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

Divergence and High Aspect Ratios

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

Like Tree7Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   February 16, 2013, 18:32
Default
  #21
Senior Member
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,042
Rep Power: 17
flotus1 will become famous soon enough
Is this a picture of the actual mesh you are using?
If yes, add at least prism layers at the walls.

What mach number do you expect in your simulation? How high is the pressure at the inlet and outlet respectively?

Edit: Am I right assuming that the prism layers you added are so thin compared to the tet elements that they cannot be seen in the picture of your last post?
flotus1 is offline   Reply With Quote

Old   February 16, 2013, 18:37
Default
  #22
Member
 
Join Date: Sep 2012
Location: FL
Posts: 76
Rep Power: 4
victoryv is on a distinguished road
Quote:
Originally Posted by flotus1 View Post
Is this a picture of the actual mesh you are using?
If yes, add at least prism layers at the walls.

What mach number do you expect in your simulation? How high is the pressure at the inlet and outlet respectively?
I have added prism layers at the bottom wall.The Mach no is around 0.3. The pressure at the inlet is 103000 Pa and the outlet is what I have to find by comparing the exp results.
victoryv is offline   Reply With Quote

Old   February 16, 2013, 18:50
Default
  #23
Senior Member
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,042
Rep Power: 17
flotus1 will become famous soon enough
Since you are experiencing convergence issues, I would try a simulation with a velocity or mass flow inlet, at least to get better initial values for the following simulations.

Getting back to the prism layers, are you sure that the volume jump is better this time?

Additionally, I strongly recommend to use a hexa mesh, especially since the whole geometry basically consists of one hexaeder. A good mesh is one thing less to worry about in CFD
This could even be done with the Ansys mesher.
flotus1 is offline   Reply With Quote

Old   February 16, 2013, 18:57
Default
  #24
Member
 
Join Date: Sep 2012
Location: FL
Posts: 76
Rep Power: 4
victoryv is on a distinguished road
Quote:
Originally Posted by flotus1 View Post
Since you are experiencing convergence issues, I would try a simulation with a velocity or mass flow inlet, at least to get better initial values for the following simulations.

Getting back to the prism layers, are you sure that the volume jump is better this time?

Additionally, I strongly recommend to use a hexa mesh, especially since the whole geometry basically consists of one hexaeder. A good mesh is one thing less to worry about in CFD
This could even be done with the Ansys mesher.
I know the stagnation pressure and stagnation temp at inlet. Thats why I am using preesure inlet. yes, the volume jump is far better now. Yeah, i will try improving the mesh . If that does not succeed , I will try multizone mesh.
victoryv is offline   Reply With Quote

Old   February 16, 2013, 23:42
Default
  #25
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,902
Blog Entries: 6
Rep Power: 37
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
instead of symmetry , specify them as slip wall.

Extend domain by some unit lengths at inlet and outlet
Far is offline   Reply With Quote

Old   February 17, 2013, 01:33
Default
  #26
Member
 
Join Date: Sep 2012
Location: FL
Posts: 76
Rep Power: 4
victoryv is on a distinguished road
Quote:
Originally Posted by Far View Post
instead of symmetry , specify them as slip wall.

Extend domain by some unit lengths at inlet and outlet
Is there other option than symmetry for modeling slip walls?. Also, but if we extend the domain at the inlet and outlet, it changes the parameters (velocity, pressure) inside the domain right?

Last edited by victoryv; February 17, 2013 at 01:51.
victoryv is offline   Reply With Quote

Old   February 17, 2013, 02:13
Default
  #27
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,902
Blog Entries: 6
Rep Power: 37
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Specify extended walls as slip so you will not have any boundary layer development or pressure loss.

You can define as slip wall by specifying shear stress = 0. It will have same effect as symmetry. Moreover symmetry condition has some special purpose and it has different mathematical definition.
victoryv likes this.
Far is offline   Reply With Quote

Old   February 17, 2013, 02:26
Default
  #28
Member
 
Join Date: Sep 2012
Location: FL
Posts: 76
Rep Power: 4
victoryv is on a distinguished road
Quote:
Originally Posted by Far View Post
Specify extended walls as slip so you will not have any boundary layer development or pressure loss.

You can define as slip wall by specifying shear stress = 0. It will have same effect as symmetry. Moreover symmetry condition has some special purpose and it has different mathematical definition.
Oh, i totally forgot that we can specify shear stress in "wall" boundary condition. Thanks man . Also, i will try extending the the inlet and outlet.
victoryv is offline   Reply With Quote

Old   February 17, 2013, 03:27
Default
  #29
Senior Member
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,042
Rep Power: 17
flotus1 will become famous soon enough
Quote:
Originally Posted by Far View Post
You can define as slip wall by specifying shear stress = 0. It will have same effect as symmetry. Moreover symmetry condition has some special purpose and it has different mathematical definition.
This is the first time I heard of this. Are you sure? Where exactly is the difference?
flotus1 is offline   Reply With Quote

Old   February 17, 2013, 03:36
Default
  #30
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,902
Blog Entries: 6
Rep Power: 37
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
I always face convergence problems with symmetry, which is not the case with slip wall.

Quote:
Originally Posted by ghorrocks View Post
This is described in the documentation.

Symmetry enforces zero normal gradient to all parameters, and a slip wall does not necessarily do this. But for most normal simulations they are equivalent.

And a symmetry plane is required to be planar, but a slip wall can be any shape.


Quote:
Originally Posted by Martin Hegedus View Post
In general, slip and symmetry are much the same, if not exactly the same. But, sometimes it is implementation dependent. For example one could have p(-1)=p(1) for symmetry but p(0)=p(1) for wall. Also, the turbulence model boundary conditions could be different. OK, I don't know what it means to have a slip turbulence model, but I guess that depends on what someone is trying to do. Also, a turbulence model could depend on the distance from a surface. So it's possible that setting a far field condition to a wall will affect the turbulence model.

