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

[ICEM] export hexa mesh to fluent

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

Like Tree2Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   February 28, 2010, 15:40
Default
  #21
New Member
 
Wieland De Lepeleire
Join Date: Jan 2010
Posts: 18
Rep Power: 7
Wieland is on a distinguished road
After a meshing pause (I focused on the coupling between Fluent and Sysnoise facing some other problems...) I restarted the mesh from scratch, using the o-grid as you recommended.

The sphere cube tutorial was helping a lot. I first made an o-grid to cover the hemisphere, after that I did an o-grid around the mirror. In attachment you can see the mesh around the mirror, which looks good around the mirror, although the scan planes shows very skew elements further away.
Nevertheless I checked the mesh for errors (successful) and imported it in Fluent. But the check in Fluent gave me following error:
"Checking face handedness.
WARNING: left-handed faces detected on zone 10: 678070 right-handed, 6 left-handed.
WARNING: left-handed faces detected on zone 2: 6066 right-handed, 6 left-handed."

I know you can repair this in Fluent using the command line mesh/modify-zones/repair-face-handedness, but in this case it didn't work out.

After this disappointment I made an unstructured mesh with tetra elements. It started good, working in ICEM CFD was easy, quality was good, importing in Fluent succeeded without any error.
BUT... the CFD results were quiet unrealistic, no Karman street was visible which was the case with the hexa meshes.

So I would really like the hexa mesh, but it doesn't work. Can you give some advice concerning the error or again some other help? It is getting frustrating... But that's sometimes in this meshing area I think.

Thanks,
Wieland.
Attached Images
File Type: jpg ScanPlane.jpg (101.9 KB, 137 views)
File Type: jpg ScanPlane2.jpg (104.1 KB, 118 views)
Wieland is offline   Reply With Quote

Old   February 28, 2010, 20:02
Default Topology isn't right.
  #22
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
Your topology isn't right...

You have your OGrid connected to the plate with the Mirror sticking up into the OGrid blocks. This gives you awkward mesh at the "corners" of the sphere again, but instead of wide angles you get pinched ones. Instead, imagine a block around the mirror also so that the mirror and plate are inside the HGrid block in the middle of the OGrid... Then subdivide the inner block to capture the mirror and plate...

Be careful to imagine the mirror as having a reflection of its self so you can put an internal ogrid thru the face of the mirror to take care of poor quality... Sorry if that is hard to understand, it is really something better shown.

I really should try to make one tutorial movie a week, it is just hard to find the time, and it always takes longer to put those together than you would think...

Anyway, this one is on my list...
PSYMN is offline   Reply With Quote

Old   March 1, 2010, 08:04
Default
  #23
New Member
 
Wieland De Lepeleire
Join Date: Jan 2010
Posts: 18
Rep Power: 7
Wieland is on a distinguished road
I see what you mean with the mirror block in the o-grid blocks, and it is the same thought I had when I drove home last night. So let's try it out today. I'll keep you updated.

In previous attempts I've tried the reflection of the mirror, but it didn't really helped, I will try it again.
Wieland is offline   Reply With Quote

Old   March 1, 2010, 11:18
Default
  #24
New Member
 
Wieland De Lepeleire
Join Date: Jan 2010
Posts: 18
Rep Power: 7
Wieland is on a distinguished road
All right, update of the day: I think it's going the right way.

With the new blocking setup, the global mesh distribution looks ok (first figure). There are some skew elements due to the boundary layer, but it can be removed.
The second figure shows a scan plan in the middle of the mirror. Some skew elements due to the o-grid are present, but I hope it's fine? You can see the blockings I've used in the third figure.
Next step is to refine the mesh after the mirror to study the turbulent region, but it gets tricky there to export refined mesh from Fluent to Sysnoise afterwards.

To improve the mesh around the mirror, I tried your hint about the reflected mirror. Blockings and a scan plane are visible in the last attached figures. But I think the other setup results in a better mesh...

Importing the mesh in Fluent went fine, and a Karman street is visible in the first results, so I am getting optimistic.

