2012, 13:58
Default Icem cfd 13
  #7
Member
 
Ehab
Join Date: Nov 2011
Posts: 30
Rep Power: 5
Ehab44 is on a distinguished road
Dear Sir,


Thank you for your reply.

Here is the link for the errors (zip file):
http://www.4shared.com/rar/HkmxFqWV/errors.html

I am sending you 4 errors as follows:
- The first one is a copy screen for the program when it hangs after finishing the prism layers and it is trying to load the domain prism.uns.

- The second one illustrates that there is a difference in the total number of elements between the mesh computed in ICEM and that exported to Fluent.

- The third error occurs in Fluent after exporting the mesh from ICEM.
I can see many surfaces and I do not know where it comes from:
writing part/fluid_left_fluid_paddle:010 (type wall) (mixture)
writing part/fluid_left_fluid_paddle:011 (type wall) (mixture) ... Done.
writing part/fluid_left_fluid_paddle:012 (type wall) (mixture) ... Done.
writing part/fluid_left_fluid_paddle:013 (type wall) (mixture) ... Done.

And when I checked the mesh in Fluent, I found that these are random triangles !!!!

- The fourth error also occurs in Fluent after export and it states in the beginning "can not fill zones". I do not know if this is related to material points or what ??.

Again, I am sorry for any inconvenience and I hope you can reply soon.



Yours,
Ehab
Ehab44 is offline   Reply With Quote

Old   July 23, 2012, 08:51
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
OK, lets try to get thru some of these. If I don't have time to answer all the questions, i will come back and do some more later.

Quote:
1- After I open ICEM, I use the workbench reader to import my geometry which is created in Ansys Design Modeler. But I don't know if I should check the option "create material point" or not.
That is up to you. The option will automatically create a material point in each body. Some people like that. Some would rather place their own. If you don't have a Material point, you will see those "CREATED_MATERIAL" points appear automatically and need to figure out which is your solid or fluid...

Quote:
2- I open the global mesh parameters, then I define the global element seed size as 2, 1, 0.5,.... (different cases) and I left the scale factor as 1.
Sure no problem there, ICEM CFD Octree works better with sizes that are powers of two of each other... But just as an FYI, they could also be 1.25, 2.5, 5 and 10... all powers of 2 off the smallest size set in the model.

Quote:
3- In the global mesh parameters, I open the global prism settings and I select the following:
All fine also...

Quote:
4- I open compute mesh and I select the following:
- mesh type: Tetra/mixed
- mesh method: octree
- I checked the option "create prism layers"
That works, but if you are having any sort of trouble at all, I recommend running separate steps. One for tetra, then check it, maybe smooth it and then run prism as a separate step.

Quote:
5- I click "compute mesh".

As I told you before, some of the cases work and others faced the problems I explained previously knowing that I always change two parameters only:
- global element seed size
- number of layers in global prism settings
Yup, that should work. Problems could be due to mesh size exceeding your machine's capacity, leakage or other geometry induced problems...

Next I will check your geometry and error images. I already noticed the "null pointer error" in the first image which indicates you must have some how lost some shell elements... Did you delete them?
__________________
-----------------------------------------
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   July 23, 2012, 10:29
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
I just meshed the model you sent me... I had created a material point he first time, but then realized that you have lots of different regions and it only meshed the one the material point was in... so I just deleted that material point so it would create its own.

You didn't send me the Tetin file (*.tin), so I didn't know where you set what sizes or prisms. I just set the global max to 2 and set a min size (sizing function) to 0.5. Then I hit compute mesh...

I got about 875k elements (so I would suggest a finer mesh, perhaps setting 3 cells in gap, etc.) I checked quality and ran check mesh... both fine. So I exported to Fluent... again no problems.

If you have a particular ICEM CFD project that failed, you can send me the tetin file and I will try it with tetra and prisms.

If this is supposed to be one large flow volume (instead of broken up as it is), we could remove the interface surfaces or put the same material point in each region (the shells between volume elements in the same material are removed unless the surface is flagged as a baffle or internal wall.)

Next, your error messages...
__________________
-----------------------------------------
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   July 23, 2012, 10:49
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: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
OK, your error messages...

Quote:
- The first one is a copy screen for the program when it hangs after finishing the prism layers and it is trying to load the domain prism.uns.
Sorry, not enough info here to tell. How big is your machine? How big is the mesh? Send me this tetin file and I will run it myself. You could also try looking at the size of that prism.uns file... Try loading it separately...

