[ddungntu]

Dear all,

Thank you very much for your time and energy to give me your kind help.

I am trying to simulate the water block hitting a steel plate with velocity =4 m/s, using Ansys CFX (2-way FSI). I am interested in solution of pressure acting on steel plate and plate deformation.
To simulate this problem, I applied two-phase problem by introducing volume fraction of air and water. Then I applied the initial velocity=4 m/s to the water block, and 0 m/s for air domain. I defined all sides of fluid domain except for top of air domain as no slip wall, for the top of air domain defined as openning boundary with open pressure=0 Pa.
But unfortunately, the results of pressure and deformation obtained are small compared to what I expected.
I do not know what is wrong in my model.

Could you please tell me about boundary condition and initial conditions or other aspects to improve my solution?

Best regards,
Dac Dung

[ghorrocks]

FAQ: https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F

Have you done a no-FSI simulation of water hitting a plate to check you can model that accurately? If you can't model the simple one accurately you have no hope of getting the more complex FSI case accurate.

Have you done a mesh size, convergence tolerance, time step size and boundary proximity sensitivity analysis? These are the key steps to ensure accuracy in most CFD simulations.

[ddungntu]

Dear Dr. Glenn,

Thank you very much for your response.

Actually I am new to CFX, so I have tried to do some examples such as oscillating plate from CFX tutorial and follow you post FAQ as well.

Because time constraint I cannot perform many convergence studies.
Since I want to compare the result using CFX with LS-Dyna which I done before, so I keep the mesh size = 100x100x100 mm as the same in LS-Dyna. I set time step size =0.0005 s, (this keeps the Courant number is less than 1). My model is the full scale =5x3x3 m, it is so big and I cannot set time step size smaller because it take so long time for analysis. I used residual as MAX=0.001.

I would like to ask you for further suggestions.
Are the boundary condition and initial condition proper?

Dac Dung

[ghorrocks]

I am not talking about doing tutorials. I am assuming you have done enough of them to know how the software works. I am talking about validation and verification, which is the process you need to do to ensure an accurate simulation. The CFX tutorials do not cover any V&V work (but should, in my opinion).

You cannot tell whether your mesh, time step size, boundary proximity or convergence criteria are OK by simply listing the numbers. You need to do a sensitivity analysis to check.

I also cannot say about your boundary condition choice without more information. An image of what you are doing would help.

[ddungntu]

https://plus.google.com/photos/photo...CPfx_rLcjt65LA

Thank you for your information.

I attached a image showing my model for illustration.
Fist I would like to confirm whether my setting is correct based on my situation: a water column hit a clamped plate with velocity =4 m/s; I just make quarter model only.

Hope to see your further recommendations.

[ghorrocks]

Please post images directly onto the forum, not as links to third party sites. This FAQ describes how: https://www.cfd-online.com/Wiki/Ansy...n_the_forum.3F

From your image it appears you have symmetry in 2 planes. In this case you only need to CFD and FEA model 1/4 of the geometry. Is this what you have done? If so, provided this is compatible with what you want to do this is fine. Note that I don't know what you want to do so I am guessing there.

[ddungntu]

Sorry for my mistake on posting image.

I just posted two images showing my model and results of force and pressure.

Actually, I want to to simulate a quarter model for a water column hitting a steel plate with velocity =4 m/s. I am interesting in solution of pressure acting on steel plate and plate deformation.
To simulate this problem, I applied two-phase problem by introducing volume fraction of air and water. Then I applied the initial velocity=4 m/s to the water block, and 0 m/s for air domain. I defined all sides of fluid domain except for top of air domain and symmetry planes as no slip wall, for the top of air domain defined as openning boundary with open pressure=0 Pa, and for two symmetry planes I used symmetry boundaries.

However, at beginning the force (red line) and pressure (green line) increased suddenly as shown in the attached image, and also the finally the results of force is small.

Untitled1.png

Untitled2.png

I would like to know what is setting may I do to overcome this problem.

[AtoHM]

I don't really see your problem. You have this value only in the zero'th iteration so maybe it comes from the initialization. However, they go to zero in the first step so it seems to be ok and not diverging. How did you initialize the velocity of the air?

The plots make sense to me, as the block hits the plate there will be a timestep with max force / pressure and then the water will distribute / leave the domain whatever and those values decay to zero.
You can always print some transient results to see how the fluid is moving in time and judge if it makes sense (this does not replace a propper convergence study but gives an idea if results make sense).

[ddungntu]

Dear Dr. AtoHM,

Thank you very much for your suggestions. Your information is really helpful to me.

Regarding the initialization, I set initial velocity 4 m/s for the water column, and 0 m/s for the air domain.
I also defined all sides of air (except for the top of air and the two symmetry planes), as wall boundary with No slip wall. The top of air was set as openning boundary with pressure =0 Pa (openning press.). The two symmetry planes were defined as symmetry boundary.