Any hints to improve the mesh are still welcome, but thank you already!
Attached Images
File Type: jpg Fig_ScanPlane_Global_new.jpg (104.7 KB, 89 views)
File Type: jpg Fig_ScanPlane_Mirror_new.jpg (103.8 KB, 70 views)
File Type: jpg Fig_Blocks_new.jpg (98.7 KB, 53 views)
File Type: jpg Fig_Blocks_ReflectedMirror.jpg (100.5 KB, 60 views)
File Type: jpg Fig_ScanPlane_ReflectedMirror.jpg (106.7 KB, 57 views)
Wieland is offline   Reply With Quote

Old   March 1, 2010, 11:39
Default Almost there.
  #25
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
Great, almost there…

Two more steps and you will have a great mesh…

1)Move your verts onto your geometry. Yes, it looks ok without moving it, but later steps (such as OGrid creation) act on the blocking as it is, not how it will project. You can use the “Snap Project” button to make it quick and easy. But then you may want to adjust verts a little to optimize placement. For instance, the verts along the curve of the mirror should be placed at the 45 degree point (or where ever provides the best reduced average deviation from the edge to the curve).
2)Now that you have created the “reflection” block for your mirror, it is time to put an OGrid in it. Reduce the index control so you are looking at the block for the mirror and its “reflected” block. Then select those two for OGrid. Also select the “faces” as the base (plate) so the OGrid will go down into the plate. This will cure the bad mesh that you are probably getting just behind the “corners” of the mirror.
PSYMN is offline   Reply With Quote

Old   March 1, 2010, 11:42
Default One more thought...
  #26
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
One other thought… The above plan will work “after” your ogrid around the mirror… but it could probably be better to do it before the OGrid around your mirror. If you do the mirror boundary layer after the OGrid mentioned in 2) above, it wouldn’t need to go around the reflection, but could be done just around the mirror.
PSYMN is offline   Reply With Quote

Old   March 2, 2010, 08:18
Default
  #27
New Member
 
Wieland De Lepeleire
Join Date: Jan 2010
Posts: 18
Rep Power: 7
Wieland is on a distinguished road
Hi,

replying to your 2 steps:
1) I didn't find out how to define different materials for a block in ICEM CFD, so I still delete the plate and mirror to enforce the surfaces are meshed. When I snap the vertices to the mirror, and apply Ogrid afterwards, it gets messy when I delete the inner block.
2) In the fourth picture of my previous post you can see I already implemented an Ogrid in the reflected mirror block. Do you mean I have to do it again in the inner block?

I looked on the forum and here is something interesting to make a c-grid. I'll try it.
Wieland is offline   Reply With Quote

Old   March 2, 2010, 20:37
Default ...
  #28
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
1)To define materials, right click on the Parts branch of the model tree to either create a new part or add to an existing one (only add to parts reserved just for volumes or you will have boco troubles). In the Create Part DEZ, the last ICON is “Blocking Material, Create part”. Click that and you will be able to select blocks to put into the new part (instead of just geometry or mesh).
2)You put an OGrid “around” the mirror and reflected block. This is good for capturing boundary layer on the upstream part of the mirror. The problem is that your mirror is also rounded, so on the outer two corners of the glass, you have bad elements. The way to fix these bad elements is to put an OGRID inside the mirror. That ogrid would need to come out of the OGrid and go somewhere (pass thru the glass). You may want to just have it go back for a few blocks (a good way to refine with 1 to 1 connections) , in which case you could just select a block behind the mirror and the mirror and not worry about faces… Or you could have it turn and go into the plate (tidy)… I gave you instructions for the latter, but I have seen it done a variety of ways at various car companies…


The Cgrid Far field is no better or worse than yours (half way between what you have and a Cube... Those topologies were popular in the good old days because the structured solvers could only handle a single block. C-Grid was a good way to wrap that single block around an airfoil.
PSYMN is offline   Reply With Quote

Old   March 16, 2010, 13:02
Default
  #29
New Member
 
Wieland De Lepeleire
Join Date: Jan 2010
Posts: 18
Rep Power: 7
Wieland is on a distinguished road
Hi, I'm back with another problem.

As mentioned before I would like to export the CFD results (more exactly: surface pressure distribution on the mirror) from Fluent to LMS Sysnoise. This already succesfully worked with a test case.

I'm now facing the following problem: I would like to refine the mesh, since CFD results were in accordance with other papers for low frequencies only. Therefore I refined the zone after the mirror in ICEM CFD, but when checking the mesh the error of uncovered faces occured. There are two options: ignore the error (as proposed by Simon on this thread), or fix the error.