But, the answer, to first order, is that they are the same.
slip wall boundary condition
Far is offline   Reply With Quote

Old   February 17, 2013, 05:00
Default
  #31
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,902
Blog Entries: 6
Rep Power: 37
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
https://dl.dropbox.com/u/68746918/CFDNotes06.ppt

Refer to slide 54 and 57. Why two lateral boundaries are set as symmetry and top and bottom as slip-wall? What will be effect if two side (lateral ) boundaries are set to slip-wall or periodic? What will happen if top and bottom walls are defined as symmetry or periodic?

Edit : Some notes from CFX


victoryv and mrenergy like this.

Last edited by Far; February 17, 2013 at 05:45. Reason: Adding pics related to CFX help
Far is offline   Reply With Quote

Old   February 17, 2013, 08:42
Default
  #32
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,066
Rep Power: 15
RodriguezFatz will become famous soon enough
Hi, you should switch off energy equation and try to run the simulation. If that diverges too, please switch the inlet to velocity inlet and try if it works. Pressure inlet and outlet are not the easiest choice.
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   February 17, 2013, 13:10
Default reply for the wind tunnel simulation
  #33
New Member
 
hossam ali
Join Date: Jan 2013
Posts: 9
Rep Power: 4
hossam_ali is on a distinguished road
hi i think the problem in ur mesh skewness

u should remesh and decrease the skeness to be less than now and this will decrease the squinsh of the mesh (to be less than 0.9)
hossam_ali is offline   Reply With Quote

Old   February 18, 2013, 11:24
Default
  #34
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,066
Rep Power: 15
RodriguezFatz will become famous soon enough
Quote:
Originally Posted by hossam_ali View Post
hi i think the problem in ur mesh skewness

u should remesh and decrease the skeness to be less than now and this will decrease the squinsh of the mesh (to be less than 0.9)
Maybe (or belike) the mesh is the problem, but normally meshing is also the most time consuming part of the whole process, so rather than remeshing I would try to spot the problem before starting...
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   February 19, 2013, 01:26
Default
  #35
Member
 
Join Date: Sep 2012
Location: FL
Posts: 76
Rep Power: 4
victoryv is on a distinguished road
I have tried extending boundaries and slip walls. No use. Still it is diverging.
I will try incompressible flow and velocity inlet and simulate once again.
victoryv is offline   Reply With Quote

Old   February 19, 2013, 03:07
Default
  #36
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,066
Rep Power: 15
RodriguezFatz will become famous soon enough
Quote:
Originally Posted by victoryv View Post
I have tried extending boundaries and slip walls. No use. Still it is diverging.
I will try incompressible flow and velocity inlet and simulate once again.
You also had compressible flow? That's too much, you should really try to get simple settings running before switching on all additional equations...
Also, if you explain your case in a thread, please tell people everything about it and don't wait until post #50 to do so...
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   February 19, 2013, 04:57
Default
  #37
Member
 
Join Date: Sep 2012
Location: FL
Posts: 76
Rep Power: 4
victoryv is on a distinguished road
Quote:
Originally Posted by RodriguezFatz View Post
You also had compressible flow? That's too much, you should really try to get simple settings running before switching on all additional equations...
Also, if you explain your case in a thread, please tell people everything about it and don't wait until post #50 to do so...
I have written in the heading above the first post itself that I am doing steady state compressible. I am doing compressible because i have compressible results to compare with. Sorry for the confusion.
victoryv is offline   Reply With Quote

Old   February 19, 2013, 05:04
Default
  #38
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,066
Rep Power: 15
RodriguezFatz will become famous soon enough
My bad! I didn't know that posts have captions. Anyway, switch off all these additional equations when something does not work and try to run it.
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   April 6, 2013, 15:54
Default
  #39
Member
 
Join Date: Sep 2012
Location: FL
Posts: 76
Rep Power: 4
victoryv is on a distinguished road
I am facing a new problem now. I got rid of all the previous problems. The solution was taking a lot of time and many iterations to reach steady state. So I have used FMG initialization and pseudo transient method( time step 0.001) to make the convergence faster. When I was trying to find mesh independent solution, after 3rd refinement, the solution (pressure and velocity) started oscillating where it was supposed to reach state.

How did the mesh refinement led to oscillations?
If mesh is not the problem, what could be the problem?
victoryv is offline   Reply With Quote

Old   April 6, 2013, 17:08
Default
  #40
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,902
Blog Entries: 6
Rep Power: 37
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by victoryv View Post
I am facing a new problem now. I got rid of all the previous problems. The solution was taking a lot of time and many iterations to reach steady state. So I have used FMG initialization and pseudo transient method( time step 0.001) to make the convergence faster. When I was trying to find mesh independent solution, after 3rd refinement, the solution (pressure and velocity) started oscillating where it was supposed to reach state.

How did the mesh refinement led to oscillations?
If mesh is not the problem, what could be the problem?
Because refined mesh is capturing some unsteady flow phenomena which was not being captured in coarse mesh.
Far 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
[ANSYS Meshing] Very high aspect ratio zxin ANSYS Meshing & Geometry 12 August 16, 2011 10:49
Divergence detected in AMG solver:species-0 arulmurugan Fluent UDF and Scheme Programming 0 February 15, 2011 05:22
non zero divergence for incompressible flow! Pascal_doran OpenFOAM Running, Solving & CFD 17 September 21, 2010 11:22
multiphase flow, quick divergence of contuinity eq violet FLUENT 7 February 3, 2009 18:54
About divergence for help! xhliu1 CD-adapco 2 April 7, 2005 04:53


All times are GMT -4. The time now is 20:33.