Initializing transient analysis using static analysis in two-way FSI simulation

stumpy · July 9, 2014, 11:52

I'm not sure why the continuity residuals would be high. If other residuals are low then it could just be the way the residuals are normalized. The default residual normalization in Fluent is not the best. You can change to local scaling to get a better residual normalization. Under Monitors > Residuals, pick "compute local scale" then set the reporting option to "local scaling".

For smoothing the Diffusion smoothing is the most robust, but Spring should work OK too for this case.

Setting the reference pressure to the min transient pressure sounds good.

In the data transfers the actual force values are passed to the structure.

Daniel_Khazaei · July 9, 2014, 20:27

"You can change to local scaling to get a better residual normalization"

Velocity residuals are normal, it is only the continuity. Nevertheless, residual reporting is now OK with your suggestion about local scaling.

"Setting the reference pressure to the min transient pressure sounds good.
In the data transfers the actual force values are passed to the structure."

Changing reference pressure alters the force sending to structure part.
The mean pressure in my case is 13784.46 Pa, however minimum pressure is 10964.52 Pa.

These different values will change the final result, as they change force magnitude on the structure.

-----------

how can I set monitor points for force, displacement on FSI interface in fluent?

Thanks in advance

stumpy · July 10, 2014, 09:53

Can you assume the min pressure of 10964.52 Pa is consistent with the MRI scan geometry? Then you could adjust your pressure levels so that you always pass a positive pressure.
For force I find it easiest to monitor the Data Transfer Sum in System Coupling. Alternatively you can monitor the integral of Static Pressure in Fluent, which will be close to the force. For displacement you'll have to create a Results Tracker in Mechanical. If you use the Show Mesh option in Mechanical then you can pick a mesh node, otherwise you have to pick a geometry vertex.

Daniel_Khazaei · July 10, 2014, 17:40

"Can you assume the min pressure of 10964.52 Pa is consistent with the MRI scan geometry?"

You mean that the MRI image based geometry has its current shape (initial) due to the min pressure of 10964.52 Pa?
They have only provided the mass flow waveform at the inlet of CCA. I have no pressure related information on my geometry.
I am using pressure waveform presented in the publications with the same geometry.

"Then you could adjust your pressure levels so that you always pass a positive pressure."

How can I make this adjustment?
When I set the reference pressure to mean blood pressure, I get pressure in range of: (almost)
[-3000 Pa, 3000 Pa]

However, setting reference pressure to min blood pressure gives pressure in range of: (almost)
[0 Pa, 6000 Pa]

Daniel_Khazaei · July 11, 2014, 21:18

Would you please clarify a few things for me:

1) How many coupling iteration is normal in tightly coupled simulation?

I have read that I should keep number of coupling iteration below 10!
Ansys recommendation for transient: min:1 and max:5

2) I have set the RSM convergence target in system coupling to 1E-04, should I still expect the simulation to converge within 10 coupling iteration?

3) The fluent part hardly converges below 1E-4, should I expect that?
Fluid only transient simulation converges below 1E-5 in 6 iteration over each time step.

stumpy · July 14, 2014, 10:57

1) The number of Coupling Iterations can vary from case to case, but it should be possible to converge just about any case in 10 or less Coupling Iteration. The key point is not to use too much under-relaxation, since this will slow convergence too much. If a case is unstable from a coupling perspective (i.e. force/displacement oscillate and diverge within a coupling step) then don't reduce the under-relaxation. You should use Solution Stabilization in Fluent instead.

2) If this is the Data Transfer convergence target then 1e-4 is a very tight tolerance. I would expect it to take more coupling iterations to reach this target. So yes, more than 10 coupling iterations may be needed. I doubt you need that tight of a tolerance though. Monitor your quantities of interest and see when they are converged.

3) I assume these values are with the local scaling option. I'm not sure why Fluent wouldn't converge as well with FSI when compared to fluid-only. 1e-4 isn't too bad. As long as your quantities of interest are converged then this convergence level sounds OK.

Daniel_Khazaei · July 16, 2014, 08:06

As you suggested, very low under relaxation was needed to get convergence. Hence, I have decided to use stabilization in dynamic mesh setup on system coupling zone.

With the following setting, I was able to get convergence within 5 coupling iteration in the first time step:

- Fluent convergence target based on local scaling: 5E-05
- Force convergence target in system coupling: 1E-03
- Displacement convergence target in system coupling: 1E-03

Also I am just testing the first step to determine the optimal coefficient-based scaling factor:

Scale factors higher than 7 prevent crashing and huge oscillations, however the solution does not converge within 10 coupling iteration until I set a very large value of 450.

