
[Sponsors] 
July 14, 2009, 02:50 
FSI modeling of blood vessel???

#1 
Member
Join Date: Jun 2009
Posts: 56
Rep Power: 7 
hi:
i 'm using the fsi modeling capability of ansys 11 to model a blood vessel.i use the appropriate material property of the artery E=4.e6 pa and poisson=0.45 and density=1062kg/m3...unfortunately the following error appears in the first itterations :"one or more elements become highle distorted..." and when i postprocess the unconverged ansys result i note that the high distortion is due to material properties,i mean that it works correctly for other materials such as steel or... would you please help me ?!i really need your help 

July 14, 2009, 05:39 

#2 
Senior Member
Lance
Join Date: Mar 2009
Posts: 480
Rep Power: 10 
Modeling blood vessels is really tricky since they are so elastic. The reason your simulations works for steel is that the Young's modulus is several magnitudes higher than your 4e6 Pa = less deformation.
Three things: * Hex mesh * Slowly ramp your pressure/velocity boundary conditions from zero to the initial value * Underrelaxation! 

July 15, 2009, 01:48 

#3 
Member
Join Date: Jun 2009
Posts: 56
Rep Power: 7 
Hi Lance and thx for your help:
please explain me more about ramping the loads!!! i use a waveform(pulsatile) velocity inlet with the maximum value of0.35 m/s and a constant outlet pressure of 12000pa(relative) for boundary conditions.also i use fixed supports and fsi interface for solid(vessel)...the initial condition at t=0 is zero for U,V,W,P...i have changed underrelaxations " external coupling setting tab in solver control" to about 0.20.4 but had no effect on solving... i really need your help 

July 15, 2009, 02:24 

#4 
Senior Member
Lance
Join Date: Mar 2009
Posts: 480
Rep Power: 10 
Ramp the pressure inside the entire domain from 0 to 12 kPa before starting the velocity waveform.


July 15, 2009, 02:42 

#5 
Member
Join Date: Jun 2009
Posts: 56
Rep Power: 7 
I dont understand...what do you mean?how can i ramp the outlet b.c.?what about the initial pressure and inlet b.c.?


July 15, 2009, 05:03 

#6 
Senior Member
George
Join Date: Mar 2009
Location: Birmingham, UK
Posts: 257
Rep Power: 8 
ramp example (check the manual for what aitern or atstep mean)
LIBRARY: CEL: EXPRESSIONS: CathCurrent = (5555) [A m^2] * rampCathodeIFlux(aitern) END FUNCTION: rampCathodeIFlux Argument Units = [] Option = Interpolation Profile Function = Off Result Units = [] INTERPOLATION DATA: Data Pairs = 0,1e6,10,1e3,30,1e1,60,0.5,80,0.75,100,1,150,1 Extend Max = Yes Extend Min = Yes Option = One Dimensional END END END END
__________________
Top 4 tips 1. Knowledge is everything and Ignorance is dangerous. 2. Understand your limitations and try to eliminate them. 3. Get yerself a bike and hoon the chuffer. You will soon learn why dogs like to hang their heads out the car window. 4. Please before asking any questions on how to run simulations in CFX, go though all the tutorials 

July 15, 2009, 05:12 

#7 
Senior Member
Lance
Join Date: Mar 2009
Posts: 480
Rep Power: 10 
If you start your FSI simulation directly at 12 kPa without proper initial condtions the solver will fail. Ramping the pressure from 0 to 12 kPa will provide a better initial guess.
An easy CEL expression to ramp the pressure could look like: pressureUp = 80[mmHg/s]*10*t*step((0.1[s]t)/1[s]) which would (with a timestep size of 0.001 [s]) ramp the pressure from 0 to 80 mmHg in 0.1 [s]. 

July 15, 2009, 05:14 

#8 
Member
Join Date: Jun 2009
Posts: 56
Rep Power: 7 
I dont understand...the outlet pressure is not pulsatile in my problem,it is costant 12kpa.how can i ramp it?do you mean to ramp initial condition?
is there any tutorial about ramping the loads?please help me more best regards Last edited by smn; July 15, 2009 at 05:32. 

July 18, 2009, 01:22 

#9 
Member
Join Date: Jun 2009
Posts: 56
Rep Power: 7 
hi lance:
thanks for your helps,i was thinking about your advices for ramping loads last two days,now i shoul tell you that i have hard problems in my thesis and i realy need your more helps... pleaseeeeee tell me the details... do you mean to ramp boundary conditions or initial condition???and how??? 

July 23, 2009, 02:56 

#10 
Member
Join Date: Jun 2009
Posts: 56
Rep Power: 7 
hi:
can anyone help me???i really need your suggestions for fsi modeling of blood vessel.....pleaseeeeeee help me... 