Should I set velocity = 4 m/s for the air (same as water) using initialization? or should I define the inlet boundary at bottom of air with velocity =4 m/s? Because I think when the water column moves up with 4 m/s the surrounding air may have the same velocity? Please kindly correct me about that.

Hope to see your help.

[ghorrocks]

I agree with AtoHM, I can't see the problem. The results you are getting appear to be physical. If they are not please show us what is not correct.

The block of water starts a short distance below the plate, so it will take some time for the water block to hit the plate. During this wait time there will be very low force on the plate (which is what you are getting). Then there will be a high force as the water hits the plate and gets splashed sideways, but the water will quickly start falling away from the plate and the force will again drop to a low value. This appears to match what you are getting in your results. So can you explain what here is not correct?

[ddungntu]

Dear Dr. Glenn,

Thank you very much for your nice explanation. Now you already cleared my solution that my model is fine.

Regarding what I worry about my model seems to be wrong, actually I have done this simulation with LS-Dyna using ALE (Arbitrary Lagrangian-Eulerian) algorithm/solver, and the results from my colleagues using Star-CCM. Both simulations used the same mesh size (100x100x100 mm), time step size and initial conditions. However, although I used the same main things such as mesh size and time step size and initial condition, my results from CFX is only half of those from both software in terms of maximum deflection and maximum vertical force.
That why I thought my model was wrong, so I needed your correction of my problem.

Could you please point out me which parameters should I define to improve my model?

[AtoHM]

Please don't call us Dr. - at least I am not a Dr.
My question regarding the initialization is, how did you apply the velocities you mentioned to the fluids? How do you define where the water is located in the initialization?

My idea was that there might be something wrong there and lets assume the air is also initialized with 4 m/s. Then it will "hit" the plate was well -> right at the start of the simulation causing this peak in force. However the rest of the simulation looks fine in terms of behavior so we probably don't need to discuss this further.

I worked with LS-DYNA once but don't know how the fluid mechanics are modelled there. We did a solid-solid impact simulation back in the day. If something similar was used to investigate this water hits wall problem, there was maybe some simplification made modelling the water as a "solid" body with water density. Then this would probably lead to higher values in force and deflection as well. But thats just a guess.

[ghorrocks]

I am a Dr

Now you already cleared my solution that my model is fine.

No, I did not say that. I said that the main features I see in your results look plausible. Whether that is fine or not depends on many more factors like how accurate you want to be, and I don't know that.

Star-CCM, LS-DYNA and CFX are very different solvers. You should not assume that they will work OK with the same mesh, time step or convergence. You should do a verification and validation exercise on each solver to check each solver is giving the most accurate results it can before you compare between them. If you do not V&V the solution then you are comparing random numbers and that is not very meaningful.

[ddungntu]

Originally Posted by AtoHM

Please don't call us Dr. - at least I am not a Dr.
My question regarding the initialization is, how did you apply the velocities you mentioned to the fluids? How do you define where the water is located in the initialization?

My idea was that there might be something wrong there and lets assume the air is also initialized with 4 m/s. Then it will "hit" the plate was well -> right at the start of the simulation causing this peak in force. However the rest of the simulation looks fine in terms of behavior so we probably don't need to discuss this further.

I worked with LS-DYNA once but don't know how the fluid mechanics are modelled there. We did a solid-solid impact simulation back in the day. If something similar was used to investigate this water hits wall problem, there was maybe some simplification made modelling the water as a "solid" body with water density. Then this would probably lead to higher values in force and deflection as well. But thats just a guess.

Thank you for your nice explanation and information.

I only set 4 m/s for water block and 0 m/s for air. I set the location of the water by using expression of volume fraction (if(x>=0[m] && x<=2[m] && y>=0[m] && y<=4[m] && z>=0.4[m] && z<=1.5[m], 1, 0)).

Is there better way to define the water block location?

[ddungntu]

Originally Posted by ghorrocks

I am a Dr



No, I did not say that. I said that the main features I see in your results look plausible. Whether that is fine or not depends on many more factors like how accurate you want to be, and I don't know that.

Star-CCM, LS-DYNA and CFX are very different solvers. You should not assume that they will work OK with the same mesh, time step or convergence. You should do a verification and validation exercise on each solver to check each solver is giving the most accurate results it can before you compare between them. If you do not V&V the solution then you are comparing random numbers and that is not very meaningful.

Dear Dr. Glenn,

Thank you so much for your kind explanation. I now understand your meaning.
I would like to pay more attention on V&V before comparing the results of each solver.

Once again thank you very much for your time and patience.

Best regards.
Dac Dung