|
[Sponsors] |
September 10, 2010, 06:12 |
Closed loop pipe flow
|
#1 |
Senior Member
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 23 |
Hello everybody,
for the first time I am dealing with pipe flow and I need some ideas and suggestions on how to set up my case properly. I have a closed loop cooling system, where air passes through some pipes of different diameters: the smallest one has a diameter of some millimeters, while the largest one is of the order of meters, as shown in the attached picture. Air is moved by a fan placed in the mean diameter section. My main objective is to calculate the pressure drop in the system. Here are my questions:
or are there any other suggestions?These are only of the few questions that are running into my mind... Looking for someone that can shed some light on the subject. Regards, mad |
|
September 10, 2010, 12:37 |
|
#2 |
Senior Member
Nilesh Rane
Join Date: Apr 2010
Posts: 122
Rep Power: 16 |
Hi maddalena,
i am not sure whether one should use wall functions with low Re models or not. But one can definitely negotiate the use of very fine mesh using wall function. But doesn't it sound more logical to use high Re model then in conjunction with wall function rather than using low-Re model?? Please correct me if i am wrong. And one more thing. Can you please tell me where we should specify the wall function like nutLowReWallFunction if i have to use it??? One more thing: i think k and eps BC should alwayz be this k=eps=0. And i suppose the wallfunctions internally make sure this condition is followed and the value u specify is actually value at the edge of say log layer. Is it correct or not??
__________________
Imagination is more important than knowledge..
|
|
September 11, 2010, 15:29 |
|
#3 | |
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,912
Rep Power: 36 |
Quote:
Your last statement about the necessity of having k=eps=0 at all BC's is not correct, since in models relying on Boussinesq approximation it would lead to an undefined turbulent viscosity. Best,
__________________
Alberto Passalacqua GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM - An open-source implementation of quadrature-based moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. |
||
September 11, 2010, 15:38 |
|
#4 | ||
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,912
Rep Power: 36 |
Quote:
In the small pipe probably the flow laminarizes. In theory a low-Re k-eps model that preserves the correct behaviour in laminar cases (double check the literature, you will easily find the values of the coefficients to obtain this in L-S model) could work. Quote:
The rest seems fine. Numerical schemes are standard, the initial condition does not matter if you want a steady state solution. Best,
__________________
Alberto Passalacqua GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM - An open-source implementation of quadrature-based moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. |
|||
September 11, 2010, 16:02 |
|
#5 |
Senior Member
Nilesh Rane
Join Date: Apr 2010
Posts: 122
Rep Power: 16 |
Hello Alberto,
I apologize for the untidiness. I was actually trying to answer the questions of maddalena. Just telling my thoughts. I thought may be i can correct my knowledge through some discussion. Thats it...Otherwise i do open my own threads separately for my issues.. Sorry again..
__________________
Imagination is more important than knowledge..
|
|
September 11, 2010, 19:41 |
|
#6 |
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,912
Rep Power: 36 |
Not a prob. Just trying to spread good practices ;-)
For example, too often very old threads (not this case) are bumped to ask questions, while a new thread would help to keep things cleaner. Repetitions are not avoided anyway on a forum.
__________________
Alberto Passalacqua GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM - An open-source implementation of quadrature-based moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. |
|
September 13, 2010, 04:00 |
|
#7 | ||||
Senior Member
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 23 |
Hi Alberto,
and thanks for your quick and useful answer (as usual). You are one of the few expert member that helps the younger to address their question and gain their experience in this forum, and I really appreciated that. Now the questions... Quote:
Quote:
Quote:
Quote:
Thanks one more time for your help. cheers, mad Last edited by maddalena; September 13, 2010 at 07:04. Reason: typo |
|||||
September 13, 2010, 04:06 |
|
#8 | |
Senior Member
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 23 |
Hello,
Quote:
Enjoy mad |
||
September 13, 2010, 11:45 |
|
#9 | ||||
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,912
Rep Power: 36 |
Quote:
Quote:
Quote:
Quote:
Best,
__________________
Alberto Passalacqua GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM - An open-source implementation of quadrature-based moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. |
|||||
September 13, 2010, 12:03 |
|
#10 |
Senior Member
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 23 |
Ok, summarizing:
Cheers, mad |
|
September 13, 2010, 17:14 |
|
#11 | ||||
Senior Member
Nilesh Rane
Join Date: Apr 2010
Posts: 122
Rep Power: 16 |
Quote:
Yeah...I had looked into the source code and got that thing right after i posted here. Quote:
Quote:
Quote:
k = 0.002U^2 eps = 0.1 (Cmu x rho x k^2)/ mu...........(Cmu = 0.09) Hope it helps, Nilesh..
