CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > Siemens > STAR-CCM+

Pseudo 2D mesh

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 6, 2016, 09:47
Unhappy Pseudo 2D mesh
  #1
New Member
 
Join Date: May 2014
Posts: 13
Rep Power: 9
sandri_92 is on a distinguished road
Hi there! It's been a long time since my last post... I was then using fluent, and now I'm working as an intern and I have to fast learn Star-ccm+ to help my coworkers to do simulations ... They're pretty ambitius!

This time I want to do something that was easy in fluent & CFX. We want to make a 3D mesh, but use it for a 2D simulation. I mean, considering 3-axis, and the "depth" in the x-direction, the ZY plane should be refined, and have some nice inflation layers, but in the x-direction I want to have only one element (see screenshot mesh 3D & mesh ZY).

In fact, the problem I see here is that having only 2 or 4 elements in that direction doesn't allow me to have good results. If you see the residuals plot, you can check that x-momentum never is below 0.1, I've set as a stopping criteria 1e-4 for every equation (should be OK for our purpose, but next step is to calculate Y+ to check accuracy). And it's kind of non-sense to have more than 1 element, it multiplies the total amount of elements and gives no information, as the boundaries in the x-direction are set to symmetry walls. I've also tried with slip-walls, but I have the same problem, residuals don't go lower than 1e-3 (screenshot residuals).

The funny thing is only with 100 iterations (approx.) it gaves a good result (see screenshot velocity_106), and then at the 400th iteration weird things happens (screenshot velocity_1500)...

So people, what am I doing wrong? Is it possible to have only one element in that direction? I've tried a volumetric control (with all the geometry inside it), and applied a trimmer, anisotropic meshing (taking care in the x-direction), but the minimum number of elements I get is 2.


Some extra info:
-This is a simple simulation involving a flat plate located vertically. The size is (x,y,z)=1, 0.1, 1 (meters). The "wind tunnel" is about (1, 20.1, 11).
-The CD coefficient I want to get is about 1.9 (Frank White as reference).
-Simulations are carried in star-ccm+ 9.02. Local parallel (4 processors).

Thanks in advance!

Sandra.
Attached Images
File Type: jpg Mesh 3D.jpg (161.6 KB, 60 views)
File Type: jpg Mesh ZY.jpg (188.2 KB, 57 views)
File Type: png Residuals.png (22.2 KB, 34 views)
File Type: jpg velocity_1500.jpg (45.2 KB, 44 views)
File Type: png velocity_106.png (35.8 KB, 39 views)
sandri_92 is offline   Reply With Quote

Old   March 8, 2016, 17:48
Default
  #2
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 4,288
Rep Power: 51
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
Are you trying to do a pseudo 2D simulation or are you trying to do a normal 2D simulation?

For an normal 2D simulation:
Go to Mesh => Convert to 2D
this will chop up your 3D mesh and extract a single layer of cells and use 2D governing equations.

Otherwise I am not sure whether there is any utility to trying to work in the most inefficient way.
LuckyTran is offline   Reply With Quote

Old   March 10, 2016, 13:50
Default
  #3
New Member
 
Join Date: May 2014
Posts: 13
Rep Power: 9
sandri_92 is on a distinguished road
Thanks LuckyTran.

I want to make a "pseudo" 2D sim as I said before. The concept is more or less the same as the way the program generates the 2D simulation data.

The reason I want to do it this way is I've tried long time ago a 2D simulation and a 3D simulation with 1 element in the "depth" direction (same geometry and then extruded), and the results were not the same. So from that point in my life, I don't trust 2D sim results...
sandri_92 is offline   Reply With Quote

Old   March 10, 2016, 17:26
Default
  #4
Senior Member
 
Join Date: Nov 2010
Location: USA
Posts: 1,232
Rep Power: 21
me3840 is on a distinguished road
Quote:
Originally Posted by sandri_92 View Post
The reason I want to do it this way is I've tried long time ago a 2D simulation and a 3D simulation with 1 element in the "depth" direction (same geometry and then extruded), and the results were not the same. So from that point in my life, I don't trust 2D sim results...
Why should you expect the results to be precisely the same? You're not simulating the same thing.

The best way to convert to 2D is to use the mesh operation "badge for 2D meshing" to convert your domain. That way you can change the mesh later and the new 2D mesh will reflect it.
me3840 is offline   Reply With Quote

Old   March 10, 2016, 17:55
Default
  #5
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 4,288
Rep Power: 51
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
Quote:
Originally Posted by sandri_92 View Post
Thanks LuckyTran.

