CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   How to apply pulsatile velocity in boundary condition? (http://www.cfd-online.com/Forums/fluent/92913-how-apply-pulsatile-velocity-boundary-condition.html)

Sama September 29, 2011 00:34

How to apply pulsatile velocity in boundary condition?
 
Hello. I am simulating aorta with aneurysm ( locally dilated aorta) . for velocity boundary condition I have problem. velocity is pulsatile, it is changing during one cardiac cycle. I know how to apply constant velocity boundary condition, but I am not able to do it for a pulsatile velocity. I would appreciate you if you guide me with this problem.
Sama:o

engin September 29, 2011 04:55

Hi,

For solution to your problem, you could use transient boundary profiles if your boundary conditions are not spattially varying. I think they are not for your case. Check section 7.1.9 of the fluent user guide for more info. If spattially varying BCs are needed, you should use UDFs.

Regards

Sama September 29, 2011 13:00

Thank you very much, dear engin. yes it is not spatially variable,so I can use transient BC.I have to go to manual for precise underestanding of it I just started learning ansys Fluent 2 days ago.:rolleyes:

Behnam Ghadimi October 2, 2011 16:19

Quote:

Originally Posted by engin (Post 326037)
Hi,

For solution to your problem, you could use transient boundary profiles if your boundary conditions are not spattially varying. I think they are not for your case. Check section 7.1.9 of the fluent user guide for more info. If spattially varying BCs are needed, you should use UDFs.

Regards

hi engin
you are write, but i think you can use profile for some spattially varying case. you must insert the location of any node in the global coordinate system and then insert the velocity of that nodes. such as
((P_inlet radial 12)
(r
0 .05 .1 .15 .2 .25 .3 .35 .4 .45 .5 1.5)
(pressure
4340 4280 4060 3720 3100 2780 2370 1890 1410 740 0 0)
)
you insert 12 point velocities in radial direction and fluent interpolate velocities for nodes which lie between this nodes.
or for time changing variable:
((sampleprofile transient 3 0)
(time
1
2
3
)
(u
10
20
30
)
)

engin October 3, 2011 10:05

Dear Benham Ghadimi,

I said if not spatially varying for both spatially varying and time varying BCs as the simulation is transient. Profile file format is not suited for both spatially and time varying BCs. For this kind of BCs, you should use UDFs or periodic BCs.

Behnam Ghadimi October 4, 2011 07:09

Quote:

Originally Posted by engin (Post 326497)
Dear Benham Ghadimi,

I said if not spatially varying for both spatially varying and time varying BCs as the simulation is transient. Profile file format is not suited for both spatially and time varying BCs. For this kind of BCs, you should use UDFs or periodic BCs.

dear engin,
you are write, i misunderstanded your purpose, but i think it's possible to combine time and space variation in profiles, i don't use this but i think it must be possible, if else please tell me.
but as you said UDF is a good way for this purpose.
thanks a lot
Behnam Ghadimi

m2montazari October 5, 2011 15:50

dear sama,
take a look at http://www.cfd-online.com/Forums/flu...nlet-tube.html
it may help.
yours,
mohammad

engin October 7, 2011 07:44

Dear Behnam Ghadimi,

As I said before profile format is not suitable for spatially and time varying BCs. But if the BC is periodic you could use periodic BCs. So it is not possible with profiles if the BCs you are going to use are varying with both time and space (irregularly). Take a look at the FLUENT manual about profiles. There must be a warning about that if I remember correctly.


All times are GMT -4. The time now is 10:23.