
[Sponsors] 
June 27, 2013, 05:12 
Fluid Structure Interaction

#1 
Member

I am using Ansys 14.5.7 and is looking for FSI effect of Gas Turbines...However I am facing some problem for the Data Transfer for doing the 2 way FSI which is vital as I am not able to transfer forces as it is not highlighting..Can anybody shed some light on it?


July 5, 2013, 04:44 

#2 
Senior Member
Matthias Voß
Join Date: Mar 2009
Location: Berlin, Germany
Posts: 446
Rep Power: 12 
Fluent or CFX?
I don´t get: "which is vital as I am not able to transfer forces as it is not highlighting.." Where in CFD or in CSM? Last edited by mvoss; July 8, 2013 at 02:58. 

July 14, 2013, 23:20 
Transfer of Forces in CFD

#3 
Member

Hi,
I am unable to transfer the incremental displacement from solid surface to fluid domain where fluid forces need to be transferred in Ansys Workbench, CFD toolbar. 

July 15, 2013, 03:42 

#4 
Senior Member
Matthias Voß
Join Date: Mar 2009
Location: Berlin, Germany
Posts: 446
Rep Power: 12 
Did check for the tutorials?
How did you set up the connections between CFD and CSM? Transient or steadystate? CFX or Fluent? Actually it´s hard not to transfer the forces/displacement in the wb2.0 when setting up an FSIrun. With no info about the CFD/CSM you´re using it´s hard to provide any type of constructive help. 

July 2, 2014, 07:23 
2 way FSI verification problem

#5 
Member
David
Join Date: Aug 2013
Posts: 30
Rep Power: 4 
Hi,
I have modeled a transient blood flow in a simple flexible tube ( by 2 way FSI in Ansys14.5 (structural + CFX)). simulation was carried out for 15 periods of time (in order to fully eliminate start up effects) and the normalized longitudinal velocity with respect to non dimensional radius of the tube was plotted (as shown in the attached figure), the fluid and solid properties are: Fluid: viscosity = 0.004 density = 1060 Solid: E(Young’s modulus (Linear))=20000000 v(Poisson ratio)=0.49 density =1000 and Geometric parameter values are: radius = 0.005mm thickness = 0.0005mm length= 0.42mm but the problem is my numerical solution does not verify by analytical solution ( in the attached figure dash lines are numerical solutions and solid lines are analytical solution) and I found that the radial displacement values of the tube wall are lower than its corresponding analytical solution values. I have checked the analytical solution for many times but it is true, and my numerical solution is not dependent to time step and grid size. Please help me to fix this. Last edited by mrkmrk; July 20, 2014 at 16:27. 

July 3, 2014, 13:23 

#6 
Senior Member
Join Date: Apr 2009
Posts: 530
Rep Power: 13 
What are your fluid and structural boundary conditions? What assumptions are used in the analytical solution? Do you have a mesh independent solution?


July 4, 2014, 11:52 
2 way FSI verification problem

#7 
Member
David
Join Date: Aug 2013
Posts: 30
Rep Power: 4 
Hi stumpy,
thanks for your response Fluid boundary condition: Opening pressure inlet at the tube entrance: p_inlet= 30+1000 Sin (2*pi*t) (unit: pa) And opening pressure outlet at the tube outlet: P_outlet= (993*Sin ((2*pi*t  0.014855095))) (unit: pa) “993” and “0.014855095” is due to considering complex exponential oscillations for u, v, w, p in analytical solution in the form u=U*exp (i*2*pi(tx/c)) v=V*exp (i*2*pi(tx/c)) w=W*exp (i*2*pi(tx/c)) p=P*exp (i*2*pi(tx/c)) Wave speed (c) in the analytical solution for flexible tube is complex. And fluid structure interaction interface at the wall of tube. ************************************************** ************************ Structural boundary condition: Fixed support at the inlet and the outlet of tube to prevent rigid body motion and fluid structure interaction interface at the inner wall of the tube and the outer wall is not constrained. ************************************************** ************************ Analytical solution assumptions [1]: a/L<<1 , U/C_0<<1 Where a is the tube radius, L is the tube length, U is average longitudinal velocity and C_0 is the speed of wave propagation in rigid tube which is defined by: C_0= sqrt (E*h/ (2*ro*a)) E: Young’s modulus, h: tube thickness, ro: fluid density 1. Zamir M. The physics of pulsatile flow. New York: SpringerVerlag; 2000. p. 113–145. ************************************************** ******* For meshing structural domain: I tried Automatic and sweep method (both manual source and manual thin) also when I used manual thin Ansys gave more displacement but it was still lower than analytical solution. And for meshing the fluid domain both tetrahedral and multizone method was considered but this did not help too. ************************************************** ********* In the FSI interface boundary condition in CFX, in the boundary details tab, only ‘Total mesh displacement’ receive from ANSYS and only ‘Total force send to ANSYS and in Mass and Momentum section ‘no slip wall’ and wall velocity relative to ‘mesh motion’ was considered. Is this true? Can the mesh stiffness near boundaries affect the solution? (I use Ansys default) Last edited by mrkmrk; July 23, 2014 at 09:08. 

