
[Sponsors] 
February 27, 2012, 11:26 
Flow through material..

#1 
New Member
Hermen
Join Date: Feb 2012
Posts: 5
Rep Power: 7 
Sponsored Links
As I try to find the best program for CFD analysis , the following question rised: Is it possible to simulate an airflow that goes through a pile of stuff? eg onions or carrots? If yes, can this be done with 'all' regular CFD programs? Any input would be appreciated 

Sponsored Links 
February 27, 2012, 17:06 

#2 
Senior Member
Andrew
Join Date: Mar 2009
Location: Washington, DC
Posts: 195
Rep Power: 10 
yes, this would be flow thru porous media. Fluent will do it.


February 28, 2012, 04:20 

#3 
New Member
Hermen
Join Date: Feb 2012
Posts: 5
Rep Power: 7 
Thank you for your reaction and for posting that term.
I scanned this forum and google a bit, and it seems to me that this type of simulation is pretty advanced stuff. Could someone, with no experience in FEM, after following an Ansys course in CFD, generate reliable results within a timeline of 0,5 years? By this I also take into account that there are no colleageus that know simulation CFD`s/ FEM. Thanks, 

February 28, 2012, 08:55 

#4 
Senior Member
Andrew
Join Date: Mar 2009
Location: Washington, DC
Posts: 195
Rep Power: 10 
it's not too tough. There will be a few variables that you will need to obtain experimentally, but you might be able to find them in literature from someone that has done a similar experiment.


February 28, 2012, 11:48 

#5 
Senior Member
Martin Hegedus
Join Date: Feb 2011
Posts: 480
Rep Power: 12 
I think this sounds like a hard problem!
This sounds like you have a pile of stuff on the ground and you would like to calculate the amount of air/liquid going over it and through it. The pile could be onions, carrots, rocks, tires, etc. I don't know of a turbulence model that has been validated for this. Of course a lot depends on how accurate you want the results to be. Your solution is probably unsteady so expect to devote a lot of resources to it. Also, I believe, wall functions do not apply here so you'll need to capture the entire boundary layer on your objects. In which case, the solution could take a lot of grid points and griding boundary layer could get a little tricky if you have a lot of touching elements. On the other hand, if you would like to model something with darcy's law, that is easier. You'll probably need to determine the resistence experimentally or find it in the literature. Darcy's law can be used if flow can only go through the objects, and not over it. However, it will not give you the details of the flow going through the media. It gives you the head loss. Also, the velocity profile in front and behind the porous media will be incorrect to some degree, especially if there is some sort of recirculation region in front or behind. 

February 28, 2012, 11:51 

#6 
Senior Member
Martin Hegedus
Join Date: Feb 2011
Posts: 480
Rep Power: 12 

February 28, 2012, 11:59 

#7 
Senior Member
Andrew
Join Date: Mar 2009
Location: Washington, DC
Posts: 195
Rep Power: 10 
that is all flow thru porous media..packed bed..whatever you want to call it..it is all the same thing just with different values for the variables. It is easy to do, and Fluent does a great job of it. There is no need at all for the wall functions and a giant grid. You will model it in Fluent as porous media and set the BCs..it is very straight forward. You care going to have to get some constant from either your own lab work or published data.
Darcy and Forchheimer 

February 28, 2012, 12:22 

#8 
Senior Member
Martin Hegedus
Join Date: Feb 2011
Posts: 480
Rep Power: 12 
I'm not a fluent user so I don't know the ins and outs of it.
Usually to use Darcy's law there has to be a coupling of two grid points so the delta velocity can be found. So this works well for things like a blockage in a pipe or something thin like a filter. But, for this case, I literally have an image of a pile of food on the ground and the original poster wants knowledge of the airflow within (i.e. through) the pile. I didn't think Darcy's law could be used for this. But, maybe the description by the original poster has left me with a bad visual. 

February 28, 2012, 12:54 

#9 
Senior Member
Andrew
Join Date: Mar 2009
Location: Washington, DC
Posts: 195
Rep Power: 10 
its porous media. You will have plugflow..basically a square velocity profile. Unless, the OP is trying to simulate wind flow thru a pile of bananas that is out on a windy street. I guess the OP needs to more descriptive. I am picturing a pipe full of bananas, thus my porous media analogy which Darcy is applicable.


