
[Sponsors] 
October 13, 2015, 17:33 
problem in 2D simulation?

#1 
Senior Member
hamidi
Join Date: Sep 2012
Posts: 251
Rep Power: 7 
Hi dear friends
i want simulating one spillway as shown follow in 2D, i using version 14, in previous version like v12 for apply 2d meshing, we used tree menu , option, meshing strategy,extruded 2D mesh, now in new versions this capability is removed, i have multiple question: 1 whether before entering to ansys meshing , i should know thicnkness of element in z direction? my mean is that in drawing geometry i should extrude object equal to thickness of element, therefore i should know thickness it before entering to meshing. How thickness is usually considered for 2d simulation? i extrude 2d geometry 1cm in z direction in autocad, then i exported it to ansys, What type of mesh method(multizone , sweep ,,,) should I use for do this? I have little experience in the 2D simulation, please help me. thanks a lot for any comment and advice best regards 

October 14, 2015, 11:47 

#2 
Member
Join Date: Jan 2015
Posts: 63
Rep Power: 4 
Hi
As CFX is a 3D solver, you need to extrude normal to the 2D. The thickness does not matter as long as you are able to get a nice and regular hex mesh (usually it should be in the order of the smallest mesh dimension): you should be able to put 1 element only across the thickness (otherwise, if you put more elements the runtime will be longer and the accuracy will not get benefits). Symmetry boundary conditions will be applied at front and back. Note that the residual of the velocity component normal to your 2D sketch (in the direction of the extrusion) should not affect the convergence. Sweep method (or multi zone) in ANSYS Meshing will work fine to produce hex mesh. Last edited by highorder_cfd; October 14, 2015 at 17:39. 

October 14, 2015, 13:32 

#3 
Senior Member
hamidi
Join Date: Sep 2012
Posts: 251
Rep Power: 7 
dear highorder_cfd
thanks for clear explanation, unfortuantely i dont understand your mean about : Note that the residual of the velocity component normal to your 2D sketch (in the direction of the extrusion) should not affect the convergence. if your possible, please explain more. thanks in advance bet wishes 

October 14, 2015, 13:58 

#4 
Member
Join Date: Jan 2015
Posts: 63
Rep Power: 4 
As you are solving a 2D problem, the velocity vector should be V=(u,v), with w=0. However, as CFX is a 3D code it will keep to solve equations for u,v and w (V=(u,v,W).
It might be that during the convergence the residuals of all the variables will converge, whereas the residual of the velocity component normal to your sketch (w) will be at a different level of convergence. In CFX Pre you can exclude the residual of the w component from the convergence monitor, in this way the convergence criteria will not consider that equation. However, please open the ANSYS Help and look at the CFX tutorials. You should be able to find an example of 2D model. Last edited by highorder_cfd; October 14, 2015 at 17:49. 

October 14, 2015, 15:14 

#5 
Senior Member
hamidi
Join Date: Sep 2012
Posts: 251
Rep Power: 7 
dear highorder_cfd
i do reading free surface flow over a bump for several times, but in it is not written things about w component, whether your mean this is that in monitor point i put velocity w=0? please help me, I am involved for several days on this discussion. best regards Last edited by hamidciv; October 15, 2015 at 07:12. 

October 14, 2015, 16:30 

#6 
Member
Join Date: Jan 2015
Posts: 63
Rep Power: 4 
No, you misunderstood me, you do not need to set up monitors for the w component.
Just run normally as for a 3D problem, with a mesh with 1 element through the thickness and using symmetry boundary conditions at front and back. That's it! If it can help, from the CFD manual: The following is advice for modeling 2D problems: Make the mesh only 1 element thick. More elements will slow computational time and require more memory. For planar 2D geometries, apply symmetry conditions to the front and back planes. Free Surface Flow Over a Bump is one example of a case that uses this setup. Do not use free slip walls; doing so will hurt accuracy because control volume gradients will not be computed. The extrusion distance should be on the order of the smallest mesh dimension. For axisymmetric 2D geometries, apply symmetry conditions to the hightheta and lowtheta planes unless there is swirl anticipated in the flow, in which case, 1:1 periodic connections should be applied instead. Do not use GGI periodic connections; doing so will hurt accuracy. The extrusion rotation angle for axisymmetric geometries should be small (for example, 1 to 5 degrees). 