July 28, 2009, 02:15 

#11 
Member
Ali Torbaty
Join Date: Jul 2009
Location: Sydney, Australia
Posts: 71
Rep Power: 7 
I would change the CEL to this:
pressureUp = 12[kpa]*10*(t/1[s])*step((0.1[s]t)/1[s]) + 12[kpa]*step((t0.1[s])/1[s]) if you run the model for a time step of .001s the "pressureUp" value will increase from 0.12 kpa to 12kpa in 0.1 second you should use the "pressureUp" for pressure initialisation and also in your BC 

July 28, 2009, 04:03 

#12  
Member
Join Date: Jun 2009
Posts: 56
Rep Power: 7 
Quote:


July 28, 2009, 04:09 

#13 
Member
Ali Torbaty
Join Date: Jul 2009
Location: Sydney, Australia
Posts: 71
Rep Power: 7 
Actulay, this is just for ramp up in early 0.1 second to keep your model stable, after that it will stay constant at 12kpa.


July 28, 2009, 04:39 

#14  
Member
Join Date: Jun 2009
Posts: 56
Rep Power: 7 
Quote:
now i am solving this problem in a new way :at first i solved the problem for structural steel material,and then used the res file and .db file as initial file for the run of vessel material and this runs perfectly.but unfortunately when i post process the results i see no difference for example for mesh displacement...what do you think?would you please help me??? 

July 28, 2009, 07:17 

#15 
Senior Member
Join Date: Apr 2009
Posts: 503
Rep Power: 11 
The restart procedure for FSI is not obvious, so it's probably still running using steel as the material. The FSI training course for CFX has an example of solving a flexible rubber pipe with a similar youngs modulus and poissons ratio to your case. Tech support may be able to send you this, or better still take the training course. About ramping the pressure  your initial geometry will represent the true geometry at some pressure, let's assume that it's representative of the vessel at 0 rel. pressure. You said you were starting the case with an initial condition pressure of 0 and an outlet pressure of 12 kPa. The inlet pressure will be >12kPa. This is not a consistent set of initial conditions  the structure is not in equilibrium with the fluid pressure! In the first timestep the pressure is going to jump to at least 12 kPa and cause large deformations.


July 28, 2009, 07:25 

#16  
Member
Join Date: Jun 2009
Posts: 56
Rep Power: 7 
Quote:
but i should tell you that i have also tried 12 kpa for initial condition but no difference...how can i get that example?i cant take the course now... best regards 

July 29, 2009, 06:42 

#17 
Senior Member
Join Date: Apr 2009
Posts: 503
Rep Power: 11 
To get the example you could try submitting a support request through the ansys customer portal. What happens if you set your inlet velocity to 0, your initial pressure to 12kPa and your outlet pressure to 12kpa? I expect the vessel will expand  is this physically what should happen? If not, and assuming your fluid is incompressible, then just reduce everything by 12kPa (initial pressure = 0, outlet pressure = 0) so the loads sent to the structure are zero. If the vessel is supposed to expand then you should start with a steadystate fsi simulation using zero initial and outlet pressure, then slowly ramp up the outlet pressure so that the vessel expands gradually to its deformed shape at 12kPa.


March 5, 2012, 20:28 
have prob in FSI

#18 
New Member
abdul khader
Join Date: Dec 2010
Posts: 19
Rep Power: 5 
Dear all,
I am trying to simulate a pulsatile flow across a straight flexible tube using time varying velocity as inlet and time varying pressure at outlet. The total time step is 1sec with time step of 0.005sec. The solution is done with nor errors. But when I see the results, I observe a bending of structure / fluid in x direction after 0.02sec and I can see a pulsatile flow with the wave travelling thrice in 1sec. But the deformation is higher in x direction rather than a radial deformation all along the cycle. When I tried doing steady state analysis, there i observed the load transfer into structure after importing from CFX results is not uniform like. the force transfer is having  value in X direction and + in Y and Z directions. Please help me, I am facing this problem from past 6 months. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Modeling blood flow  FloWorks  mcneelyd  FloEFD, FloWorks & FloTHERM  2  June 15, 2009 12:53 
how to extend FSI 2D codes to 3D, need advises  abouziar  Main CFD Forum  1  May 30, 2008 04:08 
BLOOD FLOW MODELING  Keith  FLUENT  2  January 5, 2006 14:04 
BLOOD FLOW MODELING (need help)  Keith  FLUENT  3  December 21, 2005 05:14 
Urgent..Needs for FSI modeling using ANSYS  Eugene  CFX  7  March 27, 2005 10:19 