Quote:
- The second one illustrates that there is a difference in the total number of elements between the mesh computed in ICEM and that exported to Fluent.
Yes, you are not comparing correctly. First of all, that screen shot is not even in Fluent... it is the ICEM CFD output window as it creates the fluent file. At the top of the page, Total elements refers to the total of all the elements in the model (including shells, lines and nodes, as well as tetras and prisms). Lower down, when it refers to cells, it is counting only the volume elements. Go into ICEM CFD => info => mesh info. The number of cells will match the number of tetra + penta elements.

Better yet, read the model into prism and you will see the number of tetrahedral cells for each zone listed. This list will match the ICEM CFD mesh info exactly.

One other thing... This model has ~5 million cells... that shouldn't be a problem. I guess this one worked. Was the one that failed substantially finer?

Quote:
- The third error occurs in Fluent after exporting the mesh from ICEM.
I can see many surfaces and I do not know where it comes from:
writing part/fluid_left_fluid_paddle:010 (type wall) (mixture)
writing part/fluid_left_fluid_paddle:011 (type wall) (mixture) ... Done.
This is probably just Fluent trying to make sense of all your different zones. These zones all meet at interface walls and Fluent needs to create a bunch of shadows to separate things out. It is not an error, it is just Fluent working. Which is why every row ends in "... Done."

No idea about the random triangles. Would need more info...

Quote:
- The fourth error also occurs in Fluent after export and it states in the beginning "can not fill zones". I do not know if this is related to material points or what ??.
The 4th screen shot you send me doesn't say "can not fill zones", but it does show "NULL face pointer"... Basically this just means that you have missing shells. By default, Octree creates shell elements around all the volume elements. You would only get this error if you deleted shell elements. You can run "Check Mesh" inside ICEM CFD and quickly find and repair uncovered faces. If you had simply deleted shells between volumes that you wanted to be continuous, you must make sure that the volume elements are in the same part before sending to Fluent. Zones in Fluent must be separated by shells.
__________________
-----------------------------------------
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   July 23, 2012, 11:02
Default Icem cfd 13
  #11
Member
 
Ehab
Join Date: Nov 2011
Posts: 30
Rep Power: 5
Ehab44 is on a distinguished road
Dear Sir,


I will read carefully your reply and I will try what you told me then I will get back to you.

Thank you for your help.



Yours,
Ehab
Ehab44 is offline   Reply With Quote

Old   July 23, 2012, 11:54
Default
  #12
Member
 
Ehab
Join Date: Nov 2011
Posts: 30
Rep Power: 5
Ehab44 is on a distinguished road
Dear Sir,


I just tried your settings, 2 for maximum size then I check the curvature and proximity based refinement and I set the min size limit to 0.5.

The total number of elements is 873767.

1- When I run mesh check, I received the following:

Running diagnostics for Duplicate elements in subset "all"
No problems were found for Duplicate elements
Running diagnostics for Uncovered faces in subset "all"
No problem volume elements were found for Uncovered faces
Running diagnostics for Missing internal faces in subset "all"
No problems were found for Missing internal faces
Running diagnostics for Volume orientations in subset "all"
No problems were found for Volume orientations
Running diagnostics for Surface orientations in subset "all"
no orientation errors
faces are correctly oriented
Surface orientations are OK
Running diagnostics for Hanging elements in subset "all"
No problems were found for Hanging elements
Running diagnostics for Multiple edges in subset "all"
4783 problems were found for Multiple edges
Running diagnostics for Triangle boxes in subset "all"
No problems were found for Triangle boxes
Running diagnostics for Single edges in subset "all"
No problems were found for Single edges
Running diagnostics for Non-manifold vertices in subset "all"
No problems were found for Non-manifold vertices
Running diagnostics for Unconnected vertices in subset "all"
7030 unconnected vertices were found.
Unconnected vertices are OK


I do not know if multiple edges is a serious problem or not.


2- When I checked mesh quality, I found the minimum to be 0.25. I do not know what is the optimum range.

3- When I export to Fluent, I found the same problem. Not the shadows.... The problem is that Fluent is detecting surfaces that is not existing in ICEM and when I zoom it I found it triangles. Is this problem related to multiple edges or not ?.


Note: I sent you the tetin file, please check your email.

Again, Thank you for your continuous support.



Yours,
Ehab
Ehab44 is offline   Reply With Quote

Old   July 23, 2012, 12:00
Default
  #13
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
1) No, multiple edges should be expected in this model.

2) 0.25 is fine. Smoothing it could probably bring it up, but anything above 0.1 will run without any problems in Fluent.

3) I will check the file when I get a chance.
__________________
-----------------------------------------
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   July 24, 2012, 04:59
Default Icem cfd 13
  #14
Member
 
Ehab
Join Date: Nov 2011
Posts: 30
Rep Power: 5
Ehab44 is on a distinguished road
Dear Mr. Simon,


I tried yesterday to know the reasons of multiple edges but I was not able to detect it.

