CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

Warning about mesh when initialization

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 18, 2017, 00:33
Default Warning about mesh when initialization
  #1
Member
 
Join Date: Jun 2014
Location: Taiwan
Posts: 89
Rep Power: 5
SJSW is on a distinguished road
Hi~

I drew a mesh shaped like the attached file "Pic1.jpg" for VOF model using Detached Eddy Simulation(DES) in ANSYS 17 Workbench.
The length of the cell edge is 1mm for all cells.
I tried two methods to created the geometry as drew in the attached file "Pic2.jpg".
Method A is to draw a full geometry and then slice it. Then "select both->right click->Form a New Part".
Method B is to create two bodies and then "select both->right click->Form a New Part".

When it comes to initialization, the following warning showed up:

Info: The mesh contains elements that are invalid or of poor quality.

A different numerical scheme will be applied to these elements,
which may affect the quality of the solution. It is recommended
that you consider removing the invalid and poor quality elements
in the mesh.

For more information on the invalid and poor quality elements,
please use the following TUI commands:

/mesh/check

> /mesh/repair-improve/report-poor-elements.
WARNING: The mesh contains high aspect ratio quadrilateral,
hexahedral, or polyhedral cells.
The default algorithm used to compute the wall
distance required by the turbulence models might
produce wrong results in these cells.
Please inspect the wall distance by displaying the
contours of the 'Cell Wall Distance' at the
boundaries. If you observe any irregularities we
recommend the use of an alternative algorithm to
correct the wall distance.
Please select /solve/initialize/repair-wall-distance
using the text user interface to switch to the
alternative algorithm.


If the turbulence model was changed to k-epsilon, this warning will not show up.

For now, I don't know what the reason is.
If the turbulence model matters?
or the meshing steps went wrong? need some merge?

In Text User Interface,I used command "mesh/check". "left-handed faces detected" and "WARNING: Mesh check failed" showed up.
Then use "solve/initialize/repair-wall-distance".
Then use "mesh/check", still "left-handed faces detected" and "WARNING: Mesh check failed" showed up.
Then use "/mesh/repair-improve/repair".
Then use "/mesh/check" and no left-handed faces detected.

Is it OK now? @@ is there something missing?
Honestly speaking, I don't know what happened.
orz
Attached Images
File Type: jpg Pic1.jpg (71.1 KB, 8 views)
File Type: jpg Pic2.jpg (15.7 KB, 5 views)
SJSW is offline   Reply With Quote

Old   May 18, 2017, 01:42
Default
  #2
Senior Member
 
Svetlana Tkachenko
Join Date: Oct 2013
Location: Australia
Posts: 144
Rep Power: 5
Светлана is on a distinguished road
What program did you use for creating your mesh?
Светлана is offline   Reply With Quote

Old   May 18, 2017, 02:01
Default
  #3
Member
 
Join Date: Jun 2014
Location: Taiwan
Posts: 89
Rep Power: 5
SJSW is on a distinguished road
Quote:
Originally Posted by Светлана View Post
What program did you use for creating your mesh?
Component systems->Mesh

I don't know is it ICEM or just ANSYS Meshing?
The title of this program/feature in Workbench is "B: Mesh- Meshing [ANSYS ICEM CFD]".
However, opening the Help manual from the menu bar, it shows "Meshing User's Guide".
@@
SJSW is offline   Reply With Quote

Old   May 18, 2017, 02:11
Default
  #4
Senior Member
 
Svetlana Tkachenko
Join Date: Oct 2013
Location: Australia
Posts: 144
Rep Power: 5
Светлана is on a distinguished road
This means you used ICEM. Use edit meshcheck mesh feature to view the problematic mesh regions.

Just to confirm, you are modelling this in 2d (not 3d with symmetry condition), correct?

As a personal recommendation, I would suggest to use a non-uniform mesh distribution such as shown here.
Светлана is offline   Reply With Quote

Old   May 18, 2017, 02:31
Default
  #5
Member
 
Join Date: Jun 2014
Location: Taiwan
Posts: 89
Rep Power: 5
SJSW is on a distinguished road
Quote:
Originally Posted by Светлана View Post
This means you used ICEM. Use edit meshcheck mesh feature to view the problematic mesh regions.

Just to confirm, you are modelling this in 2d (not 3d with symmetry condition), correct?

As a personal recommendation, I would suggest to use a non-uniform mesh distribution such as shown here.
Yes, this model is 2D.

The Graphic User Interface(GUI) is like the attached file "pic3.jpg".
It seems not ICEM. @@
I will try to find the function "mesh->check" you suggested.

Orinially, this model is for supersonic under-water flow and boundary layer was assumed to be not important.
I will try to use "inflation" in Meshing.
Attached Images
File Type: jpg Pic3.jpg (76.9 KB, 4 views)
SJSW is offline   Reply With Quote

Old   May 19, 2017, 00:49
Default
  #6
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 1,904
Rep Power: 26
LuckyTran will become famous soon enoughLuckyTran will become famous soon enough
You did some commands out of the proper sequence, but you should be ok now. Let me explain what each does.

Quote:
Originally Posted by SJSW View Post
1.In Text User Interface,I used command "mesh/check". "left-handed faces detected" and "WARNING: Mesh check failed" showed up.
2.Then use "solve/initialize/repair-wall-distance".
3.Then use "mesh/check", still "left-handed faces detected" and "WARNING: Mesh check failed" showed up.
4.Then use "/mesh/repair-improve/repair".
5.Then use "/mesh/check" and no left-handed faces detected.
1. You ran the mesh check and it failed
2 You tried to change a numerical setting (the hint that it is numerical is that you are in solve/initialize), which doesn't do anything to the mesh
3. You ran the mesh check again. Of course the mesh check will again fail because it is the exact same mesh as before.
4. You finally ran the repair utility (note that you're not in mesh/check and not solve/initialize)
5. Now when you check the mesh, it's ok because the mesh has been repaired.

The high aspect ratio cells WARNING is just a warning. Usually you mesh this way intentionally and it is expected. I.e. you often have super high aspect ratios cells because of wall clustering to achieve a small y+. If you don't think you have high aspect ratio cells however, then you should go back to the mesher and see what happened because you clearly do. The warning appears when you have aspect ratios around 25-ish or more.

Btw your geometry looks very simple. I would spend some effort to learn how to generate good meshes from the start to avoid these errors.
LuckyTran 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
refineWallLayer Error Yuby OpenFOAM Meshing & Mesh Conversion 1 May 19, 2017 10:13
installing funkySetFields prapanj OpenFOAM Installation 65 October 8, 2015 17:46
Courant number blowing up, non-orthogonal mesh? odellar OpenFOAM Running, Solving & CFD 5 October 22, 2013 19:50
using METIS functions in fortran dokeun Main CFD Forum 7 January 29, 2013 05:06
Icemcfd 11: Loss of mesh from surface mesh option? Joe CFX 2 March 26, 2007 18:10


All times are GMT -4. The time now is 23:25.