[mvoss]

Load both meshes into Post And Check If they line up.
If there is no error besides the 0% carefully check the dimensions (m vs. mm).

[Daniel_Khazaei]

Originally Posted by mvoss

Load both meshes into Post And Check If they line up.
If there is no error besides the 0% carefully check the dimensions (m vs. mm).

I have tried to do that, however solid mesh is not shown in the CFD-post.

Does Ansys FSI simulation require the presence of geometry?
Have you ever used only mesh files (fluid and solid) to setup a FSI simulation?

I have generated both meshes in ICEM CFD.
I have created the fluid mesh and then I have used the surface mesh of the fluid (extrude normal) to create the solid part.

Best wishes

[mvoss]

Solid Mesh is shown in post (only 3D!!). Disable the Fluid And rezoom the window. This is exactly what i was suggesting by "checking the dimensions".
And yes- geometry needs to be persistent afaik.
What do you mean by "presence of geometry"?

[Daniel_Khazaei]

Originally Posted by mvoss

Solid Mesh is shown in post (only 3D!!). Disable the Fluid And rezoom the window. This is exactly what i was suggesting by "checking the dimensions".
And yes- geometry needs to be persistent afaik.

I will check it and comeback.

Have you ever used only mesh files (fluid and solid) to setup a FSI simulation?

"What do you mean by "presence of geometry"?" : I didn't load any geometries only meshes have been imported.

I have generated both meshes in ICEM CFD.
I have created the fluid mesh and then I have used the surface mesh of the fluid (extrude normal) to create the solid part.

[Daniel_Khazaei]

Originally Posted by mvoss

Solid Mesh is shown in post (only 3D!!). Disable the Fluid And rezoom the window. This is exactly what i was suggesting by "checking the dimensions".
And yes- geometry needs to be persistent afaik.
What do you mean by "presence of geometry"?

Hello Sir,

Thanks for your help.
Inconsistent unit system in FE Modeler was the cause.
Global unit system was correct, however unit system of FE Modeler was set to mm.

----------

I have some general questions regarding FSI in Ansys:

1) Is it possible to run a steady-state 2-way FSI using Fluent and Mechanical and use it as an initial condition for transient case?

2) How can I stabilize the solution without reducing the relaxation factors?
I know there is an option in dynamic mesh setup to stabilize the solution, however I can not find any documentation for it.

[skinnyfluid]

Hello Daniel,

Leave your e-mail address and I'll send you some documentation.

[Daniel_Khazaei]

Originally Posted by skinnyfluid

Hello Daniel,

Leave your e-mail address and I'll send you some documentation.

Hello

Here is my email address:

shadowfax2011@gmail.com

Did you have any success in your method of initializing the transient solution?
I have tried that but it seems that there is no exchange of data before actually solving one part.

Does ansys exchange data for initial conditions?

Best wishes

[stumpy]

Regarding initializing a transient FSI with steady-state FSI results....

As you found you cannot mix Transient Structural with steady-state Fluent (this is the approach used with CFX FSI). Also, if you solve a steady-state case FSI then you cannot switch it to transient and then restart. So the only solution is less than ideal....

Use a Transient Structural system with Time Integration set to Off. This will behave like a Static Structural solution. Fluent will need to be transient too, but use solver settings so that it behaves more like a steady-state solution. The training material that you can download from ANSYS says:
- Use the pressure based coupled solver with 1 iteration per time step
- Set the Flow Courant Number to 1e6 of higher (under Solution Controls)
- Set the Explicit Relaxation Factor to 1 for Momentum and Pressure
- Set the Time Step Size in System Coupling as if you were solving a pseudo-transient steady-state case

You'll need Fluent to march forward in time, which means you'll need to set the end time in System Coupling so that many Coupling Steps are performed. Use 1 Coupling Iteration per step. Once this finishes you should have a converged "steady state" FSI solution. To restart:
- In Mechanical turn on time integration and then manually pick the restart point
- In Fluent edit the Solution cell and adjust the solver settings so you can resolve the real transient. Save or "sync with Workbench" before you proceed.
- In System Coupling extend the End Time and adjust the time step.
- Solve!

