CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM (http://www.cfd-online.com/Forums/openfoam/)
-   -   How to define outlet convective BC for the cyclic BC (http://www.cfd-online.com/Forums/openfoam/103362-how-define-outlet-convective-bc-cyclic-bc.html)

zxj160 June 18, 2012 11:30

How to define outlet convective BC for the cyclic BC
 
I define the inlet and outlet as cyclic BC. But now I want to set the outlet as convective BC for the passive scalar. Is it possible to achieve that?

zxj160 July 11, 2012 09:45

Or how to define other types of BC for cyclic patches? such as zeroGradient?

Does any one have the experience of creating this kind of customer cyclic derived BC?

chegdan July 11, 2012 10:19

Quote:

Originally Posted by zxj160 (Post 370831)
Or how to define other types of BC for cyclic patches? such as zeroGradient?

Does any one have the experience of creating this kind of customer cyclic derived BC?

The way I got around this easily was to use directMapped for momentum (setting it to an average velocity or flowrate) and that allows you to use fixed and zeroGradient boundary conditions for your passive scalar.

Dan

zxj160 July 11, 2012 10:35

Quote:

Originally Posted by chegdan (Post 370843)
The way I got around this easily was to use directMapped for momentum (setting it to an average velocity or flowrate) and that allows you to use fixed and zeroGradient boundary conditions for your passive scalar.

Dan

Dear Dan,

Thanks. Do you mean that I set inlet and outlet as normal 'patch' type and use directMapped to map the cyclic velocity? Then I can set uniform value and zeroGradient for passive scalar?

If yes, I have tried this and also mapped pressure. But the output of pressure is so different (all the other conditions are same)?

for cyclic case:
p
(
0.000572052
0.000389558
6.02371e-05
-0.000262527
-0.000663079
-0.00121091
-0.00193648
-0.00261434
.......

for directMapped case:
p
(
126.072
126.067
126.061
126.055
126.052
126.049
.......

I can not identify the problem.

chegdan July 11, 2012 11:02

Quote:

Originally Posted by zxj160 (Post 370849)
Dear Dan,

Thanks. Do you mean that I set inlet and outlet as normal 'patch' type and use directMapped to map the cyclic velocity? Then I can set uniform value and zeroGradient for passive scalar?

If yes, I have tried this and also mapped pressure. But the output of pressure is so different (all the other conditions are same)?

for cyclic case:
p
(
0.000572052
0.000389558
6.02371e-05
-0.000262527
-0.000663079
-0.00121091
-0.00193648
-0.00261434
.......

for directMapped case:
p
(
126.072
126.067
126.061
126.055
126.052
126.049
.......

I can not identify the problem.

Is your pressure drop through the domain the same? I always never use directMapped for pressure. The values will be different than the cyclic case since its pressure driven in the directMapped case.

zxj160 July 11, 2012 11:12

Quote:

Originally Posted by chegdan (Post 370858)
Is your pressure drop through the domain the same? I always never use directMapped for pressure. The values will be different than the cyclic case since its pressure driven in the directMapped case.

Yes, the pressure drop is same and only the BCs for pressure are different. But the pressure is also cyclic. If we do not use cyclic, then what type of BC can we define for pressure.

Best regards,
Jian

chegdan July 11, 2012 11:20

Quote:

Originally Posted by zxj160 (Post 370861)
Yes, the pressure drop is same and only the BCs for pressure are different. But the pressure is also cyclic. If we do not use cyclic, then what type of BC can we define for pressure.

Best regards,
Jian

0 on the outlet and zeroGradient on the inlet.

See tutorials/incompressible/pisoFoam/les/pitzDailyDirectMapped for inspiration

zxj160 July 11, 2012 11:29

Quote:

Originally Posted by chegdan (Post 370863)
0 on the outlet and zeroGradient on the inlet.

See tutorials/incompressible/pisoFoam/les/pitzDailyDirectMapped for inspiration

Many thanks. I will try it later. By the way, is there any tutorials introducing pressure (p) in the OpenFOAM? Because I cannot understand the meaning of pressure clearly?

april0100 July 21, 2012 16:27

Pressure is typically normalized by density in OpenFOAM, hence the units [m^2/s^2].

cfdonline2mohsen October 9, 2012 11:28

This is true only for incompressible flow, but for the compressible flow the dimension of pressure is
dimensions [1 -1 -2 0 0 0 0];
check the 0 folder of incompressible & compressible cases in Tutorial


All times are GMT -4. The time now is 23:44.