July 4, 2014, 14:54 

#8 
Senior Member
Join Date: Apr 2009
Posts: 530
Rep Power: 13 
Are the fixed supports at the inlet/outlet really valid? Should the tube be allowed to stretch there so you aren't restricting the flow?
I'm not sure if that outlet boundary condition in CFX is a good boundary condition to use either. It feels like you are trying to impose the analytical solution on the CFD solution, rather than let the CFD solution solve the case. I'm not sure what a good condition is though. If the end of the tube is open then just use zero Static Pressure. 

July 20, 2014, 09:47 
2 way FSI verification problem

#9 
Member
David
Join Date: Aug 2013
Posts: 30
Rep Power: 4 
Hi stumpy,
thanks for your useful information and I really appreciate your help, I changed the structural boundary conditions to fixed support for inlet side and remote displacement (only rotations are constrained) for the other side. and I used zero Static Pressure for the outlet boundary condition of the fluid part. but the problem was not solved. I tried to simplify my problem, and rerun it for 3 different conditions: first I simulate the fluid flow in a rigid tube, then I simulate the fluid flow in a flexible tube which its young modulus was 2e+17 and in the third case the simulation was carried out in a tube which its young modulus was 3.85e+05, in the rigid tube the results verified by analytical solution completely and the results of the second and the first simulation were the same with approximately no difference (as it was expected) but the result of the third simulation has significant difference in comparison to its corresponding analytical solution. For all cases the inlet boundary condition was opening pressure inlet (30*cos(2*pi*t)) and the outlet boundary condition was opening zero Static Pressure.) what parameters can increase this numerical solution errors when I decrease the young modulus(except reduction of the analytical solution accuracy by decreasing the young modulus)? Last edited by mrkmrk; July 20, 2014 at 16:25. 

July 21, 2014, 11:42 

#10 
Senior Member
Join Date: Apr 2009
Posts: 530
Rep Power: 13 
I would recommend trying to verify the structural solution before you look at the FSI solution any further. Can you get an analytical solution when a constant pressure is applied to the structure, then verify this?
Some things to think about on the structural side include:  If you are using solid elements then you need at least 2 elements through the thickness, or use Full Integration rather than the default Reduced Integration (switch Element Control to Manual for the Body/Part)  If you are using shell elements, and your geometry represents the inside radius of the pipe, then you need to offset the nodes to the top or bottom shell layer (depending on your element normal).  Is Large Deflection set to On? 

July 22, 2014, 04:05 
Measuring mean flow in Ansys Fluent

#11 
Member

Hi,
I want to measure the mean flow rate in Ansys Fluent...I am using SAS Turbulent model,compressible flow..Any suggestion from anybody will help me to proceed furthur.. 

July 22, 2014, 14:21 
2 way FSI verification problem

#12 
Member
David
Join Date: Aug 2013
Posts: 30
Rep Power: 4 
Hi stumpy,
Thank you for your very useful information, (I did not know about them before) I read about solid45 3D in this URL: www.ansys.stuba.sk/html/elem_55/chapter4/ES445.htm But I can't understand what you said in the third case. I applied a constant pressure with a magnitude of 300 pa perpendicular to the inner side of the tube, by the Hooke’s law for thin walled cylinder the radial and the axial displacement should be equal to 6.2*e07 and 6.6*e08 respectively. ************************************************** ******* Hooke’s law: Radial displacement=(1/E)*((2sigma)*stress_l)*r Axial displacement=(1/E)*((1(2*sigma))*stress_l)*L Where sigma is the Poisson ratio (= 0.499) and "stress_l" is axial stress(= p*r/(2*thickness)) ************************************************** ******* Here is the numerical solution of the structural domain: By fixed support constraint in two sides: Max radial displacement= 6.6*e07 Max axial displacement= 7.71*e08 (however I used fixed support!) By remote displacement constraint in two sides (only rotations are constrained): Max radial displacement= 8.27*e07 Max axial displacement= 1.49*e05 (does not verify by analytical solution!) In all simulations the element type is solid (because they can give better convergence) and there are four elements through the tube thickness and large deflection is set to on. (I changed element control to manual but the "rigid body behavior" did not change (still is set to "dimensionally reduced") therefore I decided to increase elements through the tube thickness) I also rerun the FSI simulation (this time with four elements through the tube thickness) but the results did not change. It seems that the fluid does not understand the solid part displacements. I want to use the "SOLSH190" elements in the ansys structural, can you tell me how should I do this? Last edited by mrkmrk; July 24, 2014 at 05:14. 

July 24, 2014, 09:18 

#13 
Senior Member
Join Date: Apr 2009
Posts: 530
Rep Power: 13 
To use SOLSH190 you need to mesh the pipe using the "Sweep" method. Within this method there's an option for "Thin Sweep" then a further option to mesh with solid shells.


Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Fluid Structure Interaction using icoFsiFoam Problems  lr103476  OpenFOAM Running, Solving & CFD  79  August 7, 2014 09:30 
Fluid structure interaction on baloons  vinz  OpenFOAM Running, Solving & CFD  37  June 3, 2008 10:03 
Optimization or fluid structure interaction  Steve_NTUA  Main CFD Forum  9  August 29, 2006 03:40 
Fluid structure interaction  tomm  FLUENT  2  September 16, 2004 04:33 
Fluid Structure Interaction  Gabor Balint  FLUENT  2  January 5, 2000 14:08 