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

problem in 2D simulation?

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

Like Tree6Likes
  • 1 Post By highorder_cfd
  • 1 Post By highorder_cfd
  • 1 Post By highorder_cfd
  • 1 Post By highorder_cfd
  • 1 Post By highorder_cfd
  • 1 Post By ghorrocks

Reply
 
LinkBack Thread Tools Display Modes
Old   October 13, 2015, 17:33
Default problem in 2D simulation?
  #1
Senior Member
 
hamidi
Join Date: Sep 2012
Posts: 234
Rep Power: 7
hamidciv is on a distinguished road
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
Attached Images
File Type: jpg 2015-10-10_191028.jpg (51.5 KB, 10 views)
hamidciv is offline   Reply With Quote

Old   October 14, 2015, 11:47
Default
  #2
Member
 
Join Date: Jan 2015
Posts: 46
Rep Power: 3
highorder_cfd is on a distinguished road
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.
hamidciv likes this.

Last edited by highorder_cfd; October 14, 2015 at 17:39.
highorder_cfd is offline   Reply With Quote

Old   October 14, 2015, 13:32
Default
  #3
Senior Member
 
hamidi
Join Date: Sep 2012
Posts: 234
Rep Power: 7
hamidciv is on a distinguished road
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


hamidciv is offline   Reply With Quote

Old   October 14, 2015, 13:58
Default
  #4
Member
 
Join Date: Jan 2015
Posts: 46
Rep Power: 3
highorder_cfd is on a distinguished road
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.
hamidciv likes this.

Last edited by highorder_cfd; October 14, 2015 at 17:49.
highorder_cfd is offline   Reply With Quote

Old   October 14, 2015, 15:14
Default
  #5
Senior Member
 
hamidi
Join Date: Sep 2012
Posts: 234
Rep Power: 7
hamidciv is on a distinguished road
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.
hamidciv is offline   Reply With Quote

Old   October 14, 2015, 16:30
Default
  #6
Member
 
Join Date: Jan 2015
Posts: 46
Rep Power: 3
highorder_cfd is on a distinguished road
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 high-theta and low-theta 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).
hamidciv likes this.
highorder_cfd is offline   Reply With Quote

Old   October 15, 2015, 05:47
Default
  #7
Senior Member
 
hamidi
Join Date: Sep 2012
Posts: 234
Rep Power: 7
hamidciv is on a distinguished road
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
hamidciv is offline   Reply With Quote

Old   October 15, 2015, 05:51
Default
  #8
Member
 
Join Date: Jan 2015
Posts: 46
Rep Power: 3
highorder_cfd is on a distinguished road
Quote:
Originally Posted by hamidciv View Post
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 with an example.
best wishes
Planar means a standard 2D planar problem (there is no symmetry axis).

Axisymmetric 2D is symmetric relative to an axis (representative of a body of revolution).
hamidciv likes this.
highorder_cfd is offline   Reply With Quote

Old   October 15, 2015, 07:27
Default
  #9
Senior Member
 
hamidi
Join Date: Sep 2012
Posts: 234
Rep Power: 7
hamidciv is on a distinguished road
thanks a lot for clear explanation
therefore figure as shown is an example of axisymmetric geometry, that is correct?
Attached Images
File Type: jpg 2015-10-15_151115.jpg (32.1 KB, 5 views)
hamidciv is offline   Reply With Quote

Old   October 15, 2015, 07:30
Default
  #10
Member
 
Join Date: Jan 2015
Posts: 46
Rep Power: 3
highorder_cfd is on a distinguished road
Quote:
Originally Posted by hamidciv View Post
thanks a lot for clear explanation
therefore figure as shown is a axisymmetric geometry, that is correct?
An axisymmetric geometry is a body of revolution.
https://en.wikipedia.org/wiki/Solid_of_revolution

Can you obtain your geometry by revolving a 2D Sketch around an axis?
hamidciv likes this.
highorder_cfd is offline   Reply With Quote

Old   October 15, 2015, 07:39
Default
  #11
Senior Member
 
hamidi
Join Date: Sep 2012
Posts: 234
Rep Power: 7
hamidciv is on a distinguished road
dear highorder , i am sorry for inattention , previous figure that i sent was one planar geometry.
thanks infinitely for attention and rapid answer
hamidciv is offline   Reply With Quote

Old   March 12, 2016, 15:30
Default
  #12
Senior Member
 
hamidi
Join Date: Sep 2012
Posts: 234
Rep Power: 7
hamidciv is on a distinguished road
[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.
hamidciv is offline   Reply With Quote

Old   March 12, 2016, 17:41
Default
  #13
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,838
Rep Power: 100
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
I have had a quick look at this thread and highorder's comments appear to be correct.
hamidciv likes this.
ghorrocks is offline   Reply With Quote

Old   March 13, 2016, 03:08
Default
  #14
Senior Member
 
hamidi
Join Date: Sep 2012
Posts: 234
Rep Power: 7
hamidciv is on a distinguished road
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
hamidciv is offline   Reply With Quote

Old   March 13, 2016, 04:20
Default
  #15
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,838
Rep Power: 100
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
I do not understand your question.

Are you saying should you put a symmetry condition on the central axis of a 2D axisymmetric simulation?
ghorrocks is offline   Reply With Quote

Old   March 13, 2016, 16:35
Default
  #16
Senior Member
 
hamidi
Join Date: Sep 2012
Posts: 234
Rep Power: 7
hamidciv is on a distinguished road
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 high-theta and low-theta 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.
hamidciv 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
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
Large-scale simulation problem Purushothama Main CFD Forum 0 November 7, 2010 21:12


All times are GMT -4. The time now is 20:37.