# 1 cell thick mesh not running as 2D simulation- why?

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 September 16, 2010, 06:39 1 cell thick mesh not running as 2D simulation- why? #1 Member   Join Date: Feb 2010 Location: Australia Posts: 65 Rep Power: 15 Structured mesh is only one cell thick (generated in ICEM CFD 12.1): smallest width of a cell: 0.25 units smallest height of a cell: 0.5 units thickness of 2D mesh: 0.25 or 0.025 or 0.0025 (all produce w components of momentum etc) I'm using a free slip wall for the top boco, no slip wall for bottom boco, symmetry on front and back walls and inlet and outlet as inlet and outlet. I'm getting a w component for momentum in the results. What is the go? I take it that if a calculation is being conducted for the w components of values, that the computational cost is the same whether the value is very large or not? -------------- I was using the trick of generating a 2D mesh in ICEM CFD and saving it as a Fluent file, but this doesn't always get the mesh thin enough to be a thickness similar to that of the smallest element of the 2D mesh.

 September 16, 2010, 18:02 #2 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,326 Rep Power: 138 The basics are covered here: http://www.cfd-online.com/Wiki/Ansys..._simulation.3F I assume "front and back" are your one cell thick direction, with symmetry planes. You sometimes get some W momentum stuff because your geometry is not totally flat, you are not converging tight enough or you are doing a axisymmetric simulation (which will always have a W component).

 September 17, 2010, 01:50 #3 Member   Join Date: Feb 2010 Location: Australia Posts: 65 Rep Power: 15 Yes, front and back are on either side of the 1 cell thick mesh. Does CFX calculate values in the thickness/w direction even when the mesh is setup to run as 1 cell thick? I ran a very simple 10x10x1 cell mesh (that I'm certain is flat and sufficiently thin [1 order of magnitude thinner than required]) with all the same setup conditions I've been using and still get a w velocity component, although it is very small (3e-18 m/s as opposed to the u velocity component of 557.6m/s in the free stream area). Last edited by RossFS; September 17, 2010 at 21:11.

September 17, 2010, 05:45
#4
Super Moderator

Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,326
Rep Power: 138
Quote:
 Does CFX calculate values in the thickness/w direction even when the mesh is setup to run as 1 cell thick?
Yes, CFX has no 2D solver so uses a 3D solver. A very poor imitation - uses far more memory, CPU time and results file than it should but this is the most requested thing of the CFX solver I am sure. But it will never happen.

Quote:
 I ran a very simple 10x10x1 cell mesh (that I'm certain is flat and sufficiently thing [1 order of magnitude thinner than required])
What do you think is required? Sounds like you have no idea what are talking about here...

If the mesh has only one element thickness in the z direction with symmetry planes on top and bottom it should not matter what the thickness is. But numerical issues become important so you should make the thickness approximately the size of the smallest element.

But the end effect is as you note - the Z velocities are 1E20 less than the U and V velocities. Once you take engineering accuracy into account that is a zero Z velocity.

 September 17, 2010, 21:16 #5 Member   Join Date: Feb 2010 Location: Australia Posts: 65 Rep Power: 15 I guess the confusion has been that the documentation for CFX indicates that it will conduct a 2D simulation if you make the mesh 1 cell thick. According to you it does not (thanks very much for the clarification, if only I knew this much earlier!).

 September 17, 2010, 21:39 #6 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,326 Rep Power: 138 What the documentation means is the 3D simulation degenerates to a 2D one, where the third equation is trivial (but still calculated). This is why it is a 2D model, but very inefficient as it is using the full 3D equations.

 Tags 2d simulation, icem cfd

 Thread Tools Search this Thread Search this Thread: Advanced Search Display Modes Linear Mode

 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 OffTrackbacks are Off Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Althea FLUENT 22 January 4, 2017 03:19 tommymoose ANSYS Meshing & Geometry 48 April 15, 2013 04:24 kedarj14 OpenFOAM Programming & Development 0 January 29, 2010 01:48 lr103476 OpenFOAM Running, Solving & CFD 30 November 19, 2007 14:09 Frank Muldoon Main CFD Forum 1 January 5, 1999 10:09

All times are GMT -4. The time now is 20:24.

 Contact Us - CFD Online - Privacy Statement - Top