# Pseudo 2D mesh

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

March 6, 2016, 10:47
Pseudo 2D mesh
#1
New Member

Join Date: May 2014
Posts: 13
Rep Power: 10
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).

Sandra.
Attached Images
 Mesh 3D.jpg (161.6 KB, 73 views) Mesh ZY.jpg (188.2 KB, 70 views) Residuals.png (22.2 KB, 43 views) velocity_1500.jpg (45.2 KB, 56 views) velocity_106.png (35.8 KB, 51 views)

 March 8, 2016, 18:48 #2 Senior Member   Lucky Join Date: Apr 2011 Location: Orlando, FL USA Posts: 5,141 Rep Power: 61 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.

 March 10, 2016, 14:50 #3 New Member   Join Date: May 2014 Posts: 13 Rep Power: 10 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...

March 10, 2016, 18:26
#4
Senior Member

Join Date: Nov 2010
Location: USA
Posts: 1,232
Rep Power: 23
Quote:
 Originally Posted by sandri_92 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.

March 10, 2016, 18:55
#5
Senior Member

Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,141
Rep Power: 61
Quote:
 Originally Posted by sandri_92 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.

May 19, 2016, 16:30
#6
New Member

Join Date: May 2014
Posts: 13
Rep Power: 10
Quote:
 Originally Posted by me3840 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.

May 19, 2016, 16:30
#7
New Member

Join Date: May 2014
Posts: 13
Rep Power: 10
Quote:
 Originally Posted by LuckyTran 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!

October 19, 2017, 13:54
mesh refinement
#8
New Member

Join Date: Oct 2017
Posts: 1
Rep Power: 0
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,
best

ps: as you see in mesh.jpg the orange part is what i want to increase the mesh number
Attached Images
 mesh.jpg (185.8 KB, 33 views)

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