I want to make a "pseudo" 2D sim as I said before. The concept is more or less the same as the way the program generates the 2D simulation data.

The reason I want to do it this way is I've tried long time ago a 2D simulation and a 3D simulation with 1 element in the "depth" direction (same geometry and then extruded), and the results were not the same. So from that point in my life, I don't trust 2D sim results...
There's little reason to do a pseudo 2D sim when you can do a true 2D sim. A pseudo 2D sim will always be more inefficient than a true 2D sim. A pseudo 2D sim is also prone to numerical inaccuracies because of the discretization in the 3rd direction (a pseudo 2D sim is also more numerically dissipative because of the addition wiggle room in the 3rd dimension). This manifests as a non-zero velocity and non-zero gradient in the 3rd dimension.

Even if your mesh contains only 1 cell in the 3rd dimension, the linear system you are solving is still a 3D one and the solution of the sparse matrix (which is becoming more singular, more stiff) is more prone to numerical inaccuracies. A 2D solver is free from these issues and is more efficient (faster to solve).

I would always prefer and choose the results of a 2D sim over a pseudo 2D sim. The only time I would trust the results of a pseudo 2D sim is if the fluxes are forcibly fixed to 0. Sorry but I don't support the usage of pseudo 2D simulations if that is your logic.
LuckyTran is offline   Reply With Quote

Old   May 19, 2016, 15:30
Default
  #6
New Member
 
Join Date: May 2014
Posts: 13
Rep Power: 9
sandri_92 is on a distinguished road
Quote:
Originally Posted by me3840 View Post
Why should you expect the results to be precisely the same? You're not simulating the same thing.

The best way to convert to 2D is to use the mesh operation "badge for 2D meshing" to convert your domain. That way you can change the mesh later and the new 2D mesh will reflect it.


I forgot to answer both of you. Thanks for your advice!
sandri_92 is offline   Reply With Quote

Old   May 19, 2016, 15:30
Default
  #7
New Member
 
Join Date: May 2014
Posts: 13
Rep Power: 9
sandri_92 is on a distinguished road
Quote:
Originally Posted by LuckyTran View Post
There's little reason to do a pseudo 2D sim when you can do a true 2D sim. A pseudo 2D sim will always be more inefficient than a true 2D sim. A pseudo 2D sim is also prone to numerical inaccuracies because of the discretization in the 3rd direction (a pseudo 2D sim is also more numerically dissipative because of the addition wiggle room in the 3rd dimension). This manifests as a non-zero velocity and non-zero gradient in the 3rd dimension.

Even if your mesh contains only 1 cell in the 3rd dimension, the linear system you are solving is still a 3D one and the solution of the sparse matrix (which is becoming more singular, more stiff) is more prone to numerical inaccuracies. A 2D solver is free from these issues and is more efficient (faster to solve).

I would always prefer and choose the results of a 2D sim over a pseudo 2D sim. The only time I would trust the results of a pseudo 2D sim is if the fluxes are forcibly fixed to 0. Sorry but I don't support the usage of pseudo 2D simulations if that is your logic.
Thanks LuckyTran!
sandri_92 is offline   Reply With Quote

Old   October 19, 2017, 12:54
Default mesh refinement
  #8
New Member
 
Join Date: Oct 2017
Posts: 1
Rep Power: 0
mahdiderakhshan is on a distinguished road
hello,
Dear Sandri_92
could you please tell m how you did your mesh in different refinements ( i mean the boxes that you created with different mesh setting )
I am doing simulation 2d and I used automated mesh 2d as opération to create these boxes and using the volumetric control for defining them is not working,
that will be great if you you know what i mean i helping me in this way,
thanks in advance
best

ps: as you see in mesh.jpg the orange part is what i want to increase the mesh number
Attached Images
File Type: jpg mesh.jpg (185.8 KB, 26 views)
mahdiderakhshan is offline   Reply With Quote

Reply

Tags
2d simulation, mesh, residuals, star-ccm+

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
sliding mesh problem in CFX Saima CFX 46 September 11, 2021 07:38
Star CCM Overset Mesh Error (Rotating Turbine) thezack Siemens 7 October 12, 2016 11:14
[ICEM] surface mesh merging problem everest ANSYS Meshing & Geometry 44 April 14, 2016 06:41
[ICEM] Problem making structural mesh on a surface froztbear ANSYS Meshing & Geometry 1 November 10, 2011 08:52
[snappyHexMesh] snappyHexMesh won't work - zeros everywhere! sc298 OpenFOAM Meshing & Mesh Conversion 2 March 27, 2011 21:11


All times are GMT -4. The time now is 14:13.