FSI modeling of blood vessel???
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:( 
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! 
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 
Ramp the pressure inside the entire domain from 0 to 12 kPa before starting the velocity waveform.

I dont understand...what do you mean?how can i ramp the outlet b.c.?what about the initial pressure and inlet b.c.?

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 
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]. 
:(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 
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??? 
hi:
can anyone help me???i really need your suggestions for fsi modeling of blood vessel.....pleaseeeeeee help me... 
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 
Quote:

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.

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??? 
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.

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 
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.

have prob in FSI
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. 
Quote:
I need to implement this for my problem. you have mentioned that a steadystate FSI needs to be run by slowly ramping the outlet pressure to 12 kPa. Do you mean that a static structural analysis be coupled with a transient CFX analysis? because to rampup the pressure in CFX the CFX analysis needs to be transient right? Please confirm. 
All times are GMT 4. The time now is 09:55. 