# "prevent fluid from flowing into the domain"

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

 March 13, 2008, 11:09 "prevent fluid from flowing into the domain" #1 J Guest   Posts: n/a Hi guys... During simulations I got this message: Notice A wall has been placed at portion(s) of an OUTLET boundary condition (at 1.3% of the faces, 0.9% of the area) to prevent fluid from flowing into the domain. The boundary condition name is: Outlet2. The fluid name is: Blood1. If this situation persists, consider switching to an Opening type boundary condition instead. I put as boundary condition the average pressure. In ICEM if I run Build Topology I found a blue triangle in this outlet. Somebody have an idea to correct this problem? Thanks guys J

 March 13, 2008, 16:09 Re: "prevent fluid from flowing into the domain" #2 Usman Guest   Posts: n/a Wall is being placed on very small area (0.9%) which i think should not affect your solution too much. I would say carry on with the simulation and see how out come is affected. or Switch your outlet BC to opening for some iteration and then swich it back to your normal BC. If problem still persists then, You will have to move your outlet further downstream. Usman

 March 14, 2008, 03:46 Re: "prevent fluid from flowing into the domain" #3 Neel Guest   Posts: n/a Hi Usman, What if areas are 100% of the faces and 100% of the area?

 March 14, 2008, 06:57 Re: "prevent fluid from flowing into the domain" #4 Usman Guest   Posts: n/a In that case my friend you have problem at hand. Switch to opening BC and run it for lets say 40 iterations or time steps. And then switch back to normal BC. In my simulations message under consideration usually disappears when i do that. Usman

 March 14, 2008, 15:56 Discussion continued. #5 Kushagra Guest   Posts: n/a I am relatively new to CFD, hence my comments should be taken as my offence .. The impression that I got from many people, that outlet (flow out of domain) is the only physically sensible boundary condition at outflow boundaries. I think it may be right for most of the cases. Hence the suggestions to 1) extend the outlet pipes OR 2) to change the 'outlets' to 'openings' for some time and then rechange it to 'outlets' may work as it helps removing the numerical affect. BUT for some cases, flow 'in' and 'out' at the same boundary is indeed. Hence using an 'opening' for whole simulation should not be a bad idea. AGAIN remember, 'openings' are not good with LES type models. They make linear solver fail very often (atleast CFX fails for me. While I have read that FLUENT is pretty stable with LES and 'pressure-outlet' BCs which are nothing but 'opening' in CFX). So I may suggest not to buy the idea of always using outlets. Think about the physics of your problem and then take the decision. Mostly 'outlet' will be the appropriate decision. And I would love to hear the feedback upon my comments. I just learnt it from my experience so far. There may be need of correction. Cheers, Kushagra

 March 14, 2008, 15:57 Re: Discussion continued. #6 Kushagra Guest   Posts: n/a correction.... I am relatively new to CFD, hence my comments should NOT be taken as my offence ..

 March 17, 2008, 05:21 Re: "prevent fluid from flowing into the domain" #7 Neel Guest   Posts: n/a Hi Guys, Thank you for advicing me on this. I tried using "opening" initially for 50 iteractions and then switched back to 'outlet' and ran it over the weekend. I still get 100% faces & areas. I also get negative pressures.

 March 17, 2008, 08:04 Re: "prevent fluid from flowing into the domain" #8 Usman Guest   Posts: n/a Hi Neel Are you simulating RANS case or is it LES? You can switch to opening BC if your case is RANS as Kushagra mentioned and see how that will affect your results. As a last resort you will have to draw your model again and move your outlet further downstream. Usman

 March 17, 2008, 09:31 Re: "prevent fluid from flowing into the domain" #9 Neel Guest   Posts: n/a Hello guys, I am not using RANS nor LES, I have chosen k-epsilon model for this.( I am using ansys 10.0)I thought it k-epsilon is a good start. what do you suggest?

 March 17, 2008, 10:31 Re: "prevent fluid from flowing into the domain" #10 Magnoli Guest   Posts: n/a Hi, if you are using k-e, you are using RANS.

