# Why the generated waves disappear when moving away from the wavemaker?

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

 July 10, 2021, 19:51 Why the generated waves disappear when moving away from the wavemaker? #1 Member   Saeed Pashazanousi Join Date: Mar 2020 Location: Iran Posts: 51 Rep Power: 3 I simulated a NWT to study an elastic plate vibration fixed on the tank floor exposed to group waves. but the generated waves disappear before reaching the plate. I used ANSYS CFX with VOF model and Laminar flow model. NWT.PNG __________________ Best regards Saeed Pashazanousi Urmia University Tel: 0098 936 811 864 What's App: 0098 936 811 8647 Email: st_s.pashazanousi@urmia.ac.ir

 July 11, 2021, 19:58 #2 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 16,871 Rep Power: 132 I have no idea what a NWT is. Please do not assume people know what your acronyms mean. But the answer to your question is you have too much dissipation. This is probably due to a poor simulation setup, possibly things like: * Mesh too coarse * Not converging tight enough * Not high enough order advection scheme * Other numerics too diffusive (interpolation schemes on other variables) * Unsuitable advection scheme on VOF equation (should use compressive) * Time step too large * Need double precision numerics aero_head likes this. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

 July 18, 2021, 22:30 #3 Member   Saeed Pashazanousi Join Date: Mar 2020 Location: Iran Posts: 51 Rep Power: 3 Thanks, ghorrocks Sorry for late reply You're right. I'm sorry for that mistake. The NWT is the abbreviation for Numerical Wave tank. Let's back to my problem: The excitation period is about 2.96 sec and I considered the timestep equal to 0.01 sec. My computational mesh is 100 per wavelength and 21 per wave height in the free surface area. The free surface area height is about two-wave height. I used RMS residual target with 1E-4. Max. Coefficient loop of 200 used in CFX-pre and Max 20 Iteration for the coupling solver. Simulation Time=180 sec I selected these parameters according to recommendations in references and papers. What is your idea about these parameters? __________________ Best regards Saeed Pashazanousi Urmia University Tel: 0098 936 811 864 What's App: 0098 936 811 8647 Email: st_s.pashazanousi@urmia.ac.ir

 July 18, 2021, 22:35 #4 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 16,871 Rep Power: 132 Max coeff loops of 200 sounds way too high. 10 is more like what you want. Coupling solver? What does this mean? What coupling solver? Are you doing this as a FSI simulation? If so, why? __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

 July 18, 2021, 22:45 #5 Member   Saeed Pashazanousi Join Date: Mar 2020 Location: Iran Posts: 51 Rep Power: 3 Thanks for your quick reply I'm working on vibration of an elastic plate exposed to some group waves. I need to validate with a paper results. The paper used non-dimensional parameters. It's made it hard to validate for me! I think the 2 way FSI is the right solution! Do you have an other idea? __________________ Best regards Saeed Pashazanousi Urmia University Tel: 0098 936 811 864 What's App: 0098 936 811 8647 Email: st_s.pashazanousi@urmia.ac.ir

 July 18, 2021, 23:01 #6 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 16,871 Rep Power: 132 I would get this model working accurately as a CFD only simulation before adding FSI. Putting it another way, there is no point doing the FSI model when the CFD sub-model is inaccurate. So just do a CFD only model and get it working accurately. Then add the FSI bits. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

 July 18, 2021, 23:13 #7 Member   Saeed Pashazanousi Join Date: Mar 2020 Location: Iran Posts: 51 Rep Power: 3 You mean at first I should do a simulation with 1 way FSI or a simple numerical wave tank with rigid plate? I simulated an empty tank to validate Wavemaker theory! The results were in agreement with the theory! Please explain more if you can! Thanks ghorrocks! __________________ Best regards Saeed Pashazanousi Urmia University Tel: 0098 936 811 864 What's App: 0098 936 811 8647 Email: st_s.pashazanousi@urmia.ac.ir Last edited by pashazanousi; July 19, 2021 at 05:52.