Hope this works Ok.

[Daniel_Khazaei]

Originally Posted by stumpy

Regarding initializing a transient FSI with steady-state FSI results....

As you found you cannot mix Transient Structural with steady-state Fluent (this is the approach used with CFX FSI). Also, if you solve a steady-state case FSI then you cannot switch it to transient and then restart. So the only solution is less than ideal....

Use a Transient Structural system with Time Integration set to Off. This will behave like a Static Structural solution. Fluent will need to be transient too, but use solver settings so that it behaves more like a steady-state solution. The training material that you can download from ANSYS says:
- Use the pressure based coupled solver with 1 iteration per time step
- Set the Flow Courant Number to 1e6 of higher (under Solution Controls)
- Set the Explicit Relaxation Factor to 1 for Momentum and Pressure
- Set the Time Step Size in System Coupling as if you were solving a pseudo-transient steady-state case

You'll need Fluent to march forward in time, which means you'll need to set the end time in System Coupling so that many Coupling Steps are performed. Use 1 Coupling Iteration per step. Once this finishes you should have a converged "steady state" FSI solution. To restart:
- In Mechanical turn on time integration and then manually pick the restart point
- In Fluent edit the Solution cell and adjust the solver settings so you can resolve the real transient. Save or "sync with Workbench" before you proceed.
- In System Coupling extend the End Time and adjust the time step.
- Solve!

Hope this works Ok.

Thank you very much for the help.

Only one question, what does this step mean:

- Set the Time Step Size in System Coupling as if you were solving a pseudo-transient steady-state case

does it mean I need to adjust a large time step or there is way to determine that?

Best wishes

[stumpy]

Yes, it means to use a large time step. Typically you might choose some fraction (perhaps 20%) of the residence time of the fluid in the domain, but this can be very much case dependent. Larger time steps will reach a steady-state faster, but could be less stable (but in some cases small time steps can be less stable too, since you'll start to resolve transient physics that is not of interest).

[Daniel_Khazaei]

Originally Posted by stumpy

Yes, it means to use a large time step. Typically you might choose some fraction (perhaps 20%) of the residence time of the fluid in the domain, but this can be very much case dependent. Larger time steps will reach a steady-state faster, but could be less stable (but in some cases small time steps can be less stable too, since you'll start to resolve transient physics that is not of interest).

Thanks for your help.

When I use steady-state with pseudo transient and Time scale factor 1 every thing is fine.
In the new version, ANSYS 15, pseudo transient method can only be activated if I select steady-state and that gives inconsistency in system coupling.
I have seen that this method was part transient mode in ANSYS 14.

-------

I am a little bit confused about this method, I will try to explain:

- Use the pressure based coupled solver with 1 iteration per time step

This means that fluent solution is not fully converged in the first few iterations and then calculated forces are passed to the structural solver.
How the FSI solution can be stable in this situation?

[stumpy]

You cannot select pseudo-transient when Fluent is in transient mode. The idea is to get the transient solver to behave as close as possible to the pseudo-transient approach.

1 iteration per time step does seem low. I would suggest initializing Fluent with a converged steady-state flow to provide a good starting point for the steady-state FSI. 1 iteration per time step might then work OK, but feel free to try more iterations if that's not working.

[Daniel_Khazaei]

Originally Posted by stumpy

You cannot select pseudo-transient when Fluent is in transient mode. The idea is to get the transient solver to behave as close as possible to the pseudo-transient approach.

1 iteration per time step does seem low. I would suggest initializing Fluent with a converged steady-state flow to provide a good starting point for the steady-state FSI. 1 iteration per time step might then work OK, but feel free to try more iterations if that's not working.