February 28, 2012, 13:09 

#10  
Senior Member
Martin Hegedus
Join Date: Feb 2011
Posts: 480
Rep Power: 12 
Quote:
I really do wish posters would show sketches with some of these questions. 

February 28, 2012, 13:28 

#11 
Senior Member
Martin Hegedus
Join Date: Feb 2011
Posts: 480
Rep Power: 12 
BTW, to the original poster, is this some sort of industrial food processor?


February 28, 2012, 13:34 

#12 
New Member
Hermen
Join Date: Feb 2012
Posts: 5
Rep Power: 7 
thanks for sharing your thoughts all.
Sorry for the fact that my OP wasn`t as clear as it should be. Let me try to explain. There are two situations that my company is going to face: 1) A storage cel (closed environment) with bulk vegetables, thru which air flows. This air flow is generated by an aircooler (bigger than the one in your cars). see here: http://www.onionspotatoes.com/stora...metalducts.php 2) A storage cel (closed environment) with boxes, filled with vegetables, thru which air flows. see here: http://www.onionspotatoes.com/stora...spressure.php hope this brightens things a little will these cases be erliable when simulated, or do I have to use constant valeus that I will get from practical tests? thanks, (will look into dardy`s law now and get back to you) EDIT: I look at it as a flow thru a PCB. exept that has no porous material in it. 

February 28, 2012, 14:00 

#13 
Senior Member
Martin Hegedus
Join Date: Feb 2011
Posts: 480
Rep Power: 12 
Yes, IMO, the tool you have to work with is Darcy's law. http://en.wikipedia.org/wiki/Darcy%27s_law
I think the boxes is doable since it seems similar to flow through a pipe with restriction. However, the pile of potatoes/onions, I'm just not sure. IMO, that would take some creative and iffy simulation. Probably an advanced subject. You'll probably need to use tests to get your constants and to check your model. 

February 29, 2012, 04:26 

#14 
New Member
Hermen
Join Date: Feb 2012
Posts: 5
Rep Power: 7 
Thanks,
Im still not so sure about darcys law. The Re number of 1 or sometimes max 10 makes me doubt a bit. (or Re 2000, For now I had like really non darcian numbers) Ill check again later. Anyway, when looking at this pic: when assuming the boxes are empty, what simulation package would be able to simulate the airflow in that room? And which one of these is the most easy to use/ straightforward program? Thanks already, Hermen 

February 29, 2012, 10:16 

#15 
Senior Member
Andrew
Join Date: Mar 2009
Location: Washington, DC
Posts: 195
Rep Power: 10 
I would still use the porous media model. You need to measure a few things to get the variables needed, but that is really it. You should really read up on porous media flow, and I think you'll have a better understanding of your problem. There are a lot of journal articles written that will help you out (sciencedirect.com) The variables that you measure will change depending on the what you have in the boxes (which will change the porosity and the pressure drop of the problem)


