|
[Sponsors] |
June 15, 2010, 10:28 |
Blood flow with FSI in Ansys 12
|
#1 |
New Member
Marten
Join Date: Jun 2010
Posts: 7
Rep Power: 16 |
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 Last edited by Marten; June 15, 2010 at 10:49. |
|
July 25, 2010, 08:57 |
mesh type
|
#2 |
New Member
Mehran Saeedi
Join Date: Jan 2010
Posts: 8
Rep Power: 16 |
Hi,
Can I ask you what is the type of mesh you are using? |
|
July 27, 2010, 05:25 |
|
#3 |
New Member
Join Date: Apr 2009
Posts: 12
Rep Power: 17 |
You can't do an automatic remesh when using FSI. CFX won't allow you to add a "configuration" sub module.
|
|
March 23, 2012, 12:58 |
help to set the inflow BC in CFX
|
#4 |
Member
Hesam Moghaddam
Join Date: Mar 2012
Posts: 49
Rep Power: 14 |
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 |
|
March 23, 2012, 14:13 |
|
#5 |
New Member
Marten
Join Date: Jun 2010
Posts: 7
Rep Power: 16 |
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 |
|
March 23, 2012, 14:31 |
|
#6 |
Member
Hesam Moghaddam
Join Date: Mar 2012
Posts: 49
Rep Power: 14 |
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 |
|
March 23, 2012, 17:19 |
|
#7 |
Senior Member
|
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. |
|
March 24, 2012, 06:52 |
|
#8 |
New Member
Marten
Join Date: Jun 2010
Posts: 7
Rep Power: 16 |
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 |
|
March 24, 2012, 07:02 |
|
#9 |
New Member
Marten
Join Date: Jun 2010
Posts: 7
Rep Power: 16 |
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) } |
|
April 14, 2012, 16:33 |
|
#10 |
Member
Hesam Moghaddam
Join Date: Mar 2012
Posts: 49
Rep Power: 14 |
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 |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Pulsatile blood flow | Duncan | FLUENT | 12 | October 26, 2016 09:23 |
fsi model of water flow in a pipe | alinik | CFX | 11 | November 5, 2009 11:29 |
ccl for fsi modeling of blood vessel | smn | CFX | 0 | July 19, 2009 05:36 |
Modeling blood flow - FloWorks | mcneelyd | FloEFD, FloWorks & FloTHERM | 2 | June 15, 2009 12:53 |
modelling blood flow in arteries with starcd | sara | Siemens | 5 | April 10, 2007 09:17 |