 July 19, 2021, 00:13 #8 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 16,871 Rep Power: 132 A simple numerical wave tank with a rigid plate sounds like a good next step. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

 July 19, 2021, 05:51 #9 Member   Saeed Pashazanousi Join Date: Mar 2020 Location: Iran Posts: 51 Rep Power: 3 Thanks, ghorrocks I will try it and share the results here __________________ Best regards Saeed Pashazanousi Urmia University Tel: 0098 936 811 864 What's App: 0098 936 811 8647 Email: st_s.pashazanousi@urmia.ac.ir

 July 19, 2021, 08:07 #10 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 16,871 Rep Power: 132 You don't have to share it. What I describe is just good engineering practise: If you have a complex system of many parts and it does not work, then what is wrong? It is hard to fix as it is so complex. So separate out all the individual component systems and get them working properly by themselves. Time spent doing this at the beginning means that when the complex system fails to work (like it always does first time around) then you know the problem has to be the interaction between the systems, because all the systems by themselves work OK. This applies to any engineering system, not just CFD. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

 July 19, 2021, 08:50 #11 Member   Saeed Pashazanousi Join Date: Mar 2020 Location: Iran Posts: 51 Rep Power: 3 Thank you for your generosity ghorrocks You are so good and right is yours. I will do as you said. __________________ Best regards Saeed Pashazanousi Urmia University Tel: 0098 936 811 864 What's App: 0098 936 811 8647 Email: st_s.pashazanousi@urmia.ac.ir

 July 20, 2021, 19:24 #12 Member   Saeed Pashazanousi Join Date: Mar 2020 Location: Iran Posts: 51 Rep Power: 3 Hi ghorrocks I'm using a Desktop PC with these configurations: CPU: Intel 10600 corei5 Ram: 16 GB ram SSD & HDD: 240 GB+ 4 TB I want to set up a MPI Local Parallel but I don't know how should I do it. __________________ Best regards Saeed Pashazanousi Urmia University Tel: 0098 936 811 864 What's App: 0098 936 811 8647 Email: st_s.pashazanousi@urmia.ac.ir

 July 20, 2021, 20:12 #13 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 16,871 Rep Power: 132 Setting up parallel simulations is all described in the installation manual. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

 July 20, 2021, 20:53 #14 Member   Saeed Pashazanousi Join Date: Mar 2020 Location: Iran Posts: 51 Rep Power: 3 Thank you ghorrocks I study the manual about how set up a MPI Local parallel but honestly I understand almost nothing! But I defined a MPI Parallel Partition for CFX Solver with specified direction(1,0,0) and High Priority! I set 2 for allocated factor! I don't know are they the correct settings or not but Now the system is running well with 4 core (Max allowed partitions for free student version of Ansys). Thank you for your attention and the time you spent

 August 19, 2021, 15:51 #15 Member   Saeed Pashazanousi Join Date: Mar 2020 Location: Iran Posts: 51 Rep Power: 3 Hi ghorrocks I set the coupling residual equal to 0.01 (default value) and maximum coupling iteration equal to 20. Does this setting lead to a good result? __________________ Best regards Saeed Pashazanousi Urmia University Tel: 0098 936 811 864 What's App: 0098 936 811 8647 Email: st_s.pashazanousi@urmia.ac.ir

 August 19, 2021, 18:19 #16 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 16,871 Rep Power: 132 If you have parameters which you do not know if they are set correctly then do a sensitivity analysis to find out if they are important. Try coupling residuals of 0.001, 0.01 and 0.1 and see if it makes any difference. Likewise try max coupling iterations of 10, 20 and 40. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

 August 19, 2021, 21:01 #17 Member   Saeed Pashazanousi Join Date: Mar 2020 Location: Iran Posts: 51 Rep Power: 3 Thank you ghorrocks OK, I got it! I will do it! But I want to know what is the meaning of residual target in the coupling regions! For example for mesh transfer data from transient structural to CFX, I choose 0.01! It means 0.01 m as residual target? Or for Force Data transfer, 0.01 for residual target means 0.01 Newton? I need the residual target equal to 0.0001 m for the mesh displacement! I can't anything about that in Ansys help or other documents! __________________ Best regards Saeed Pashazanousi Urmia University Tel: 0098 936 811 864 What's App: 0098 936 811 8647 Email: st_s.pashazanousi@urmia.ac.ir

 August 19, 2021, 21:06 #18 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 16,871 Rep Power: 132 I don't know the exact definition of that residual target. All I can say is to look in the documentation. If you do a sensitivity analysis and show that you have set it tight enough that it is not affecting results then it does not matter what the exact definition is. It just means you have set it tight enough that your results are accurate (for that parameter at least). __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

 Tags ansys cfx, freesurface, fsi 2-way coupling, transient analisys, water waves