But I noticed that the multiple edges occur at the common surfaces between the fluid zones. I searched the forum for a similar case but I did not find.



Yours,
Ehab
Ehab44 is offline   Reply With Quote

Old   July 24, 2012, 05:41
Default Icem cfd 13
  #15
Member
 
Ehab
Join Date: Nov 2011
Posts: 30
Rep Power: 5
Ehab44 is on a distinguished road
Dear Mr. Simon,


I knew what is going wrong with Fluent. The random triangles that I see is coming out of the mesh. I mean as if it has been cut from the mesh.

Please check your email and you will understand what I want to say as I can not explain it good.

I sent you a photo for part of the mesh that is computed by ICEM.

I am sorry for wasting your time.



Yours,
Ehab
Ehab44 is offline   Reply With Quote

Old   July 24, 2012, 10:45
Default More on Single/Multiple Edges...
  #16
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
Multiple edges just means that a shell element edge has more than 2 elements attached. Single edges means that a shell edge has only one element attached.

These are only "possible problems".

A single edge may indicate a hole in your model and should be a concern if you were trying to run a delaunay fill or didn't expect to see any holes in the surface. But if you were meshing some stamped steel pieces with a shell and beam model, you would expect single edges around the perimeter and around each hole.

In the same way, a multiple edge could mean you had some mesh pinching problems or other collapsing mesh issues, or it could just mean that you have a T-connection in your shell and beam model (perfectly alright). In you case, you had a number of parts meeting at interfaces, you should expect that all the shells at those interfaces would have multiple edges...
__________________
-----------------------------------------
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   July 24, 2012, 11:19
Default Icem cfd 13
  #17
Member
 
Ehab
Join Date: Nov 2011
Posts: 30
Rep Power: 5
Ehab44 is on a distinguished road
Dear Mr. Simon,



Thank you for your reply.

Did you check your email ?. May be the multiple edges is not a problem for Fluent. But there is another something wrong, please check your email ?.



Yours,
Ehab
Ehab44 is offline   Reply With Quote

Old   July 25, 2012, 04:31
Default Icem cfd 13
  #18
Member
 
Ehab
Join Date: Nov 2011
Posts: 30
Rep Power: 5
Ehab44 is on a distinguished road
Dear Mr. Simon,


I hope you checked your email.

I have another problem. When I import the geometry from Workbench, I checked "create material point" but after computing the mesh I found that the volumes are not filled. When I export to Fluent it gives an error and when I returned to ICEM and use Floodfill, I found that it yields new created material in addition to the material points that I already created.

I want to know if I should define the material points in the beginning or what ?.



Yours,
Ehab
Ehab44 is offline   Reply With Quote

Old   July 25, 2012, 10:50
Default
  #19
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
I will try to get to your email today...

Just noticed this simple question come in, so I jumped on it.

The material points are used during "flood fill". Flood fill is included in the octree meshing process, so ideally you would have material points before meshing.

However, you can run flood fill on its own after the mesh is generated. It is under "Edit Mesh => Repair"

Best regards,

Simon
__________________
-----------------------------------------
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   July 25, 2012, 11:32
Default Icem cfd 13
  #20
Member
 
Ehab
Join Date: Nov 2011
Posts: 30
Rep Power: 5
Ehab44 is on a distinguished road
Dear Mr. Simon,


Thank you for your reply.

To be more clear. I have now two main problems:

1- Material point

I have the following options and I want to know which of them is more suitable for Fluent:
a- Creating material points while importing the geometry.
b- Importing the geometry without material points, then creating material points using Geometry -> Create body.
c- Computing the mesh and then it will be created automatically.

What should I do here ?.

2- Missing cells in the geometry.

This issue you can check in the email I sent you previously. I want to know how can I fix this problem.

Also I need something like procedures that I can follow to reach a fine mesh, if possible.

Again, I am sorry for any inconvenience.




Yours,
Ehab
Ehab44 is offline   Reply With Quote

Reply

Tags
icem cfd 13.0

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
Need help icem cfd kakhtar ANSYS Meshing & Geometry 24 March 24, 2014 14:04
[ICEM] Icem CFD on Linux mechanicaldesign ANSYS Meshing & Geometry 6 February 14, 2013 11:39
Transport mesh from ICEM CFD, to Fluent, to Sysnoise Wieland FLUENT 2 April 15, 2012 06:28
Importing Solidworks part into ICEM CFD MetalSupremacist FLUENT 0 October 8, 2010 17:46
Which is better to develop in-house CFD code or to buy a available CFD package. Tareq Al-shaalan Main CFD Forum 10 June 12, 1999 23:27


All times are GMT -4. The time now is 07:53.