CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > FloEFD, FloWorks & FloTHERM

Empty object Meshing and Fan boundary condition

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree2Likes
  • 1 Post By Boris_M
  • 1 Post By Boris_M

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   January 29, 2020, 11:50
Exclamation Empty object Meshing and Fan boundary condition
  #1
New Member
 
Join Date: Oct 2018
Posts: 22
Rep Power: 3
cfd_user_pune is on a distinguished road
Hi all,

I am new to FloEFD trying to solve refrigeration problem to calculate pressure drop of my system on air side (and not modeling refrigerant side flow) and heat leak into system through insulating wall. I am not considering evaporator/condenser and fan in model. I do have a fan curve which is used to find an operating point (intersecting point of fan curve and system Impedence curve (calculated from CFD simulation) )

You can imagine my system just like a box having a volume flow inlet and a pressure outlet since I am modeling it as open loop system as of now. Inside that box there are some trays (solid body) over which cool air flow. I am modeling it as internal flow simulation and able to find out operating point.

I am stuck at below problems

1) For heat transfer study I turn on "heat conduction in solid" And give "outer wall temperature". By this definition mesher will put cells in solid regions in contact with fluid. But I want to avoid mesh inside the trays since those does not take part in heat transfer. Trays are just like obstacles to fluid flow. Is there any way to avoid mesh inside some solid regions for such kind of simulation? Since my mesh count in heat transfer study goes to 4M where as with same mesh settings mesh count is 1.2 M for only flow simulation where trays are not meshed inside.

2) In only flow simulation I am trying to use Fan boundy condition on faces where I used volume flow inlet and pressure outlet since in reality my system is closed loop system where cool air recirculate through refrigerator.
I found that when I use "external inlet fan" , I am getting operating point flow rate lower than actual flow rate and same apply to pressure drop value. But when I use "internal fan" boundary condition I am able to get correct operating point flow rate and dP. But in that case my Inlet and outlet total pressure values goes on increasing for indefinite iteration when put them for convergence. In short total pressure values at inlet and outlet are not correct for "internal fan boundary condition".
I tested both fan on a simple pipe with orifice inside to compare results with theoretical values anf found same behavior. Should I supposed to get operating point from CFD on fan curve?
cfd_user_pune is offline   Reply With Quote

Old   January 30, 2020, 03:00
Default
  #2
Senior Member
 
Boris Marovic
Join Date: Jul 2009
Posts: 600
Rep Power: 20
Boris_M will become famous soon enough
Hi Pramod,

Ok, I think I can help you with your first question:
You can apply Insulator material on the parts that shall not take part in the heat transfer. Everything will be meshed, but cells do not show for the insulator parts or if there is no heat conduction. But they still take up some space in the memory, basically filled with zeros. But if you use insulator material, these cells don't get computed and therefore save CPU time.

As for the second question:
I understand your setup to some degree, just not sure how and where you apply the internal fan compared to the external inlet fan as this of course can influence what comes out. An internal fan has the fan intake and outlet surface defined and if you only have an inlet on the one end and an outlet on the other, then I'm not sure where the intake surface of the fan (sucking side) is.
Also you have to consider that the external inlet fan has a pressure given which is used to calculate the dP for the fan and its flow rate according to the fan curve.
For an internal fan, the dP is measured between the two faces of the fan.
Also it depends on which type of pressure drop measurement you chose as this will define how the dP is measured. It might use Ptotal or Pstatic and will also depend if you use an external inlet fan or an internal fan.
Maybe this is causing the deviation as you expect it to be calculated this way but it actually uses the other pressure values to calculate it.
You can find out which method is used in the Help if you search for "Fans - Basic information".

Also since I don't know your model setup, I might be wrong in what I'm saying as it depends on the model, but if you have the inlet on the one side of the box and the outlet on the other side, then the dP is for the fan curve is not the dP between these two inlet and outlet. The dP for the fan is between the fan intake and outlet surface of the fan.