October 15, 2015, 05:47 

#7 
Senior Member
hamidi
Join Date: Sep 2012
Posts: 251
Rep Power: 7 
i appreciate you for all.
The only thing that I did not understand this is: what is differnce within planar and axisymmetric 2D geometries? as i know both have symmetry relative to axis. if your possible, please express axisymmetric geometries with an example, whether it can be a shaft? best wishes 

October 15, 2015, 05:51 

#8  
Member
Join Date: Jan 2015
Posts: 63
Rep Power: 4 
Quote:
Axisymmetric 2D is symmetric relative to an axis (representative of a body of revolution). 

October 15, 2015, 07:27 

#9 
Senior Member
hamidi
Join Date: Sep 2012
Posts: 251
Rep Power: 7 
thanks a lot for clear explanation
therefore figure as shown is an example of axisymmetric geometry, that is correct? 

October 15, 2015, 07:30 

#10  
Member
Join Date: Jan 2015
Posts: 63
Rep Power: 4 
Quote:
https://en.wikipedia.org/wiki/Solid_of_revolution Can you obtain your geometry by revolving a 2D Sketch around an axis? 

October 15, 2015, 07:39 

#11 
Senior Member
hamidi
Join Date: Sep 2012
Posts: 251
Rep Power: 7 
dear highorder , i am sorry for inattention , previous figure that i sent was one planar geometry.
thanks infinitely for attention and rapid answer 

March 12, 2016, 15:30 

#12 
Senior Member
hamidi
Join Date: Sep 2012
Posts: 251
Rep Power: 7 
[QUOTE=highorder_cfd;568358]Planar means a standard 2D planar problem (there is no symmetry axis).
hello dear all Does the above definition is correct about planar objects? (unless triangle is not a planar object? And it is symmetric to the y axis. kind regards Last edited by hamidciv; March 13, 2016 at 03:03. 

March 12, 2016, 17:41 

#13 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,298
Rep Power: 103 
I have had a quick look at this thread and highorder's comments appear to be correct.


March 13, 2016, 03:08 

#14 
Senior Member
hamidi
Join Date: Sep 2012
Posts: 251
Rep Power: 7 
thanks dear glenn
if i understand concept it correctly, meant of symmetric relative to axis is same revolve relative to axis, that dont exist in planar objects. thanks in advance 

March 13, 2016, 04:20 

#15 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,298
Rep Power: 103 
I do not understand your question.
Are you saying should you put a symmetry condition on the central axis of a 2D axisymmetric simulation? 

March 13, 2016, 16:35 

#16 
Senior Member
hamidi
Join Date: Sep 2012
Posts: 251
Rep Power: 7 
hi dear glenn
Are you saying should you put a symmetry condition on the central axis of a 2D axisymmetric simulation? yes, in really, whether i can removing part of symmetric geometry of central axis and defining central axis as symmetry condition? i studied manual of cfx about this, as i attcahed in following:  For axisymmetric 2D geometries, apply symmetry conditions to the hightheta and lowtheta planes unless there is swirl anticipated in the flow, in which case, 1:1 periodic connections should be applied instead. Do not use GGI periodic connections; doing so will hurt accuracy. The extrusion rotation angle for axisymmetric geometries should be small (for example, 1 to 5 degrees) if your possible, are you have an example of geometry for high theta and low theta and also 1:1 periodic connection or GGI? unforunately i dont understand above sentences exactly. with the best wishes hamid Last edited by hamidciv; March 15, 2016 at 13:04. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Contact simulation Problem  nguyenthanhctm  FLUENT  0  December 19, 2013 09:21 
SimpleFoam convergence problem with really simple simulation  mayank.dce2k7  OpenFOAM Running, Solving & CFD  2  November 19, 2013 06:28 
Low pressure de Laval simulation convergence problem  heksel8i  FLUENT  3  July 22, 2013 10:28 
about valve closing problem during ANSYS FSI simulation  ivy  CFX  4  June 8, 2011 21:01 
Largescale simulation problem  Purushothama  Main CFD Forum  0  November 7, 2010 21:12 