Solver output for scale factor = 450:

Code:

======================================================================
 +====================================================================+
 |                                                                    |
 |                              Solution                              |
 |                                                                    |
 +====================================================================+
 ======================================================================

 +--------------------------------------------------------------------+
 |                        MAPPING SUMMARY                             |
 +--------------------------------------------------------------------+
 | Data Transfer                    |                                 |
 |   Diagnostic                     |   Source Side     Target Side   |
 +----------------------------------+---------------------------------+
 | Data Transfer 2                  |                                 |
 |   Percent Nodes Mapped           |       N/A             100       |
 | Data Transfer                    |                                 |
 |   Percent Nodes Mapped           |       100             100       |
 |   Percent Area Mapped            |       100             100       |
 +--------------------------------------------------------------------+

 +====================================================================+
 | COUPLING STEP =      1              SIMULATION TIME = 2.00000e-003 |
 |--------------------------------------------------------------------|
 | Solver                           |         Solution Status         |
 |   Data Transfer                  |                                 |
 |     Diagnostics                  |   Source Side     Target Side   |
 +====================================================================+
 |                     COUPLING ITERATION = 1                         |
 +--------------------------------------------------------------------+
 | Transient Structural             |           Converged             |
 |- - - - - - - - - - - - - - - - - + - - - - - - - - - - - - - - - - |
 |   Data Transfer                  |       Not yet converged...      |
 |     Change:RMS                   |   1.00000e+000   1.00000e+000   |
 |--------------------------------------------------------------------|
 | transient FSI Fluent             |       Not yet converged...      |
 |- - - - - - - - - - - - - - - - - + - - - - - - - - - - - - - - - - |
 |   Data Transfer 2                |       Not yet converged...      |
 |     Change:RMS                   |   1.00000e+000   1.00000e+000   |
 +--------------------------------------------------------------------+
 |                     COUPLING ITERATION = 2                         |
 +--------------------------------------------------------------------+
 | Transient Structural             |           Converged             |
 |- - - - - - - - - - - - - - - - - + - - - - - - - - - - - - - - - - |
 |   Data Transfer                  |       Not yet converged...      |
 |     Change:RMS                   |   1.22517e-002   1.22517e-002   |
 |--------------------------------------------------------------------|
 | transient FSI Fluent             |           Converged             |
 |- - - - - - - - - - - - - - - - - + - - - - - - - - - - - - - - - - |
 |   Data Transfer 2                |       Not yet converged...      |
 |     Change:RMS                   |   4.32637e-002   4.32637e-002   |
 +--------------------------------------------------------------------+
 |                     COUPLING ITERATION = 3                         |
 +--------------------------------------------------------------------+
 | Transient Structural             |           Converged             |
 |- - - - - - - - - - - - - - - - - + - - - - - - - - - - - - - - - - |
 |   Data Transfer                  |       Not yet converged...      |
 |     Change:RMS                   |   1.41697e-003   1.41697e-003   |
 |--------------------------------------------------------------------|
 | transient FSI Fluent             |           Converged             |
 |- - - - - - - - - - - - - - - - - + - - - - - - - - - - - - - - - - |
 |   Data Transfer 2                |       Not yet converged...      |
 |     Change:RMS                   |   6.29899e-003   6.29899e-003   |
 +--------------------------------------------------------------------+
 |                     COUPLING ITERATION = 4                         |
 +--------------------------------------------------------------------+
 | Transient Structural             |           Converged             |
 |- - - - - - - - - - - - - - - - - + - - - - - - - - - - - - - - - - |
 |   Data Transfer                  |           Converged             |
 |     Change:RMS                   |   2.48035e-004   2.48035e-004   |
 |--------------------------------------------------------------------|
 | transient FSI Fluent             |           Converged             |
 |- - - - - - - - - - - - - - - - - + - - - - - - - - - - - - - - - - |
 |   Data Transfer 2                |       Not yet converged...      |
 |     Change:RMS                   |   2.17488e-003   2.17488e-003   |
 +--------------------------------------------------------------------+
 |                     COUPLING ITERATION = 5                         |
 +--------------------------------------------------------------------+
 | Transient Structural             |           Converged             |
 |- - - - - - - - - - - - - - - - - + - - - - - - - - - - - - - - - - |
 |   Data Transfer                  |           Converged             |
 |     Change:RMS                   |   5.81177e-005   5.81177e-005   |
 |--------------------------------------------------------------------|
 | transient FSI Fluent             |           Converged             |
 |- - - - - - - - - - - - - - - - - + - - - - - - - - - - - - - - - - |
 |   Data Transfer 2                |           Converged             |
 |     Change:RMS                   |   2.10873e-004   2.10873e-004   |
 +====================================================================+

 ======================================================================
 +====================================================================+
 |                                                                    |
 |                          Shut Down                                 |
 |                                                                    |
 +====================================================================+
 ======================================================================


 System Coupling Service shut down...

