CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

Prevent turbulence generation in and transport through a porous zone

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   July 21, 2022, 05:19
Default Prevent turbulence generation in and transport through a porous zone
  #1
siw
Senior Member
 
Stuart
Join Date: Jul 2009
Location: Portsmouth, England
Posts: 733
Rep Power: 25
siw will become famous soon enough
I'm modelling a internal airflow system which contains a filter (incompressible flow with the SST model). The filter is modelled macroscopically as a subdomain with experimental derived permeability and loss coefficient in the streamwise direction and the default streamwise multiplier for the traverse directions. The porous zone pressure drop is as expected from the experimental data.

In reality the narrow, random pathways through the filter will prevent upstream eddies passing through and then downstream. Also the turbulence generated in the filter will not happen as locally the flow is laminar. So just downstream of the porous zone the k-omega values must 'start again'. In CFX I guess a sink expression is needed (with a total coefficient). Anyone have a clue what expression I could use? In Fluent a laminar zone or enforced source value can be set. But I'm not sure how to set k and omega to 0 in the porous zone.

Thanks
siw is offline   Reply With Quote

Old   July 21, 2022, 05:40
Default
  #2
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,827
Rep Power: 27
Gert-Jan will become famous soon enough
I would just give it a try with several values. In principle, you just want get rid of the turbulence, so the lower the better, I would say.

Alternatively, I would try to switch off the option "Constant Domain Physics" under Options>General>Beta Options. This allows you to run turbulent in domain 1, and laminar in domain 2. This works pretty if these are separated by a wall. Not sure if it works when they are connected and the fluid flows from turbulent to laminar, but you could give it a try.
Gert-Jan is offline   Reply With Quote

Old   July 21, 2022, 06:24
Default
  #3
siw
Senior Member
 
Stuart
Join Date: Jul 2009
Location: Portsmouth, England
Posts: 733
Rep Power: 25
siw will become famous soon enough
Not sure yet if I can just enter very low numbers into CFX-Pre Subdomain area.

It will take some trying but I want to stop turbulence from the upstream fluid domain transporting through the porous domain, whilst also stopping new turbulence generation in the porous domain (the Fluent laminar zone option only does the latter).
siw is offline   Reply With Quote

Old   July 21, 2022, 06:32
Default
  #4
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,827
Rep Power: 27
Gert-Jan will become famous soon enough
Shouldn't you set a huge Eddy Dissipation Rate?
Gert-Jan is offline   Reply With Quote

Old   July 21, 2022, 10:15
Default
  #5
Senior Member
 
Join Date: Jun 2009
Posts: 1,803
Rep Power: 32
Opaque will become famous soon enough
Have you thought about setting Eddy Viscosity = 0 in the porous domain? The equation is solved, but no diffusion and no production.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Old   July 21, 2022, 19:00
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,699
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Yet another approach to consider is to use the turbulence transition model, with specified intermittency. This way you can explicitly set the laminar and turbulent bits. So set the foam as laminar and the flow domain as turbulent.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is online now   Reply With Quote

Old   August 11, 2022, 05:34
Default
  #7
siw
Senior Member
 
Stuart
Join Date: Jul 2009
Location: Portsmouth, England
Posts: 733
Rep Power: 25
siw will become famous soon enough
Quote:
Originally Posted by Opaque View Post
Have you thought about setting Eddy Viscosity = 0 in the porous domain? The equation is solved, but no diffusion and no production.
How can this be achieved?
siw is offline   Reply With Quote

Old   August 11, 2022, 09:19
Default
  #8
Senior Member
 
Join Date: Jun 2009
Posts: 1,803
Rep Power: 32
Opaque will become famous soon enough
Quote:
Originally Posted by siw View Post
How can this be achieved?
In the panel for Domain/Fluid Models/Turbulence/Advanced Turbulence Control
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Old   August 15, 2022, 01:54
Default
  #9
siw
Senior Member
 
