Need help in FSI CFX+WORKBENCH
Greetings,
I am trying to simulate a FSI for simple straight elastic tube with time varying velocity at inlet and time varying pressure at outlet. The BC include solving pulsatile flow for 0.8sec (each cycle), with time varying velocity at inlet and pressure at outlet. I have defined .csv file in MS excel from which we can import into CFX for defining BC. The solution is done properly with no errors, but in results, i see a unusual deformation in the structure. Instead of uniform radial deformation, i see a the structure bends more in X direction . Do we have to perform any static analysis also, I tried doing that, but when the pressure is imported into structure interface, the forces are having  value in X direction and rest other directions have + values. Can this be one of the reasons for this unusual behavior. 
In general if the elastic tube is in tension (positive force are passed) then I would expect radial deformations to uniform (or close to uniform). If you are passing negative forces, then that would cause compression of the tube  I would not expect that to be uniform (try squashing an elastic tube, you don't get uniform deformation).

3 Attachment(s)
thanks for your reply stumpy.
I have attached some images of structural deformation. I hope this will give you an idea how the deformation is going on. It is related to blood flow through arteries. I validated bench mark problem wit available literature(Inlet pres and zero traction at outlet). When I use time varying vel and pres at inlet and outlet respectively, i am observing this kind of deformation. I tried using expression as well as csv file. Both has same effect. Kindly suggest what can be the reason for this kind of deformation and how to tackle it. 
Dear Stumpy,
May I know if you were able to find out the solution for this problem. Regards, Abdul 
It looks like the tube is in tension. If you run a Mechanical simulation (no FSI) and apply a constant Pressure do you get uniform raidal deformation? If so, then look at the Pressure field in CFX  is it constant for a given axial location? If not, then you should not expect constant radial deformation. Have you applied gravity in either Mechanical or CFX, that would cause the tube to sag?
Note that just because your boundary conditions are symmetric this does not mean your solution will be. If the pipe is very flexible then it may well bend to one side or another. If you want perfectly uniform radial deformation then model a small segment of the tube and apply symmetry boundary conditions. 
5 Attachment(s)
Dear stummpy,
you are right. I too feel same thing. I did a static analysis and transfer cfd load from fluid to inner wall of sturcture. if i use steel as mat, i get perfect uniform radial expansion, but when i do same thgn for artery material prop, it slightly bends like wat we saw before. I hv attached snap of load transfer, and deformation of steel and artery as mat. I also tried doing only structure static analysis wit ends fixed and external pressure on inner wall, in that case also, there is uniform radial deformation for steel as well as artery as material. But when i transfer load from CFX with artery as material, there is slight bending but no such behavior for steel as material. I have attached some snaps please have a look. also, when i do the same thing for concentric stenosis in same model, there is heavy negative pressure at stenosis and fsi cannt proceed further as elements are distorted. please suggest how to overcome this problem. 
Negative pressures on flexible tubes are not good  they will cause the tube to collapse. In the real world do you expect negative pressures? If you are using zero pressure boundary conditions then consider setting these to be the real blood pressure.