 System coupling run completed successfully.

Now I have question about over-damping, how can I check that I am not over-damping the solution?

here is the force summery:

Code:

 *** FORCE SUM ACROSS TARGET INTERFACE . . . . .Fluid Solid Interface (FSIN_1)
     RECEIVING FORCE FX SUM =  0.69983E-02
     RECEIVING FORCE FY SUM = -0.13517E-03
     RECEIVING FORCE FZ SUM =  0.87715E-02

   COUPLING ITERATION. . . . . . . . . . . . . . .     2

 *** FORCE SUM ACROSS TARGET INTERFACE . . . . .Fluid Solid Interface (FSIN_1)
     RECEIVING FORCE FX SUM =  0.62144E-02
     RECEIVING FORCE FY SUM =  0.29081E-03
     RECEIVING FORCE FZ SUM =  0.88670E-02

 *** FORCE SUM ACROSS TARGET INTERFACE . . . . .Fluid Solid Interface (FSIN_1)
     RECEIVING FORCE FX SUM =  0.63194E-02
     RECEIVING FORCE FY SUM =  0.18824E-03
     RECEIVING FORCE FZ SUM =  0.88334E-02

   COUPLING ITERATION. . . . . . . . . . . . . . .     4

 *** FORCE SUM ACROSS TARGET INTERFACE . . . . .Fluid Solid Interface (FSIN_1)
     RECEIVING FORCE FX SUM =  0.62649E-02
     RECEIVING FORCE FY SUM =  0.23105E-03
     RECEIVING FORCE FZ SUM =  0.88437E-02

   COUPLING ITERATION. . . . . . . . . . . . . . .     5

 *** FORCE SUM ACROSS TARGET INTERFACE . . . . .Fluid Solid Interface (FSIN_1)
     RECEIVING FORCE FX SUM =  0.62679E-02
     RECEIVING FORCE FY SUM =  0.22082E-03
     RECEIVING FORCE FZ SUM =  0.88426E-02

stumpy · July 16, 2014, 11:43

To avoid over-damping it is best to start with the unstable solution and increase the coefficient until you approach the converged solution. The unstable solution will have oscillations that grow in magnitude. As you increase the coefficient you'll move to oscillations that decrease in magnitude, then to a critically damped response (i.e. a slight overshoot then convergence), then to over-damped (no overshoot, steadily approaching the converged solution).
A case that has a slight overshoot in the force/displacement monitor values, then approaches convergence, is the ideal response. Look at the force/displacement values obtained with this case. If you use a very large coefficient of 450 you may be so over-damped that the solution is almost stationary, which may give "converged" residual values, but the wrong answer.
If you haven't reached the same force/displacement value as the case that has a slight overshoot, then you have too much damping. I would focus more on the monitor point convergence than on reaching specific residual targets. Residuals can be misleading.

Daniel_Khazaei · July 20, 2014, 20:52

Hello again

I have tried to find the optimal scale factor for my case, starting with unstable solution while slowly increasing the scale factor.

I have set 2 different result trackers in Structural to monitor displacement.
After reaching to scale factor equal to 1.5, one of these monitor points shows the behavior you have described, however the other one looks unstable.

Also I am monitoring integral of static pressure on the arterial wall, however it's stable no matter what.
When I use small scale factors, continuity equation never reaches the residual criteria with very slow convergence.

---------

I am also working on a much simpler 2D case involving an elastic flap in a channel.
The exact same problem with continuity equation is also there. (Without local scaling continuity residual goes beyond 1e+1)
However, velocity components converge smoothly under 1E-5.

I have noticed that the continuity converges well when I disable the solution stabilization in dynamic mesh, but structural crashes at the second coupling iteration.

Best wishes

yonpanman · January 17, 2017, 06:03

Sorry for opening this thread again but I noticed that you have discussed the initialization of "steady" FSI results with system coupling, Fluent and Mechanical. I was wondering if it's possible doing this and then changing to the pressure-based solver when the initialization is done with the density-based solver?

Regards!

Edit: I see, pressure-density coupling, not density based solver. My bad.