__________________
Imagination is more important than knowledge..
|
|||||
September 13, 2010, 17:22 |
|
#12 | |
Senior Member
Nilesh Rane
Join Date: Apr 2010
Posts: 122
Rep Power: 16 |
Quote:
__________________
Imagination is more important than knowledge..
|
||
September 13, 2010, 17:50 |
|
#13 | |
Senior Member
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 23 |
Hello,
Quote:
The junction is the real problem. I though I could extrude the pipe mesh for a while, in normal direction, but the mesh quality is not good. Do you have any suggestions on this point? Thank you! mad Last edited by maddalena; September 14, 2010 at 05:36. |
||
September 13, 2010, 18:21 |
|
#14 | |
Senior Member
Nilesh Rane
Join Date: Apr 2010
Posts: 122
Rep Power: 16 |
Quote:
May not be relevant to your software, but just in case this is the reason: If you mesh the domain with tet volume mesh and then extrude the surface mesh for prism layer, then in that case keep tet cells coarse at walls as compared to the core area. then extrude the surface layer. And try keeping least possible prism layers. This is what i would have done. just my opinion. I am no expert of this, but I hope it solves your problem. Nilesh
__________________
Imagination is more important than knowledge..
|
||
September 14, 2010, 01:59 |
|
#15 | |
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,912
Rep Power: 36 |
Quote:
Best,
__________________
Alberto Passalacqua GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM - An open-source implementation of quadrature-based moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. |
||
September 14, 2010, 03:34 |
|
#16 | ||
Senior Member
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 23 |
Good morning!
Quote:
Quote:
Thanks to both of you! mad |
|||
September 14, 2010, 06:18 |
|
#17 |
Senior Member
Nilesh Rane
Join Date: Apr 2010
Posts: 122
Rep Power: 16 |
In Gambit, one can define the surface mesh on junction face, with boundary layer on it. Can you do that in your software?? What i do in such case is, when i can, i define a good quality surface mesh on the junction interface. Then the volume mesh is generated based on this surface mesh and thus i have good quality nice mesh around that interface. This basically puts the constraint on the volume mesh. You can give good quality evenly based mesh on the face. I dont think it would be impossibly difficult to get good quality mesh on your geometry.
I think Alberto also want to say something like this. Edit: Just googled a bit on pointwise. If its similar to gridgen, then i am sure there must be a way to define low level constraints (meaning surface or line mesh) on the volume mesh. I have used gridgen for sometime for simple geometry, but i know it has the capability. i am expecting pointwise must also be having the same. Nilesh...
__________________
Imagination is more important than knowledge..
|
|
September 14, 2010, 06:46 |
|
#18 | ||
Senior Member
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 23 |
Hello.
Quote:
Quote:
Maybe the only thing I need is to refine the mesh... Regards mad |
|||
September 14, 2010, 10:52 |
|
#19 |
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,912
Rep Power: 36 |
Yes. You might want to try to add the layer surrounding the trapezoidal section. Just be careful that cell size changes very smoothly, or it might end up giving you worse results than an automatically generated tet mesh.
__________________
Alberto Passalacqua GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM - An open-source implementation of quadrature-based moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. |
|
September 14, 2010, 19:59 |
|
#20 |
Senior Member
Nilesh Rane
Join Date: Apr 2010
Posts: 122
Rep Power: 16 |
Hi,
I meant meshing the whole face where the two pipes meet, boundary layer as well as central part of the face. And the more constraints you specify the better mesh you get.
__________________
Imagination is more important than knowledge..
|
|
Tags |
fan, flowrateinletvelocity, low-re, pipe, simplefoam |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
flow in perforated pipe distributor | pertupd | ANSYS | 0 | August 12, 2009 09:36 |
NACA0012 geometry/design software needed | Franny | Main CFD Forum | 13 | July 7, 2007 16:57 |
Flow in a Closed Loop | John Collins | Main CFD Forum | 2 | February 27, 2003 11:26 |
Terrible Mistake In Fluid Dynamics History | Abhi | Main CFD Forum | 12 | July 8, 2002 10:11 |
Pulsatile blood flow in closed loops | Michael F. Wolf | Main CFD Forum | 3 | July 1, 1999 17:37 |