Stuart
Join Date: Jul 2009
Location: Portsmouth, England
Posts: 733
Rep Power: 25
siw will become famous soon enough
Quote:
Originally Posted by Opaque View Post
In the panel for Domain/Fluid Models/Turbulence/Advanced Turbulence Control
Unfortunately, that would switch the eddy viscosity off in the entire flow-field. I have one fluid domain and multiple subdomains for the filter volumes. In SpaceClaim I used Shared Topology to share the adjoining faces. Otherwise, if I did not use Shared Topology I would have to split the single fluid domain into separate domain and use CFX Interfaces to connect them, then in CFX I would need to assign separate domains, each with the turbulence model etc.

Ideally, there would be a option in the subdomain Equation Sources to do this.
siw is offline   Reply With Quote

Old   August 15, 2022, 02:14
Default
  #10
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,699
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
I cannot see how you can use Opaque's suggestion wither. Hopefully he can explain how to do it.

So can't you just use a source term to set k=0 in the filter regions?

Note you don't want to set omega =0, that might lead to problems. I would just let omega go to any value it wanted.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is online now   Reply With Quote

Old   August 15, 2022, 05:55
Default
  #11
siw
Senior Member
 
Stuart
Join Date: Jul 2009
Location: Portsmouth, England
Posts: 733
Rep Power: 25
siw will become famous soon enough
I am giving the TKE source term a try now within the subdomain, based on the general momentum source term equation of -C(k - kspec), where kspec is zero and C is the CFX recommended value of 1x10^5.

Glenn, interesting that you say to leave omega alone. I have CFX running now and I did set it as a source term also: -C(omega). I'll see what it looks like.

Thanks.
siw is offline   Reply With Quote

Old   November 15, 2022, 02:33
Default
  #12
siw
Senior Member
 
Stuart
Join Date: Jul 2009
Location: Portsmouth, England
Posts: 733
Rep Power: 25
siw will become famous soon enough
Quote:
Originally Posted by Opaque View Post
Have you thought about setting Eddy Viscosity = 0 in the porous domain? The equation is solved, but no diffusion and no production.
I have found how to do this from an entry in the Ansys Knowledge Resource (#2046598) on the Ansys Customer Portal, titled 'How to Model Laminar Flow in One Domain and Turbulent Flow in Adjacent Domain'. There an expression is used to set the eddy viscosity (SST advanced option) to a very low number in a domain or subdomain for the porous volume: e.g. eddyvisc = if(inside()@Porous==1,1.e-18[Pa s],Eddy Viscosity).

Taking this one step further, but I cannot get it to work yet. In my CFX model I have 1 domain and I use a subdomain for each porous volume to input the directional loss model values. How can I extend the above expression for multiple porous volume subdomains, since I have only one domain? I tried using the AND operator in the expression for each subdomain e.g. if(inside()@Porous1==1&&inside()@Porous2==1,1.e-18[Pa s],Eddy Viscosity) but CFX-Solver Manager gave an error code which I could not resolve (see image) and also tried using the OR operator but that also failed.
Attached Images
File Type: jpg Capture.JPG (49.0 KB, 6 views)
siw is offline   Reply With Quote

Old   November 15, 2022, 03:46
Default
  #13
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,699
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
I should have mentioned this a long time ago, but do you need to do any of this? If you just model everything with a turbulence model which degenerates nicely to laminar flow (like SST or k-w, k-eps does not) then the turbulence will naturally fade to zero in the laminar bits and it will be very close to the laminar solution in those regions.

I have done several tests of SST turbulence models in benchmark laminar flows and found that the error is tiny in many cases (a fraction of a percent).

So I would try just running the whole thing with the SST model. Do a benchmark simulation to check, maybe just of the filter element to check the SST model does degenerate acceptably close to a laminar solution - I bet you will it is close enough for what you are doing, and does not require weeks of your development and debugging time.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is online now   Reply With Quote

Reply

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



All times are GMT -4. The time now is 19:19.