I will try to test that.

As you can see, I have a vessel to model.
I have a velocity profile at the inlet and two pressure profile for each outlets.

Pressure force at the beginning of the simulation is in order of 10,000 Pa.
This cause significant deformation on the structure side.

I have tried to test the model using complete static simulation.
Static Structural and steady-state fluent.

After Fluent solved the fluid part, forces was received by the structural and caused significant deformation.
However, after that the Fluent solver crashed with negative cell volume error.

Also the fluid mesh has good quality:

Minimum Orthogonal Quality: 0.51
Aspect Ratio : 36.4
Skewness: 0.62


Best wishes

[stumpy]

From the looks of the geometry this is an artery simulation. A few things to keep in mind...

What does the geometry/mesh represent? Is it probably the pre-stressed structure due to blood pressure? If so, and assuming you haven't pre-stressed your structural model, then you probably want to set your fluid operating pressure to blood pressure so that you are not passing those forces to the structure. In other words that 10,000 Pa probably shouldn't deform the structure any further because you have generate the geometry/mesh based on the pre-stressed structure. Note that adjusting the operating pressure like this is only valid if you assume linear elastic material properties.

This will be a tightly coupled FSI simulation, so "Solution Stabilization" is likely needed for any transient simulations. You might be able to get a steady-state solution by just using a lot of under-relaxation on the forces/displacements.

[Daniel_Khazaei]

Originally Posted by stumpy

From the looks of the geometry this is an artery simulation. A few things to keep in mind...

What does the geometry/mesh represent? Is it probably the pre-stressed structure due to blood pressure? If so, and assuming you haven't pre-stressed your structural model, then you probably want to set your fluid operating pressure to blood pressure so that you are not passing those forces to the structure. In other words that 10,000 Pa probably shouldn't deform the structure any further because you have generate the geometry/mesh based on the pre-stressed structure. Note that adjusting the operating pressure like this is only valid if you assume linear elastic material properties.

This will be a tightly coupled FSI simulation, so "Solution Stabilization" is likely needed for any transient simulations. You might be able to get a steady-state solution by just using a lot of under-relaxation on the forces/displacements.

It is a Common Carotid Artery geometry obtained from the MRI images. I am working with a medical organization and they have provided the STL file for me from one of their patients. So it is an already pre-stressed geometry, isn't it?
So, I don't need to pre-stress the model again?

-----

"Note that adjusting the operating pressure like this is only valid if you assume linear elastic material properties."

You mean that I am not able to use nonlinear materials like mooney-rivlin,
If I set the operating pressure to mean blood pressure value (I have transient profile at the outlets)? What is wrong with that?
Is it related to the Mixed u-P Formulations for hyper-elastic materials?

Best wishes

[Daniel_Khazaei]

A few questions about setting operating condition, actually I am explaining the approach I am thinking about. (correct me if I am wrong):

1) Changing the operating pressure to the mean blood pressure calculated from the transient pressure profiles at the outlets.

2) Now I should make my transient profiles relative to this new operating pressure.

Correct?

------------------

How about changing the reference pressure only?
I mean leave the operating pressure untouched.
As forces are calculated based on the gauge pressure minus the Reference Pressure.

[stumpy]

So yes, since the geometry is based on the MRI scan then it represents a pre-stressed geometry. Let ignore linear/non-linear material properties for now. The forces you send to System Coupling should not include the blood pressure since the structure is already deformed due to those forces. You could adjust your operating pressure to 1[atm]+10,000[Pa], then your outlet pressure profile should be relative to this operating pressure (so you'll probably need to offset it by 10,000 [Pa]). Alternatively you can keep the operating pressure at 1[atm], keep the outlet pressure profile relative to 1[atm], then set the Reference Pressure to 10,000 [Pa]. Either approach is valid assuming the fluid is treated as constant density.
Now the problem with material properties...
For a linear material it will deform a certain amount when a certain force is applied. The amount it deforms does not depend on its pre-stress state (ignore geometric non-linearities for this discussion). For a non-linear material the amount it deforms does depend on its pre-stress state.
Here you've generated a geometry/mesh for a pre-stressed structure, but you are assuming zero initial stress in the model. So when you apply a force you won't get the correct displacements. I assume you don't know the actual stress values in the real pre-stressed geometry and you don't know the unstressed geometry. If you want to use non-linear material properties, then really you need to know one of these two things. You probably can't get that info, so you'll have to make some assumptions/best guesses.

