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

How to fix / solve local instability

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 28, 2016, 17:28
Default How to fix / solve local instability
  #1
Member
 
Hector Redal
Join Date: Aug 2010
Location: Madrid, Spain
Posts: 93
Rep Power: 8
HectorRedal is on a distinguished road
Hi,

I would like to know how a local instability can be fixed. Is there any strategy when choosing the parameters for the solver?

I am attaching an image of a local instability I am experiencing when simulating a flow past a circular cilinder. The flow is from left to right.

Best regards,
Hector.
Attached Images
File Type: jpg Local instability.jpg (90.5 KB, 19 views)
HectorRedal is offline   Reply With Quote

Old   April 29, 2016, 03:13
Default
  #2
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 2,692
Rep Power: 33
FMDenaro will become famous soon enoughFMDenaro will become famous soon enough
but running this solution for long time you get a numerical blow-up of the solution? Apparently it seems that something in the BC.c can be wrong...

However, check for the CFL and viscous stability parameters in that local region
FMDenaro is offline   Reply With Quote

Old   April 29, 2016, 06:14
Default
  #3
Member
 
Hector Redal
Join Date: Aug 2010
Location: Madrid, Spain
Posts: 93
Rep Power: 8
HectorRedal is on a distinguished road
Hi Filippo,

The instability appears after the flow has been stablished and had reached the end of the domain (right).
The boundary conditions I have using at the end of the domain are: du/dx = dv/dx = 0.

The CFL is far below the critical CFL (by a factor of 2 or more).

Best regards,
hector.
HectorRedal is offline   Reply With Quote

Old   April 29, 2016, 07:50
Default
  #4
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 2,692
Rep Power: 33
FMDenaro will become famous soon enoughFMDenaro will become famous soon enough
thus, this is not a numerical instability but a wiggle in the steady solution... check in which variables (those resolved in the code) you see such oscillations
FMDenaro is offline   Reply With Quote

Old   April 29, 2016, 08:28
Default
  #5
Senior Member
 
Arjun
Join Date: Mar 2009
Location: Nurenberg, Germany
Posts: 502
Rep Power: 13
arjun is on a distinguished road
Quote:
Originally Posted by HectorRedal View Post
Hi,

I would like to know how a local instability can be fixed. Is there any strategy when choosing the parameters for the solver?

I am attaching an image of a local instability I am experiencing when simulating a flow past a circular cilinder. The flow is from left to right.

Best regards,
Hector.

Could you check if you have reversed flow at this point of problem.

This information is important before any judgement be made because i know one way it could arise in case of reversed flow.
arjun is online now   Reply With Quote

Old   April 29, 2016, 10:01
Default
  #6
Member
 
Hector Redal
Join Date: Aug 2010
Location: Madrid, Spain
Posts: 93
Rep Power: 8
HectorRedal is on a distinguished road
Hi Arjun,

After the instability appears, the flow reverses and start growing and growing until it becomes very large.

The flow is supposed to be incompressible.

There are two parameters that control the time marching scheme (relaxation factors) that can be varied.
Theta1 for velocity which I set to 1.0 (It can be changed from 0.0 to 1.0)
Theta2 for pressure which I set to 1.0 (It can be changed from 0.0 to 1.0)

Best regards,
Hector.
HectorRedal is offline   Reply With Quote

Old   April 29, 2016, 10:02
Default
  #7
Member
 
Hector Redal
Join Date: Aug 2010
Location: Madrid, Spain
Posts: 93
Rep Power: 8
HectorRedal is on a distinguished road
Quote:
Originally Posted by FMDenaro View Post
thus, this is not a numerical instability but a wiggle in the steady solution... check in which variables (those resolved in the code) you see such oscillations
Which is the difference between wiggle and instability?

Maybe I have misunderstood you in my reply.
When the instability appears, there is not any steady state solution that can be reached.
HectorRedal is offline   Reply With Quote

Old   April 29, 2016, 10:27
Default
  #8
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 2,692
Rep Power: 33
FMDenaro will become famous soon enoughFMDenaro will become famous soon enough
Quote:
Originally Posted by HectorRedal View Post
Which is the difference between wiggle and instability?

Maybe I have misunderstood you in my reply.
When the instability appears, there is not any steady state solution that can be reached.
Numerical instability is a process that during the time integration drive the solution to blow-up, wiggle is a finite numerical (and unphysical) oscillation in the solution eve in the steady state.

