Does the inlet boundary condition *generate* air?

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 February 12, 2016, 18:42 Does the inlet boundary condition *generate* air? #1 Member   Join Date: Oct 2015 Posts: 54 Rep Power: 2 Hi, so I have a model - think a small rectangular box within another big rectangular box. I would like air to come in on 2 sides of the small box and out its top. So in order to make that happen, I am thinking of defining an outlet on the sides of the small rectangular box. I have air coming in from the large rectangular box. Now, I would like air that came in to shoot out the top (and into the big rectangular box). Should I define the top face as an inlet - will it use the air that came in on its sides or will it generate new air to spit out the top?

 February 12, 2016, 19:08 #2 Senior Member   Erik Join Date: Feb 2011 Location: Earth (Land portion) Posts: 547 Rep Power: 11 It will *generate* new air with the properties you give it. The Outlet will have air disappear entirely, not come into the small box. I think you need to use interfaces, and do some tutorials, as this is really basic fundamental stuff.

 February 12, 2016, 20:37 #3 Member   Join Date: Oct 2015 Posts: 54 Rep Power: 2 So what do you recommend? Use opening BC for the sides of the box? The small box is actually an air handler (sucks air from the sides and spits it from the top) - so what BC would you recommend? Or generate a new domain for the small box?

 February 13, 2016, 06:25 #4 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,395 Rep Power: 96 Air which goes out an outlet disappears. Air which comes in an inlet is magically generated. You could couple the flow rate of air at an inlet to the flow rate out of the outlet - you may have convergence issues with this. Another approach is to use a momentum source term. This just adds momentum to the flow, such as what a fan does. Then it is the same air going around and around, but the momentum source term is giving it energy to move it all about. You can also use the interface Erik suggests - this is really a momentum source term on a interface surface. This makes it a bit easier to apply.

 February 13, 2016, 13:19 #5 Member   Join Date: Oct 2015 Posts: 54 Rep Power: 2 Ok, so in the small box, I think Ill just put an outlet on the sides of mass flow rate say 100lb/s each side (200lb/s total). Let it magically disappear. Then, I will put a mass flow rate of 200lb/s on the top (magically generated). I dont really care about the flow within the small box, more interested to see what it is doing relative reference to the big box...

 February 14, 2016, 05:03 #6 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,395 Rep Power: 96 OK, this sounds like a pretty simple way to do it.

 February 14, 2016, 13:34 #7 Member   Join Date: Oct 2015 Posts: 54 Rep Power: 2 Will doing a body sizing and making the tetra mesh elements small be good enough? Should I add some inflation at the outlets/inlets as well (the bigger room has 12 inlets and 12 outlets as well)?

 February 14, 2016, 17:44 #8 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,395 Rep Power: 96 You do not put inflation layers over inlets or outlets. What mesh size is required? This is problem dependent so there is no universal answer. Do a mesh size sensitivity check and find out in your case.

 February 14, 2016, 17:57 #9 Member   Join Date: Oct 2015 Posts: 54 Rep Power: 2 So inflation goes only over walls? I thought inflation by definition means "boundary"? By the way, I want to do the tutorials in ANSYS help section, but cant find the 3d renders/models? Where do they keep those?

 February 14, 2016, 18:02 #10 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,395 Rep Power: 96 Go back to the basics - why do you put inflation layers on walls anyway? It is because there are steep gradients of flow variables near the wall due to the boundary layer. Steep gradients mean you need a fine mesh to resolve it. So walls need inflation layers (keeping in mind this applies to mid and high Reynolds number flows only, non-Newtonian and multiphase flows are more complex etc etc; the usual exceptions) Are there steep variable gradients at inlet and outlet boundaries? No. In fact some options of inlets/outlets apply zero normal gradient to make there no gradient at all. So no steep gradient means inflation is not required. There are also issues about high aspect ratio elements and flow direction - I will discuss that if you are interested.

 February 14, 2016, 18:10 #11 Member   Join Date: Oct 2015 Posts: 54 Rep Power: 2 So like in a serpentine shaped heat exchanger, we would put inflation on the the curved areas due to a drastic change in flow? I used to think a good mesh by definition is one that has the mesh metric skewness really tight? It seems this is not the case? We can have good meshes without a low skewness?

 February 15, 2016, 01:05 #12 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,395 Rep Power: 96 You put inflation layers on wall boundaries. I do not see how a serpentine heat exchanger is any different to any other device in that respect. The key mesh quality measures are aspect ratio, orthogonality and size ratio of adjacent volumes. But what mesh quality your simulation requires is strongly dependent on what you are modelling. Some flows work fine with horrible meshes (eg low Re flows), some flows require meshes which are just about perfect and have almost no tolerance to deviations from 1:1 aspect ratio and 90 degree orthogonality (eg surface tension models).

 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 Ozgur_ FLUENT 5 August 25, 2015 04:58 jaypatel OpenFOAM 8 February 20, 2014 13:12 murali CFX 5 August 3, 2012 08:56 Tudor Miron CFX 15 April 2, 2004 06:18 Tudor Miron CFX 17 March 19, 2004 20:23

All times are GMT -4. The time now is 16:19.

 Contact Us - CFD Online - Top