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

permeable wall

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

Like Tree3Likes
  • 1 Post By Gert-Jan
  • 1 Post By ghorrocks
  • 1 Post By Gert-Jan

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   November 30, 2019, 05:24
Wink permeable wall
  #1
Member
 
Zese
Join Date: Sep 2013
Posts: 40
Rep Power: 8
zese is on a distinguished road
Dear Friends

I have a highly swirling flow in a pipe and I want to damp it before outlet using an external force because I want to have a straight streamline at the outlet. do you know how I can set suction, blowing or permeablity at the wall in cfx?

Best regards
zese is offline   Reply With Quote

Old   November 30, 2019, 16:11
Default
  #2
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Posts: 921
Rep Power: 15
Gert-Jan is on a distinguished road
you can create a volume with subdomain with a high resistance next to the outlet.

But to be honest, why do you want this?
Gert-Jan is offline   Reply With Quote

Old   November 30, 2019, 16:15
Default
  #3
Member
 
Zese
Join Date: Sep 2013
Posts: 40
Rep Power: 8
zese is on a distinguished road
Dear Gert-Jan

thanks very much for your answer. excuse me what do you mean about high resistance?

I am aiming to do stability analysis and it is sensitive to the outlet BC and swirl must be damped.

Quote:
Originally Posted by Gert-Jan View Post
you can create a volume with subdomain with a high resistance next to the outlet.

But to be honest, why do you want this?
zese is offline   Reply With Quote

Old   November 30, 2019, 16:23
Default
  #4
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Posts: 921
Rep Power: 15
Gert-Jan is on a distinguished road
Then it is better to extend your domain. Meaning, you have to place your outlet further downstream. That's better than adding a volume with flow resistance which is easy but not realistic.
zese likes this.
Gert-Jan is offline   Reply With Quote

Old   December 1, 2019, 03:35
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,920
Rep Power: 122
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Alternately you can use a source term which sets the swirl velocities to zero.

But as Gert-Jan states, be very careful doing this (or any of the other artificial approaches) as the result might not be realistic. If the actual device is sensitive to swirl then it probably has some device in it to stop the swirl - so then the best approach is to model that device.
zese likes this.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   December 1, 2019, 03:39
Default
  #6
Member
 
Zese
Join Date: Sep 2013
Posts: 40
Rep Power: 8
zese is on a distinguished road
thank you.
in some papers I saw that they used a sponge region next to the outlet but their Reynolds number was 300 however my Re is 400000 and extending the pipe doesn't damp it in outlet unless I use a very long one which is computationally expensive.

Quote:
Originally Posted by ghorrocks View Post
Alternately you can use a source term which sets the swirl velocities to zero.

But as Gert-Jan states, be very careful doing this (or any of the other artificial approaches) as the result might not be realistic. If the actual device is sensitive to swirl then it probably has some device in it to stop the swirl - so then the best approach is to model that device.
zese is offline   Reply With Quote

Old   December 1, 2019, 17:44
Default
  #7
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Posts: 921
Rep Power: 15
Gert-Jan is on a distinguished road
You need to come with an extended description and a picture of what you are modelling and what the problem exactly is. Otherwise we are not able to help.
Gert-Jan is offline   Reply With Quote

Old   December 2, 2019, 03:59
Default
  #8
Member
 
Zese
Join Date: Sep 2013
Posts: 40
Rep Power: 8
zese is on a distinguished road
you are right

I am modeling a swirl generator which in it's draft tube vortex rope and a high swirling flow happen (fig is attached). now for further calculations I need an area of straight streamlines without swirling near the outlet. In a paper sponge region was proposed which was somehow like porosity assumption. they decreased Re number from 300 to 0.1 in a 60mm distance (fig2). I extended the draft tube for 2 meters it wasnt damped. you talked about flow resistance and after reading manual I didnt know how I should define the coeffs.

In addition some proposed using an external force.


Quote:
Originally Posted by Gert-Jan View Post
You need to come with an extended description and a picture of what you are modelling and what the problem exactly is. Otherwise we are not able to help.
Attached Images
File Type: png CFX_001.png (133.3 KB, 10 views)
File Type: png CFX_021.png (60.8 KB, 8 views)
zese is offline   Reply With Quote

Old   December 2, 2019, 04:42
Default
  #9
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Posts: 921
Rep Power: 15
Gert-Jan is on a distinguished road
Weird approach. Why do you need something without swirl? If you explain why you need this, then we might come with a more realistic approach.

Nevertheless, the article did not use resistance. They increased the dynamic viscosity somehow. Probably they had an expression for the dynamic viscosity as function of coordinate Z. Not sure if that is allowed in CFX.
(BTW, I don't believe the low Reynolds numbers given the huge dimensions).

Alternatively, create a additional volume next to the outlet, define a subdomain there with a high resistance (with streamwise coefficients?). But I already mentioned that above. Be carefull, it will increase the pressure which will affect density.
zese likes this.
Gert-Jan is offline   Reply With Quote

Old   December 2, 2019, 04:48
Default
  #10
Member
 
Zese
Join Date: Sep 2013
Posts: 40
Rep Power: 8
zese is on a distinguished road
I told that I want a flow without swirling at the outlet because stability analysis is highly sensitive to outlet BC. if I dont do such a thing the frequency that the stability show me is not accurate.

about the second picture, yes they used a relation based on z to decrease Re to 0.1 at the outlet and I defined it using function in cfx in nondimensional matter and define a new material.

thank you for your response

Quote:
Originally Posted by Gert-Jan View Post
Weird approach. Why do you need something without swirl? If you explain why you need this, then we might come with a more realistic approach.

Nevertheless, the article did not use resistance. They increased the dynamic viscosity somehow. Probably they had an expression for the dynamic viscosity as function of coordinate Z. Not sure if that is allowed in CFX.
(BTW, I don't believe the low Reynolds numbers given the huge dimensions).


Alternatively, create a additional volume next to the outlet, define a subdomain there with a high resistance (with streamwise coefficients?). But I already mentioned that above. Be carefull, it will increase the pressure which will affect density.
zese is offline   Reply With Quote

Old   December 2, 2019, 17:17
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,920
Rep Power: 122
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
I think you will find your proposed methods of stopping swirl create more problems than is present when you just model the device with swirl. So I would recommend modelling the device as is, with no special treatment, and see if you have any problems - if not then forget about stopping the swirl.

To be more specific: When you stop the swirl through Bernoulli's equation you will increase the pressure. This will then change the pressure drop through the device and change the entire flow field. You can't stop the swirl without affecting the device.

If the actual device has something in it to stop the swirl then your model should include those devices. If the actual device does not have anything to stop the swirl then that is how you should model it, and let the swirl go right through the device.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   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


Similar Threads
Thread Thread Starter Forum Replies Last Post
Enhanced Wall Treatment paduchev FLUENT 24 January 8, 2018 12:55
What's the problem with turbulence models near the wall region? Jaydi_21 Main CFD Forum 6 July 7, 2017 03:39
Centrifugal fan-reverse flow in outlet lesds to a mass in flow field xiexing CFX 3 March 29, 2017 11:00
Radiation interface hinca CFX 15 January 26, 2014 18:11
permeable wall peter.zhao Main CFD Forum 0 October 23, 2000 09:06


All times are GMT -4. The time now is 18:15.