Since your case is incompressible, I suggest to check the Div v = 0 constraint near the outflow
FMDenaro is offline   Reply With Quote

Old   April 29, 2016, 10:42
Default
  #9
Senior Member
 
Arjun
Join Date: Mar 2009
Location: Nurenberg, Germany
Posts: 502
Rep Power: 13
arjun is on a distinguished road
Quote:
Originally Posted by HectorRedal View Post
Which is the difference between wiggle and instability?
I think what he means is that wiggle appears but solver is able to recover from it.
Instability is some disturbance that keep growing until solver blows up the residuals.

Quote:
Originally Posted by HectorRedal View Post
Hi Arjun,

After the instability appears, the flow reverses and start growing and growing until it becomes very large.

The flow is supposed to be incompressible.

There are two parameters that control the time marching scheme (relaxation factors) that can be varied.
Theta1 for velocity which I set to 1.0 (It can be changed from 0.0 to 1.0)
Theta2 for pressure which I set to 1.0 (It can be changed from 0.0 to 1.0)

Best regards,
Hector.
The issue is that usually solvers add dynamic head at the pressure boundary to avoid reversed flow.

So if you specify pressure Pbnd at boundary, in case of reversed flow
it will be changed to

Pbnd - 1/2 density velocity sqr

It is done to remove reversed flow and it generally helps.

But sometimes what happens is that due to sudden change of boundary pressure from Pbnd to Pbnd - dynamic head, the pressure gradient at that cell sees sudden change.

What it means is that sudden change in fluxes and other things in that cell. Sometimes solver becomes instable or produces wiggles due to this.

I suspect what you see is this thing.
arjun is online now   Reply With Quote

Old   April 29, 2016, 10:43
Default
  #10
Senior Member
 
Arjun
Join Date: Mar 2009
Location: Nurenberg, Germany
Posts: 502
Rep Power: 13
arjun is on a distinguished road
For incompressible flow pressure urf of 1 is too high, I would hesitate to try above 0.3 usually.

Only in pressure based coupled solver that i have i use p urf around 0.9
arjun is online now   Reply With Quote

Old   April 29, 2016, 10:45
Default
  #11
Member
 
Hector Redal
Join Date: Aug 2010
Location: Madrid, Spain
Posts: 93
Rep Power: 8
HectorRedal is on a distinguished road
Quote:
Originally Posted by FMDenaro View Post
Numerical instability is a process that during the time integration drive the solution to blow-up, wiggle is a finite numerical (and unphysical) oscillation in the solution eve in the steady state.

Since your case is incompressible, I suggest to check the Div v = 0 constraint near the outflow
Thanks for the explanation.
Then I think that I am facing up an instability, since the solution blows up.
I have double check the boundary condition (at the outflow), and it appears to be well posed: du/dx = 0 and dv/dx=0, which I understand this is the normal way of specifying the constraints at exit flow.

On the other hand, I have been playing around with the time step (delta t), and after incresing the value of the delta t (from 0.001s to 0.005s) it seems it is working now. Why is this happening?
I have always believed that reducing the time step means incresing the accuracy of the solution.
This is someting that is puzzling me now. ???
HectorRedal is offline   Reply With Quote

Old   April 29, 2016, 10:47
Default
  #12
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 2,692
Rep Power: 33
FMDenaro will become famous soon enoughFMDenaro will become famous soon enough
Quote:
Originally Posted by HectorRedal View Post
Thanks for the explanation.
Then I think that I am facing up an instability, since the solution blows up.
I have double check the boundary condition (at the outflow), and it appears to be well posed: du/dx = 0 and dv/dx=0, which I understand this is the normal way of specifying the constraints at exit flow.

On the other hand, I have been playing around with the time step (delta t), and after incresing the value of the delta t (from 0.001s to 0.005s) it seems it is working now. Why is this happening?
I have always believed that reducing the time step means incresing the accuracy of the solution.
This is someting that is puzzling me now. ???

are you solving a Poisson pressure equation? check if the continuity constraint is satisfied by using your discretized BC.s. It is just sufficient check in a single time step what happen at the outflow
FMDenaro is offline   Reply With Quote

Old   April 29, 2016, 10:50
Default
  #13
Member
 
Hector Redal
Join Date: Aug 2010
Location: Madrid, Spain
Posts: 93
Rep Power: 8
HectorRedal is on a distinguished road
Quote:
Originally Posted by arjun View Post
For incompressible flow pressure urf of 1 is too high, I would hesitate to try above 0.3 usually.