Regards,
Boris
peterjfrancis likes this.
Boris_M is offline   Reply With Quote

Old   January 31, 2020, 12:49
Exclamation FloEFD Fan Boundary Condition
  #3
New Member
 
Join Date: Oct 2018
Posts: 22
Rep Power: 3
cfd_user_pune is on a distinguished road
Dummy_Model.jpg

Fan Curve.jpg

Hi Boris,

Thank you for the reply and your help.

Regarding mesh, I have already tried using insulator as material for objects those don't take part in heat transfer. As you correctly said, those parts wont be solved but mesh will be formed inside those objects. I was guessing if FloEFD has such option where one can specify material as orphan or obstacle similar to other commercial meshing tool. Anyway I am not much bothered as of now for increased mesh count.

Regarding Fan Boundary Condition, I am still trying to figure out where I am doing wrong. I am attaching dummy model and a fan curve sketch. I am not modeling evaporator coil and fan into my simulation (neglecting dotted region). As of now I am not sure if that fan is suction fan or forced draft fan. Only thing I have is Fan curve based on Total Pressure Rise (Pt).

Referring to fan curve sketch, I am plotting impedance curve doing parametric simulation (which is really helpful tool in FloEFD) for a range of flow rate. In parametric simulation I am defining "Inlet" as Volume Flow Rate inlet and "Outlet" as Static Pressure outlet (101325 Pa).The intersection point of Fan curve and Impedance curve is the operating point at which Fan should operate as per theory.

In next simulation I am using "External Inlet Fan" where "inlet" is used as fan exit face and "outlet" as static pressure (101325 Pa). Same Fan curve has been given to solver selecting Total Pressure Rise (Pt) option and reference density of 1.2 kg/m3 (air). From this simulation I got operating point which different from point got from parametric simulation. I was expecting to get that point on Fan curve since it is input to solver.

In third simulation, I am using "Internal Fan" where "inlet" is used as fan exit face and "outlet" as fan entry face. Same fan curve is used. From this simulation I get operating point fairly close to that from parametric study. But Total pressure at inlet and outlet face goes increasing when put them into convergence criteria for indefinite iterations.

In all three simulation dP = Inlet total pressure - Outlet Total Pressure

I have tried "External Inlet Fan as inlet BC" and Pressure Outlet (101325 Pa) as outlet BC on simple pipe with perforated plate inside. I setup my own fan curve based on total pressure rise (pa) and used in external inlet fan bc. After pressure and velocity convergence I got similar kind of results where simulation gave me lesser value of flow rate and dP than true (intersection point) respective values.

If I am making mistake in defining fan can please suggest me which type of fan bc is more suitable in this case. (Internal fan, external inlet fan or else assuming real fan is forced draft fan)?

Last edited by cfd_user_pune; February 3, 2020 at 01:04.
cfd_user_pune is offline   Reply With Quote

Old   February 4, 2020, 05:40
Default
  #4
Senior Member
 
Boris Marovic
Join Date: Jul 2009
Posts: 600
Rep Power: 20
Boris_M will become famous soon enough
Ok, I just tested it on a straight pipe with an orifice as well. I ran a parametric study for various flow rates and then let the fan curve run on the inlet as well with a total pressure increase. I used the Papst DC 412 fan and switched it to the total pressure increase setting and measured the total bulk average pressure at the inlet as well as the flow rate and the set the total pressure on the outlet with 1atm and the same in the fan curve for the pressure of the not existing fan intake face as I used the external inlet fan.

You can see in my test that the fan curve in blue in my excel calculation where I gathered the data and the system curve in green cross exactly where the fan working point is when I use the fan curve and that is also seen in the other image of the simulation with the fan curve shown.
I just noticed that I named the fan working point "fan curve" this is of course not the fan curve, I meant this is the result from the fan curve calculation.