help to set the inflow BC in CFX
1 Attachment(s)
i am doing a research on an aneurysm, I want to redo an
already done work to learn details of this work. I don't know how I should set up the inlet velocity. I have the inlet velocity waveform graph from the paper, but I do not have any expression or equation which i can input into CFX. will you please guide me what I should do? I am doing my study for an aneurysm at a bifurcation of a basilar artery. I have one inlet and two outlets? I also wanted to ask what B.C i should use for the outlet. In paper, I think it mentions Newmann B.C. I have attached the picture of inflow waveform. I would really appreciate your kind help. Regards, Heasam 
Dear Stumpy,
Thanks for your reply. I have one more clarification with regard to iterations of cfx and stagger iterations, for a total time of 0.8sec, I have used 100 time steps. I have used min 2 and max 6 as CFX iterations with high resolution and second order eq. I have also used min2 and max4 stagger iterations with 0.2 as relaxation factor for displacement and force. May I know is it sufficient for proper FSI simulation or is there any thumb rule for selecting these values..? As far as stenosis is concerned, I haved used turbulent condition with K epsilion model with medium intensity. I have used carying vel & pressure @ inlet and outlet respectively. I have used ref press as 1 atms and I havn't used 0Pres anywhere. CFD analysis shows negative pres @ constriction, similar to pressure behavior in venturimeter. BUt when same pressure is transfered @ interface of structure, it cannt handle negative press. Also, is there any need of changing ref press. Bcoz @ oulet, i have applied pulse pressure of (040mmHg). Can you please share some thought on ref pressure, if it can solve the prob. 
Quote:
You can fit a curve of vel v/s time in excel and use as .csv file to import into CFX. Ref edr bloggs for this. You will get more information how to import.csv file. as far as womersely, condition, I havnt tried this in my BC, but you can go through previous replies in CFX forum. @ outlet you can use either constant pressure or time varying pressure(pulse pressure= 40mmHg). You can ref Ryo Torri et. al. literature. 
No, that's not sufficient. 4 stagger loops with an underrelaxation factor of 0.2 isn't enough for convergence. Try working through the math.... with a load change from 0 to 1, with an underrelaxation factor of 0.2, how many stagger loops does it take to reach say 0.99?
0.2, 0.36, 0.488, 0.5904, ...... etc 
dear stumpy,
I tried with several combinations of stagger iterations, starting from max of 2, 3 upto 8. but i didnt observed any difference in the results and its the same, like the deformation , velocity and pressure values also i had kept relaxation factor upto 0.5, but if i use relaxation factor of 1 or 0.9 the solution gets an error in b/w the solution. Can you kindly brief about selecting the stagger iterations. 
1 Attachment(s)
Could you post the output from the Ansys Interface Loads e.g. for the last 45 timesteps (otherwise it would be a very edgy, see attachment)?
Do you reach Interface convergence when using the mentioned number of stagger iter?? What´s the ratio between solid and fluid density, is the fluid way more viscous than water? neewbie 
1 Attachment(s)
Dear neewbie,
Kindly find the ansys output file attached. density of fluid is 1050Kg/m3 and solid is 1150 kg/m3. the viscoity of fluid is 0.004Pas. But I have also seen a warning as follows: *** WARNING *** SUPPRESSED MESSAGE CP = 12134.516 TIME= 00:06:01 The maximum number of stagger iterations has been reached for multifield solver but the interface quantities have not yet converged. The analysis will proceeds to the next time step. Increase number of stagger iterations using the MFITER command for converged interface solution. *** WARNING *** SUPPRESSED MESSAGE CP = 12191.625 TIME= 00:07:40 The maximum number of stagger iterations has been reached for multifield solver but the interface quantities have not yet converged. The analysis will proceeds to the next time step. Increase number of stagger iterations using the MFITER command for converged interface solution. But in the output file, I dont find any such error and solutions is obtained without any problem. 
Like i said. You did not reach convergence for the interface.Please post the interface convergence. Have a look at the attachment post #13.
So the densityration is almost 1 and the viscosity is moderate. Did you achieve massconvergence? If not this could point towards artificaladdedmasseffect. 
4 Attachment(s)
Dear Neewbie,
I have attached all the monitor of solution. Kindly suggest if its correct or not. The total time is 0.8sec and time step is 0.01 sec. I didnt get how to check mass convergence. Is it checking with RMS P mass or Max P mass..? 
Reduce the Time step and set the stagger iteration to smth. like 30. The amount of stagger iterations is dependent on timestep and physics. So you will only know afterwards but you'll have to give it a try. The residual for interface conv. must cross 0 to achieve convergence. As lower as the relaxation is the slower convergence is achieved but also the system is more stable.

you mean to say, that keep relaxation factor someting around 0.20.5 and keep trying with stagger iterations of around 2030 and check how it behaves.?
may i know how to look for mass convergence, is max p mass/rms p mass correct for looking mass convergence and how to judge for onvergence...? 
Quote:
dear stummpy and neewbie, I understood the concept of underrelaxation factor and no. of stagger iterations. I am trying that, once I am done wit my results I shall get back to you. Thanks stummpy, I saw your replies for previous posts on relaxation factor and stagger iterations. Also, stummpy, can you suggest is taking min of 2 and max of 6 iterations for each time step cfx analysis fine and is there any thumb rule for fixing no. of timesteps for total time. In my case as i said before, total time is 0.8sec and timestep is 0.01sec. Is there any relation or thumb rule to fix up the no. of timesteps and no. of iterations for each timestep in CFX..? Also can you suggest the solution for overcoming negative pressure prob ..? 
Dear stumpy and Newbee,
May I know if there is any relation ship between time steps and stagger iteration to be used. I am trying to find it since long time and with variety of problems worked out, I am still unable to find some logic behind that. Please reply with bit more detailed explanation on this 
All times are GMT 4. The time now is 01:30. 