When ignoring the error, the mesh (figure 1) can be succesfully imported in Fluent and realistic results are calculated. The problem is that it's impossible to export the mesh in Nastran format (which is necessary for Sysnoise). You can see this in figure 2. Only ASCII, EnSight Case Gold, and Fieldview Unstructured file formats are possible.

When I fix the error in ICEM, the uncovered faces are covered and I add these faces to the "body"-part. The mesh can be imported in Fluent (figure 3) and it's possible to export them in Nastran-format (figure 4). But the new faces cause problems in Fluent since I can not prescribe an "interior" boundary condition for this surface... So calculations are not possible.

The Fluent manual learned me: "ANSYS FLUENT supports exporting polyhedral data only for ASCII, EnSight Case Gold, and Fieldview Unstructured file formats. For further details, see Sections 4.14.4, 4.14.9, and 4.14.12."
So I need to work around the polyhedral data problem. Anyone experience with this? Or does somebody knows how to export the mesh from Fluent in another way?
Attached Images
File Type: jpg Refinement_NotFixed.jpg (95.6 KB, 74 views)
File Type: jpg Export_NotFixed.jpg (35.0 KB, 46 views)
File Type: jpg Refinement_Fixed.jpg (97.1 KB, 49 views)
File Type: jpg Export_Fixed.jpg (35.9 KB, 28 views)
Wieland is offline   Reply With Quote

Old   March 16, 2010, 14:46
Default Nastran format is your weak link...
  #30
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
Maybe someone else can help you move forward, but I can tell you that Nastran does not support hanging nodes. I don't know about SYSNOISE...
PSYMN is offline   Reply With Quote

Old   June 10, 2010, 11:31
Default ICEM to FLUENT export
  #31
New Member
 
Babak Lakghomi
Join Date: Jun 2010
Posts: 5
Rep Power: 7
Babak is on a distinguished road
Hi

Sorry guys

I think this is where I have to ask this question, I am new to ICEM and just trying to export the 2d mesh file from it to FLUENT but I get the following error when reading the mesh File in FLUENT.
3969 nodes.
3840 quadrilateral cells, zone 8.
7552 2D interior faces, zone 9.
176 2D wall faces, zone 10.

Building...
mesh
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.

Any one has an idea why this happens?

Thanks
Babak is offline   Reply With Quote

Old   June 10, 2010, 13:11
Default don't know.
  #32
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 don't know... Perhaps ask on the the Fluent Forum or perhaps contact your friendly neighborhood tech support.
PSYMN is offline   Reply With Quote

Old   December 1, 2010, 14:04
Default What do you think?
  #33
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
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   January 22, 2013, 22:02
Default
  #34
New Member
 
Join Date: Jul 2012
Posts: 25
Rep Power: 5
yuanmengyuan1989 is on a distinguished road
Quote:
Originally Posted by PSYMN View Post
I have setup several of these simulations (except on full vehicle models) using ICEM CFD and Fluent when i worked at Ford Motor Company.

The "Uncovered faces" error is just a possible problem. It would matter for some solvers, but not for Fluent if it is just referring to the hanging nodes...

However, if you get uncovered faces in other areas (such as the boundaries), you may get an error like the one you saw without refinement. Did you do your mesh checks on the unrefined grid? Is a face missing?

It looks like it thinks you have a partial grid. You could Try reading that fluent grid back into ICEM CFD and checking it there.

I would figure out the unrefined grid problem before trying again with refined blocks.
Sorry to bother you. I want to ask you a question. when I create grid for impeller by ICEM, I always take it apart to nine parts, and I create grid for one part in ICEM, then, I will use the “rotate and copy” for anther parts. Generally, I would delete the grids of periodical faces, but when I check the grid, it will remind me of “uncovered faces”, I accorded on its remind to fix the uncovered faces, and created the new part for them, and I found the uncovered faces are the periodical faces I deleted.
If I do not delete periodical faces and it will make mistakes, it says
WARNING: no face with given nodes. Thread 7, cell 352956
Clearing partially read grid.

Error: Build Grid: Aborted due to critical error.