Not sure what you are doing wrong. Do you measure the bulk average values for the goals? The average values are surface averaged which can lead to different values than the bulk average which is mass flow averaged.

Regards,
B
Attached Images
File Type: jpg test1.jpg (48.4 KB, 22 views)
File Type: jpg test2.jpg (79.6 KB, 21 views)
cfd_user_pune likes this.
Boris_M is offline   Reply With Quote

Old   February 5, 2020, 11:46
Default Fan curve boundary condition
  #5
New Member
 
Join Date: Oct 2018
Posts: 22
Rep Power: 3
cfd_user_pune is on a distinguished road
Hi Boris,

Thank you for taking time to run test case and sharing results.
I will rerun my setup targeting lower pressure drop values and share results.
(I am using bulk average values of total pressure to calculate dP)

Thank you,
Pramod

Last edited by cfd_user_pune; February 5, 2020 at 13:26.
cfd_user_pune is offline   Reply With Quote

Old   February 6, 2020, 02:59
Default
  #6
Senior Member
 
Boris Marovic
Join Date: Jul 2009
Posts: 600
Rep Power: 20
Boris_M will become famous soon enough
Yes, I can provide you with the model file, but you'll need FLOEFD 2019.4 to see the project settings. Do you have that?

Unfortunately, it is a few kB too big to post it here directly, so here is the FTP download link:
Donwload

Regards,
Boris
Boris_M is offline   Reply With Quote

Old   February 13, 2020, 01:32
Default Fan boundary condition
  #7
New Member
 
Join Date: Oct 2018
Posts: 22
Rep Power: 3
cfd_user_pune is on a distinguished road
Hi Boris,

I do not have 19.4 version. I will rerun your case later on.

I am attaching my case setup snapshot and its result.I followed same way as you told. Still not able to get operating point as intersection point when used External Inlet Fan. As I said early, with Internal Fan BC I am getting operating point at intersection but total bulk pressure values at inlet & outlet doesn't seem get converged. They goes on increasing!

Have you tried Internal Fan on your case?

Regards,
Pramod
Attached Images
File Type: jpg Cad.jpg (36.2 KB, 10 views)
File Type: jpg Convergence_Both_Fans.jpg (64.9 KB, 11 views)
File Type: jpg Fan_Data.jpg (47.9 KB, 8 views)
File Type: jpg Result.jpg (12.9 KB, 11 views)
File Type: jpg Velocity_Contours.jpg (18.4 KB, 9 views)
cfd_user_pune is offline   Reply With Quote

Old   February 13, 2020, 01:36
Default Fan boundary condition
  #8
New Member
 
Join Date: Oct 2018
Posts: 22
Rep Power: 3
cfd_user_pune is on a distinguished road
This is CAD file I used.
Attached Files
File Type: zip Rectangular_Channel.zip (8.9 KB, 1 views)
cfd_user_pune is offline   Reply With Quote

Old   February 13, 2020, 05:25
Default
  #9
Senior Member
 
Boris Marovic
Join Date: Jul 2009
Posts: 600
Rep Power: 20
Boris_M will become famous soon enough
It would be easier if you could share it with your project settings. You can also sent it or a download link in a PM if you prefer not to share the model publicly.

Regards,
Boris
Boris_M is offline   Reply With Quote

Reply

Tags
floefd, heat transfer, meshing, refrigeration

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
FAN 3D geometry and meshing for ANSYS FLUENT jose_1953 CFD Freelancers 5 July 25, 2019 15:15
Velocity jump boundary condition ASofia OpenFOAM Programming & Development 0 July 14, 2016 09:01
[GAMBIT] fan Meshing Aadhavan ANSYS Meshing & Geometry 0 December 26, 2012 08:15
meshing fan blade in tunnel... fadly CFX 4 August 10, 2007 16:52
Problems with Fan boundary condition Nish FLUENT 2 August 27, 2004 18:27


All times are GMT -4. The time now is 01:23.