Another question though, when trying to do this initialise I have to run quite many time steps in order to get a good convergence in fluent. I tried to use a large time step but when doing that the RMS in system coupling didn't converge well. I actually have a hard time getting the RMS down for smaller time steps as well. Any ideas on how to deal with this?

yk2359 · September 12, 2017, 11:56

Quote:

Originally Posted by Daniel_Khazaei

Yes, I am planning to perform a fluid-structure interaction in a vessel.

1) fluid mesh is generated in ICEM (att, fluid)

2) surface mesh which is the same on both sides (fluid & solid). (att, surfaceMesh)

3) solid mesh is the generated by extruding the surface mesh by an specific thickness.

However, it seems that system coupling is unable to read that and mapping summery reports 0 percent mapped.

Hello Daniel,

Did you manage to get this work? Please let me know. Thanks.

July 9, 2014, 11:52		#41
stumpy Senior Member Join Date: Apr 2009 Posts: 531 Rep Power: 21	I'm not sure why the continuity residuals would be high. If other residuals are low then it could just be the way the residuals are normalized. The default residual normalization in Fluent is not the best. You can change to local scaling to get a better residual normalization. Under Monitors > Residuals, pick "compute local scale" then set the reporting option to "local scaling". For smoothing the Diffusion smoothing is the most robust, but Spring should work OK too for this case. Setting the reference pressure to the min transient pressure sounds good. In the data transfers the actual force values are passed to the structure. Daniel_Khazaei likes this.

July 9, 2014, 20:27		#42
Daniel_Khazaei Senior Member Daniel Join Date: Mar 2013 Location: Noshahr, Iran Posts: 348 Rep Power: 21	"You can change to local scaling to get a better residual normalization" Velocity residuals are normal, it is only the continuity. Nevertheless, residual reporting is now OK with your suggestion about local scaling. "Setting the reference pressure to the min transient pressure sounds good. In the data transfers the actual force values are passed to the structure." Changing reference pressure alters the force sending to structure part. The mean pressure in my case is 13784.46 Pa, however minimum pressure is 10964.52 Pa. These different values will change the final result, as they change force magnitude on the structure. ----------- how can I set monitor points for force, displacement on FSI interface in fluent? Thanks in advance Last edited by Daniel_Khazaei; July 10, 2014 at 08:13.

July 10, 2014, 09:53		#43
stumpy Senior Member Join Date: Apr 2009 Posts: 531 Rep Power: 21	Can you assume the min pressure of 10964.52 Pa is consistent with the MRI scan geometry? Then you could adjust your pressure levels so that you always pass a positive pressure. For force I find it easiest to monitor the Data Transfer Sum in System Coupling. Alternatively you can monitor the integral of Static Pressure in Fluent, which will be close to the force. For displacement you'll have to create a Results Tracker in Mechanical. If you use the Show Mesh option in Mechanical then you can pick a mesh node, otherwise you have to pick a geometry vertex. Daniel_Khazaei likes this.

July 10, 2014, 17:40		#44
Daniel_Khazaei Senior Member Daniel Join Date: Mar 2013 Location: Noshahr, Iran Posts: 348 Rep Power: 21	"Can you assume the min pressure of 10964.52 Pa is consistent with the MRI scan geometry?" You mean that the MRI image based geometry has its current shape (initial) due to the min pressure of 10964.52 Pa? They have only provided the mass flow waveform at the inlet of CCA. I have no pressure related information on my geometry. I am using pressure waveform presented in the publications with the same geometry. "Then you could adjust your pressure levels so that you always pass a positive pressure." How can I make this adjustment? When I set the reference pressure to mean blood pressure, I get pressure in range of: (almost) [-3000 Pa, 3000 Pa] However, setting reference pressure to min blood pressure gives pressure in range of: (almost) [0 Pa, 6000 Pa] Last edited by Daniel_Khazaei; July 11, 2014 at 21:02.

July 11, 2014, 21:18		#45
Daniel_Khazaei Senior Member Daniel Join Date: Mar 2013 Location: Noshahr, Iran Posts: 348 Rep Power: 21	Would you please clarify a few things for me: 1) How many coupling iteration is normal in tightly coupled simulation? I have read that I should keep number of coupling iteration below 10! Ansys recommendation for transient: min:1 and max:5 2) I have set the RSM convergence target in system coupling to 1E-04, should I still expect the simulation to converge within 10 coupling iteration? 3) The fluent part hardly converges below 1E-4, should I expect that? Fluid only transient simulation converges below 1E-5 in 6 iteration over each time step. Last edited by Daniel_Khazaei; July 12, 2014 at 09:05.