Only in pressure based coupled solver that i have i use p urf around 0.9
I can try to use 0.3 as indicated, which I undestand is an semi-implicit strategy for the pressure. I will give it a try. I will inform you with the outcome.

By the way (only so as to frame the discussiion, in case it helps), the algorithm I am using is the Characteristics Based Split Algorithm which is a projection scheme for the Finite Element Method.
HectorRedal is offline   Reply With Quote

Old   April 29, 2016, 10:52
Default
  #14
Senior Member
 
Arjun
Join Date: Mar 2009
Location: Nurenberg, Germany
Posts: 502
Rep Power: 13
arjun is on a distinguished road
Quote:
Originally Posted by HectorRedal View Post
Thanks for the explanation.
Then I think that I am facing up an instability, since the solution blows up.
I have double check the boundary condition (at the outflow), and it appears to be well posed: du/dx = 0 and dv/dx=0, which I understand this is the normal way of specifying the constraints at exit flow.

On the other hand, I have been playing around with the time step (delta t), and after incresing the value of the delta t (from 0.001s to 0.005s) it seems it is working now. Why is this happening?
I have always believed that reducing the time step means incresing the accuracy of the solution.
This is someting that is puzzling me now. ???

What solver are you using btw.

Decreasing time step may introduce decoupling of pressure and velocity as it weakens the Rhie and Chow dissipation.
arjun is online now   Reply With Quote

Old   April 29, 2016, 17:29
Default
  #15
Member
 
Hector Redal
Join Date: Aug 2010
Location: Madrid, Spain
Posts: 93
Rep Power: 8
HectorRedal is on a distinguished road
Quote:
Originally Posted by arjun View Post
What solver are you using btw.

Decreasing time step may introduce decoupling of pressure and velocity as it weakens the Rhie and Chow dissipation.
For solving the poisson equation I am using a bi-conjugated gradient stabilizated solver.
I do not use any kind of Rhie and Chow dissipation.
Where can I find information about the Rhie and Chow dissipation. Do you know of any paper I can take a look at?
HectorRedal is offline   Reply With Quote

Old   April 29, 2016, 17:50
Default
  #16
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 2,692
Rep Power: 33
FMDenaro will become famous soon enoughFMDenaro will become famous soon enough
your problem is in the outflow BC.s, the dissipation term is used in cell-centred colocation to avoid pressure decoupling...

Check the BC for the pressure problem
FMDenaro is offline   Reply With Quote

Old   April 30, 2016, 11:28
Default
  #17
Member
 
Hector Redal
Join Date: Aug 2010
Location: Madrid, Spain
Posts: 93
Rep Power: 8
HectorRedal is on a distinguished road
Quote:
Originally Posted by FMDenaro View Post
your problem is in the outflow BC.s, the dissipation term is used in cell-centred colocation to avoid pressure decoupling...

Check the BC for the pressure problem
Hi Filippo,

I have checked the BC for the pressure and the velocity at the exit of the domain, and they appear to have been defined correctly.

I have also checked the gradient of the velocity at the exit, according to your previous suggestion, and you can see in the attached images that they are well defined.
I am attaching images for both gradients du/dx and dv/dx. At the exit it can be seen that they are both zero.

By the way, I have increased a bit more the delta t of the resolution and it appears is working as well.
Even the frequency of the vortex shedding approaches the value obtained by other references.
Attached Images
File Type: jpg Gradient_u0.jpg (66.6 KB, 9 views)
File Type: jpg Gradient_v0.jpg (52.7 KB, 8 views)
HectorRedal 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
How can I fix a local coordinate system to the inlet phys-zephyr STAR-CCM+ 3 May 8, 2014 05:46
How to write k and epsilon before the abnormal end xiuying OpenFOAM Running, Solving & CFD 8 August 27, 2013 15:33
same geometry,structured and unstructured mesh,different behaviour. sharonyue OpenFOAM Running, Solving & CFD 13 January 2, 2013 23:40
Transient simulation not converging skabilan OpenFOAM Running, Solving & CFD 12 September 17, 2007 17:48
Who has solve RichtmyerMeshkov RM instability by using VOF solver luckyluke OpenFOAM Running, Solving & CFD 0 May 31, 2005 03:52


All times are GMT -4. The time now is 21:24.