[Daniel_Khazaei]

Thank you very much for the detailed explanation man.

I have calculated the mean blood pressure based on my transient profile which is 13,784 Pa.
At the start of simulation (based on the earlier steady-state solution) the average pressure is 12033.48 Pa.
So, I have a pressure force of -2000 Pa (approximately) at the start of my simulation.

Now I have setup the project with the information you have provided. (actually transient)
I have used steady-state fluid solution for the initialization of fluid part in the project.



Also I don't think that initializing with steady-state solution is working:
The steady-state solution is converged to 1e-8 for all variables, but when fluent starts in the FSI mode (first part in coupling sequence):

COUPLING STEP = 1	 COUPLING ITERATION = 1

Updating solution at time levels N and N-1.
 done.

Updating mesh at time level N... done.
  iter  continuity  x-velocity  y-velocity  z-velocity  surf-mon-1     time/iter
     1  1.0000e+00  0.0000e+00  0.0000e+00  0.0000e+00  1.2043e+04  0:00:36    3
     2  6.0442e-01  1.2594e-05  1.1826e-05  2.2378e-05  1.2043e+04  0:00:22    2
     3  4.1999e-01  1.1770e-05  1.1253e-05  1.7866e-05  1.2043e+04  0:00:10    1
     4  2.9589e-01  9.4289e-06  9.0572e-06  1.2348e-05  1.2043e+04  0:00:00    0
Flow time = 0.002s, time step = 1

I have expected a jump in the residuals but the above output is confusing, is it normal?

Default system coupling settings were used, however Structural solver crashed in the first coupling iteration.

What approach should I use since pre-stressing does seem irrelevant in my case?
Do I still need to do steady-state FSI before actual transient one?



Best wishes

[stumpy]

To check if Fluent is initialized correct you can scroll up the Fluent transcript file and look for some output that says Fluent is reading the dat file. If you don't see this, then something went wrong with the initialization.
Be careful when passing negative pressures to the structure. Since the structure is not pre-stressed then any negative pressures may cause it to completely collapse/buckle, unless you have something on the structural side that can resist a compression force (e.g. if the artery is bonded to some surrounding tissue). You might want to offset your pressures so that you only ever pass positive forces to the structure.
I can't see any reason to do a steady-state FSI before the transient. If you knew the zero-stress geometry then the steady-state FSI would be useful to get to the pre-stressed state, but that's probably not possible.

[Daniel_Khazaei]

"To check if Fluent is initialized correct you can scroll up the Fluent transcript file and look for some output that says Fluent is reading the dat file. If you don't see this, then something went wrong with the initialization."

It seems that fluent has read the data file of the steady-state solution.
Reading data file notification is there, also I can see the steady-state solution in transient Fluent.

But why continuity residuals are so high in my simulation?
jumps from 1e-8 to 1e+0 and remains near that.
Could it be related to dynamic mesh settings in Fluent?

There are 3 options presented in smoothing section, which one is commonly used for structured Hexa mesh?

"Be careful when passing negative pressures to the structure, You might want to offset your pressures so that you only ever pass positive forces to the structure."

I have set the reference pressure to the minimum pressure in my transient profile, does it have any side effect on the result?

How ansys treat forces in data transfer?

1) Actual Force value?
2) Force difference between each step?

Best Wishes