July 14, 2014, 10:57		#46
stumpy Senior Member Join Date: Apr 2009 Posts: 531 Rep Power: 21	1) The number of Coupling Iterations can vary from case to case, but it should be possible to converge just about any case in 10 or less Coupling Iteration. The key point is not to use too much under-relaxation, since this will slow convergence too much. If a case is unstable from a coupling perspective (i.e. force/displacement oscillate and diverge within a coupling step) then don't reduce the under-relaxation. You should use Solution Stabilization in Fluent instead. 2) If this is the Data Transfer convergence target then 1e-4 is a very tight tolerance. I would expect it to take more coupling iterations to reach this target. So yes, more than 10 coupling iterations may be needed. I doubt you need that tight of a tolerance though. Monitor your quantities of interest and see when they are converged. 3) I assume these values are with the local scaling option. I'm not sure why Fluent wouldn't converge as well with FSI when compared to fluid-only. 1e-4 isn't too bad. As long as your quantities of interest are converged then this convergence level sounds OK. Daniel_Khazaei likes this.

July 16, 2014, 11:43		#48
stumpy Senior Member Join Date: Apr 2009 Posts: 531 Rep Power: 21	To avoid over-damping it is best to start with the unstable solution and increase the coefficient until you approach the converged solution. The unstable solution will have oscillations that grow in magnitude. As you increase the coefficient you'll move to oscillations that decrease in magnitude, then to a critically damped response (i.e. a slight overshoot then convergence), then to over-damped (no overshoot, steadily approaching the converged solution). A case that has a slight overshoot in the force/displacement monitor values, then approaches convergence, is the ideal response. Look at the force/displacement values obtained with this case. If you use a very large coefficient of 450 you may be so over-damped that the solution is almost stationary, which may give "converged" residual values, but the wrong answer. If you haven't reached the same force/displacement value as the case that has a slight overshoot, then you have too much damping. I would focus more on the monitor point convergence than on reaching specific residual targets. Residuals can be misleading. Daniel_Khazaei and mrkmrk like this.

July 20, 2014, 20:52		#49
Daniel_Khazaei Senior Member Daniel Join Date: Mar 2013 Location: Noshahr, Iran Posts: 348 Rep Power: 21	Hello again I have tried to find the optimal scale factor for my case, starting with unstable solution while slowly increasing the scale factor. I have set 2 different result trackers in Structural to monitor displacement. After reaching to scale factor equal to 1.5, one of these monitor points shows the behavior you have described, however the other one looks unstable. Also I am monitoring integral of static pressure on the arterial wall, however it's stable no matter what. When I use small scale factors, continuity equation never reaches the residual criteria with very slow convergence. --------- I am also working on a much simpler 2D case involving an elastic flap in a channel. The exact same problem with continuity equation is also there. (Without local scaling continuity residual goes beyond 1e+1) However, velocity components converge smoothly under 1E-5. I have noticed that the continuity converges well when I disable the solution stabilization in dynamic mesh, but structural crashes at the second coupling iteration. Best wishes Last edited by Daniel_Khazaei; July 21, 2014 at 01:28.

January 17, 2017, 06:03		#50
yonpanman New Member Johannes Hall Join Date: Sep 2016 Posts: 21 Rep Power: 10	Sorry for opening this thread again but I noticed that you have discussed the initialization of "steady" FSI results with system coupling, Fluent and Mechanical. I was wondering if it's possible doing this and then changing to the pressure-based solver when the initialization is done with the density-based solver? Regards! Edit: I see, pressure-density coupling, not density based solver. My bad. Another question though, when trying to do this initialise I have to run quite many time steps in order to get a good convergence in fluent. I tried to use a large time step but when doing that the RMS in system coupling didn't converge well. I actually have a hard time getting the RMS down for smaller time steps as well. Any ideas on how to deal with this? Last edited by yonpanman; January 17, 2017 at 10:00.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Fluid structure interaction	jnattia	Main CFD Forum	25	May 21, 2015 10:16
vortex shedding, transient or steady state analysis type?	alfonsojurado	CFX	0	October 25, 2012 06:33
Transient analysis of particle flow with Fluid-Structure Interaction (FSI)	Julian K.	STAR-CCM+	2	October 11, 2011 11:19
Transient analysis of particle flow with Fluid-Structure Interaction (FSI)	Julian K.	FLUENT	0	September 14, 2011 16:40
FSI Simulation unsing ANSYS Multifield	k_buz	CFX	2	April 6, 2009 18:40