February 29, 2012, 13:44 

#16 
Senior Member
Martin Hegedus
Join Date: Feb 2011
Posts: 480
Rep Power: 12 
Darcy's law is the linear part and Forchheimer's term is the nonlinear term (term multiplied by q^2). The nonlinear term is equivalent to a cp (coefficient of pressure) drop. cp=deltaP/(0.5*rho*q^2). The cp term is sort of inline with Cd (coefficient of drag). This is valid for higher Reynolds numbers and tends to be insensitive to Reynolds number and velocity. Well, at least until there is a change in the type of physics driving the problem.
For example, the boxes filled with carets might be Darcy's law. You'll need to do some experiments to find out. Now, lets say the boxes are empty. At the bottom of the boxes are probably some sort of porous base. Maybe a lattice of wire or wood, or a screen. The nonlinear model (i.e. cp loss) may be more applicable. Of course, the pressure loss through the lattice may be a lot less then the loss through the carets so the carets are more important to the analysis. I'm just trying to come up with an example. Most big name CFD packages should be able to handle this, but it depends on what flow quantities you are interested in. If you are looking for a precise flow value somewhere, I doubt any of them can. If you are looking for fuzzy numbers, then the next step is to identify the physics you are interested in and check with the vendor to see how their code handles the physics. BTW, fuzzy numbers are OK. They might help you identify areas which impact your process the most. Also, the relationship between you and the provider, especially if no one around you uses CFD, will be an important one. For example, last week I asked a question of Mentor Graphics about their FloVENT code. The sales person said they would pass the question on to a product specialist and I have not heard back yet. I don't use their code, it was just a question. Obviously, I'm not happy about this. Some of the things for you to think about in regards to the physics: 1) Is buoyancy important. (i.e. does the temperature affect your flow through the room) If one uses the incompressible equations, the energy equation is uncoupled from the conservation of mass and momentum. I would think that your model does not need to be concerned about this, but I could be wrong. 2) Are moving parts important? In other words, can you neglect the dynamics of the no return valve. If the dynamics are important, the simulation will be much harder and resource consuming. I'm assuming you can neglect it, in other words keep the "no return" valve open. 3) How do you plan to model the pressure jump through the turbine? Hopefully the manufacturer gives you a number which can be easily plugged into the CFD model. Another product of the turbine is turbulence. Hopefully you'll be able to ignore this. 4) Modeling the U turn in the pressure chamber will be hard to get right. And this may be very important. In general, I would think that the flow in the pressure chamber is very important. If there is a recirculation region inside, air just might not get in the ducts. 5) Modeling the pressure loss of the flow entering the ducts which go along the bottom of boxes may also be challenging due to the flow separation at the inlet. Hopefully the errors in modeling the pressure loss/blockage will be small relative to all the other pressure losses. 6) I have no idea how to model the flow around/through the condenser since it just seems to be hanging there. Is flow through the condenser important or can you just model it as flow blockage? 7) If you are using the incompressible equations, the velocity and pressure will be independent of the temperature. Keep that in mind when modeling the heat source. 8) Also, your overall true structure is not clean. In other words there are beams and support structure everywhere. You'll probably be, in general, ignoring it. However, in critical areas, the pressure chamber, you might want to model it. In the old days, flow was determined by resistance values. Much like an electrical circuit. So maybe thinking of things in these terms might help you determine what is, and is not, important. BTW, CFD is a wonderful tool for helping to get a handle on some of these resistance values. In other words, sometimes you don't need to model the overall system, just parts of it. Another example, to gain info on the pressure chamber, you could use Darcy's law to add resistance at the entrance to the ducts and just ignore everything else. Sorry, I don't have an explicit recommendation of a code. Good Luck! 

March 1, 2012, 05:06 

#17 
New Member
Hermen
Join Date: Feb 2012
Posts: 5
Rep Power: 7 
Thanks Andrew, Martin,
Im am aware of the fact that concessions, simplifications, dividing the system are the first steps in starting a simulation. The both of you have given me a good idea of what is waiting. Im convinced that CFD will be of great help for us. Espacially the fact that simulations will show bottlenecks in the system that, when only using tests, will be left unseen. Thanks for the imput, Ill probably get a demo of one of the bigger flow simulators (Im thinking of Ansys, CFdesign  Autodesk Simulation) And maybe when time comes ill post a nice flow through media analysis Last edited by Hermen; March 1, 2012 at 06:05. 

March 2, 2012, 15:21 

#18 
Senior Member
Martin Hegedus
Join Date: Feb 2011
Posts: 480
Rep Power: 12 
Sorry, I may have misled you to some degree about buoyancy. And, I've changed my opinion of Mentor Graphics and wish I had the opportunity to test their codes. Of course I reserve the right to change my opinion on anything at any time.
This link may be helpful to you. A quote from their (www.mentor.com) web page to describe FloVENT "FloVENT’s fast and easytouse menu system is designed specifically for engineers involved in the design and optimization of heating, ventilating and air conditioning (HVAC) systems." Just to give you an idea of what is being discussed. http://www.cfdonline.com/Forums/flo...question.html If you do end up contacting Robin/Mentor Graphics at some point, please consider mentioning that you got some information from cfdonline. 

June 4, 2012, 03:37 

#19 
New Member
Seroleh Osman
Join Date: Jun 2012
Posts: 3
Rep Power: 7 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Compressible flow, no data at the outlet  mireis  FLUENT  6  September 3, 2015 02:10 
Constant velocity of the material  Sas  CFX  15  July 13, 2010 08:56 
Mass flow and UMom flow in CFX  Zhihua Xie  CFX  0  September 3, 2007 09:49 
transform navierstokes eq. to eulereq.  pxyz  Main CFD Forum  37  July 7, 2006 08:42 
Plug Flow  Franck  Main CFD Forum  3  September 4, 2003 05:57 
Sponsored Links 