 March 17, 2008, 11:38 Re: "prevent fluid from flowing into the domain" #11 Kushagra Guest   Posts: n/a You must extend your domain at its outlet up to a good length......this will make sure that the domain does not get affected by the outlet boundary condition... then if the backflow still occurs, use opening type boundary condition.....and when the simulation converges, see if reverse flow is there...draw vectors at outlets...and see Now, as you mention that negative pressure (I assume you mean less than pressure at outlet) occurs, it seems to me a physical problem....Though may be a very less amount of reverse flow is expected....Is the area of outlet cross section is very small? then may be the 'imposed' outflow boundary condition is messing up the whole simulation and you are getting 100% backflow...it happened with me once... As you are using k-e, 'opening' will not give any convergence problem....if you were using LES then you had problem... try it out and let us know

 March 17, 2008, 11:47 Re: "prevent fluid from flowing into the domain" #12 Neel Guest   Posts: n/a Hi, Thank you for the responses. I understand now perfectly. Thank you Magnoli for confirming. As Kushagra and Usman instructed, I will extend the outlet pipe and use 'outlet'. If i still get backflow then i ll use 'opening'instead. I am wondering if i use 'opening' and 'static pressure of 12000 Pa' will there be any liquid hold up?!? Thanks, Neel

 July 31, 2009, 23:47 #13 New Member   King Join Date: Mar 2009 Posts: 8 Rep Power: 9 I am having the same problem. How do you change the BC from opening to outlet when it is running? I went to 'Edit Run in Progress' but I am not allowed to change the BC.

August 1, 2009, 00:45
#14
Member

Join Date: Jun 2009
Posts: 56
Rep Power: 9
Quote:
 Originally Posted by Neel ;86908 Hi, Thank you for the responses. I understand now perfectly. Thank you Magnoli for confirming. As Kushagra and Usman instructed, I will extend the outlet pipe and use 'outlet'. If i still get backflow then i ll use 'opening'instead. I am wondering if i use 'opening' and 'static pressure of 12000 Pa' will there be any liquid hold up?!? Thanks, Neel
hi Neel:
are you working on a blood flow?would you please tell me some details about your current work?i am modeling a blood vessel using fsi and i have some problems.

 August 1, 2009, 02:20 #15 New Member   dss Join Date: Jul 2009 Posts: 25 Rep Power: 9 Hi, You can change the calculate region, let the outlet is far from your structure.It is Ok! The second method is change the bounday to opening.It is OK! But the best method is the first.

August 1, 2009, 11:49
#16
New Member

King
Join Date: Mar 2009
Posts: 8
Rep Power: 9
Quote:
 Originally Posted by flyingd Hi, You can change the calculate region, let the outlet is far from your structure.It is Ok! The second method is change the bounday to opening.It is OK! But the best method is the first.
Hi,
Thanks for your advice but how do I change the outlet further from the structure? Do I have to use some kind of expression?
Thank you

 August 2, 2009, 00:32 reply #17 New Member   dss Join Date: Jul 2009 Posts: 25 Rep Power: 9 You can make wave region of your calculation longer.It is oK!.

 August 3, 2009, 21:17 #18 Senior Member   Bharath kumar Join Date: Apr 2009 Posts: 168 Rep Power: 9 Hi guys, is it really need of changing from opening to outlet after some iterations?how it affects the solution?

August 3, 2009, 22:28
outlet setting
#19
New Member

dss
Join Date: Jul 2009
Posts: 25
Rep Power: 9
Quote:
 Originally Posted by bharath Hi guys, is it really need of changing from opening to outlet after some iterations?how it affects the solution?
Hi:
If the calculation of region is enough length, the outlet needn't change.
If there is free surface, the outlet will be set STATIC PRESSURE.
If there is not free surface, the out let will be set ave pressure zero.

 January 26, 2014, 10:33 #20 New Member   Mustapha Join Date: Jan 2014 Posts: 2 Rep Power: 0 Im having the same problem but Im using Ansys CFX 14.0 working to model a van in a flow domain. After 20 iterations out 60, I receive the same error but dont know how to proceed as recommended i.e "how to switch to Opening type BC" see the error notice I received: Notice ****** A wall has been placed at portion(s) of an OUTLET boundary condition (at 1.0% of the faces, 0.9% of the area) to prevent fluid from flowing into the domain. The boundary condition name is: outlet.The fluid name is: Fluid 1. If this situation persists, consider switching to an Opening type boundary condition instead.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Sumedh CFX 8 May 26, 2015 08:31 robingilbert OpenFOAM 7 September 2, 2010 14:39 Fonzie CFX 3 August 24, 2010 19:42 Riken CFX 0 October 28, 2009 10:51 HervĂ© CFX 2 June 16, 2008 06:40

All times are GMT -4. The time now is 00:21.