[Marten]

Hi everyone,

for my diplom thesis I'm trying to set up a pulsatile blood flow in a vessel including fluid structur interaction. For this I use CFX and ansys under workbench enviroment. I created the vessel in the design modeler and also used the meshing tools included in workbench. The set up is almost the same like in the cfx tutorial with the oscillating plate. But when I come to run the solver I get an error after some timesteps, that the mesh gets folded. I think I have to do a remeshing everytime the mesh quality gets too low. I'm not able to do this with the documentation provided with cfx. can anybody help me with this? I also tried to set the stiffness of the mesh to 1, which seems to be the lowest, but I would rather like to solve the problem with remeshing.
Do I have to remesh the structure and the fluid domain seperatly, 'cause this is how I generated the meshes in the first place?
I'm confused and need help.


kind regards
Marten

[Mehran]

Hi,

Can I ask you what is the type of mesh you are using?

[spatialtime]

You can't do an automatic remesh when using FSI. CFX won't allow you to add a "configuration" sub module.

[hesamking]

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

[Marten]

you can use a "user function" (for example called 'veloprofile') and make a series of time points connecting to the specific velocity. this user function can be used in an expression .in the example type 'veloprofile(time)' . this makes your user function dependent of the simulation time. now use your expression as inlet velocity by selecting inlet velocity normal to boundary or something like that. I would suggest that you use an opening boundary condition at your to outlets and set the difference pressure to 0 Pa. Neumann B.C. simply means that you specify a value for the BC and not a gradient.

many greetings
Marten

[hesamking]

Thanks Marten,
The problem is finding the function to input as UDF. how should i do that? i have already extracted the data points out of the curve I showed in the picture. I have it as CVS file. Any Idea for getting the function?
Best,
Hesam

[rikio]

Hesam, UDF works in Fluent, and CEL in CFX.

You can get this profile function from Excel, for a simply expression, or obtain it from a profesional mathmatical software, like Matlab.

[Marten]

In CFX you can simply use the data points and it will interpolate between these. You can import your data points for example as a .txt-file (each data pair in a line devided by komma, I think) by clicking in the user function area under the unit selection and select 'import data'. in the unit field type for example [s] and below [m s^-1]. This is a very practical tool in CFX. If you want to solve it as a mathematical expression you might need to split the function into several parts (and produce polynomes in Excel for example) and use the step function in CEL. If you use Fluent you need to write a UDF file, which is a bit more complex.

greetings
Marten

[Marten]

This is an example of FLUENT UDF for an unsteady flow with sinus-form

/************************************************** ********************
unsteady.c
UDF for specifying a transient velocity profile boundary condition
************************************************** *********************/



#include "udf.h"

DEFINE_PROFILE(unsteady_velocity, thread, position)
{
face_t f;
real t = CURRENT_TIME;
real coeff;

coeff = 2.*3.14159265357/(60./60.);
begin_f_loop(f, thread)
{
F_PROFILE(f, thread, position) = 0.6 + 0.4*sin(t*coeff);
}
end_f_loop(f, thread)
}

[hesamking]

Dear Marten thank you so much.
Actually as I figured out the best way is to define a periodic function for
your inlet velocity cause the user profile data may not do the interpolation good and end up with some wrong results as the input. Anyhow, I created a simple expression like 1+sin(t) and then for my inlet velocity I took cylinderical coordinated with just axial velocity components and the other 2 one equal to zero.
So for my axial component I took this:
u= (1+sin(t)*(1-r^2)
and my steady state run converges good but my transient one is fluctuating
and after the run is complete I can see any results, for example for pressure on the artery wall.
I hope I could explain it good.
Thanks