Error: Build Grid: Aborted due to critical error.
Error Object: #f"


I searched the reason why it happen, it says the nodes in the periodical faces are not completely identical.
I tried to guarantee the number of nodes but the same question will occur. So I want to ask you whether you can help me to solve it .
yuanmengyuan1989 is offline   Reply With Quote

Old   January 23, 2013, 00:04
Default
  #35
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,944
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
do you merge all nine parts and elements are in same material point?
Far is offline   Reply With Quote

Old   January 23, 2013, 00:31
Default
  #36
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
If you take a periodic model and copy rotate it before sending it to the solver, you need to do a few extra steps...

First, before you even copy rotate it, run check mesh and make sure all is well. Turn on the periodic check also... If you fail that, let us know and we can discuss that question based on your specific error message.

If you pass the checks, do the the copy rotate. Then delete the periodic shell elements...

THis will leave you with uncovered faces... These are really just volume elements without a shell (or another volume element) to cover them. This is a problem for solvers like fluent because there is no where to hang the boundary condition that the solver algorithm depends on.

To fix the problem, use edit mesh => merge meshes => merge nodes with a tolerance. Set a small tolerance (like 1/10th of the smallest mesh size) and make sure to turn on "ignore projection" and apply. This will merge the volume meshes across the periodic interfaces...

Run the mesh checks again, specifically the "uncovered faces" check...

Have fun.

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   January 23, 2013, 04:18
Default
  #37
New Member
 
Join Date: Jul 2012
Posts: 25
Rep Power: 5
yuanmengyuan1989 is on a distinguished road
Quote:
Originally Posted by PSYMN View Post
If you take a periodic model and copy rotate it before sending it to the solver, you need to do a few extra steps...

First, before you even copy rotate it, run check mesh and make sure all is well. Turn on the periodic check also... If you fail that, let us know and we can discuss that question based on your specific error message.

If you pass the checks, do the the copy rotate. Then delete the periodic shell elements...

THis will leave you with uncovered faces... These are really just volume elements without a shell (or another volume element) to cover them. This is a problem for solvers like fluent because there is no where to hang the boundary condition that the solver algorithm depends on.

To fix the problem, use edit mesh => merge meshes => merge nodes with a tolerance. Set a small tolerance (like 1/10th of the smallest mesh size) and make sure to turn on "ignore projection" and apply. This will merge the volume meshes across the periodic interfaces...

Run the mesh checks again, specifically the "uncovered faces" check...

Have fun.

Simon
Thank you for your reply. I really appreciate it. When I checked the mesh for the 1/9th model, it will remind me of that “121616problems were found or volume orientation”, I do not understand what result in it. Then I fix it, it does not have problems no longer.

But after I copy rotate it and delete the mesh of periodical faces, when I check the grid, it will remind me of “it have uncovered faces”. I accord on what you said as following ,
To fix the problem, use edit mesh => merge meshes => merge nodes with a tolerance. Set a small tolerance (like 1/10th of the smallest mesh size) and make sure to turn on "ignore projection" and apply.
But it still has uncovered faces.

When I do not delete the mesh of periodical faces,it will remind me of “shell 8418 has node 709 which has no twin”.
Why it happen ?
It makes me upset for a long time. I really want to know the truth.
yuanmengyuan1989 is offline   Reply With Quote

Old   January 23, 2013, 04:27
Default
  #38
New Member
 
Join Date: Jul 2012
Posts: 25
Rep Power: 5
yuanmengyuan1989 is on a distinguished road
Quote:
Originally Posted by Far View Post
do you merge all nine parts and elements are in same material point?
Thank you for your reply. I do not know what you mean. I just create mesh for one part, and copy rotate it to gain other meshes, and when I copy rotate it, I choose the “merge nodes and delete duplicate elements”. Can it meet what you said?
I still have not found what the reason why the problems occur.
yuanmengyuan1989 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
How to open Icem mesh in Ansys Fluent? emmkell FLUENT 26 June 9, 2015 15:38
ICEM HEXA to CFX-PRE mesh export pb jaber CFX 1 April 3, 2009 10:06
ICEM HEXA to CFX-PRE mesh export pb jaber CFX 1 April 3, 2009 05:21
prob while exporting icem cfd hexa mesh to fluent mani CFX 4 March 7, 2007 04:41
mesh adaptation for hexa mesh Pete CFX 4 April 6, 2005 18:43


All times are GMT -4. The time now is 10:25.