# Periodic Inlet/Outlet with static pressure Value

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

 June 20, 2013, 09:06 Periodic Inlet/Outlet with static pressure Value #1 Member   Marco Antonio Join Date: Nov 2012 Posts: 46 Rep Power: 6 Hi guys, I am trying to model a flow into an infinite duct. I have no problem setting up the periodic inlet/outlet or the pressure gradient either, but cfx doesn't allow to set a static pressure at inlet too. I do need its value for what i am trying to model, not only the gradient itself. Suggestions?

 June 20, 2013, 18:38 #2 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,853 Rep Power: 107 This does not make sense. The periodic pair approach gives you the pressure drop per length of duct. So obviously you cannot define a pressure as well. If you want to define the pressure then you are looking at just one location in the duct and you do not have a periodic simulation.

 June 29, 2013, 02:59 #3 Member   Marco Antonio Join Date: Nov 2012 Posts: 46 Rep Power: 6 Glen thanks again. Is it correct to say that anyway we would have more Bc than needed? Because we would say v(X) = v(X+h) while trying to fix static pressure value every where both at inlet and outlet?

 June 29, 2013, 07:15 #4 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,853 Rep Power: 107 Yes, this would over-specify the problem. I presume the simulation is incompressible (I do not think the periodic assumption applies if it is compressible), and in that case you just define a pressure reference point. Pressures are calculated relative to that point.

 June 29, 2013, 07:28 #5 Member   Marco Antonio Join Date: Nov 2012 Posts: 46 Rep Power: 6 Thanks Glen. To set the press ref point, should i just set the reference pressure as usual?

 June 29, 2013, 07:35 #6 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,853 Rep Power: 107 On a quick read of the documentation I am not sure how CFX handles this. This is how most incompresisbel solvers handle it, but I am not sure what CFX does.

 June 29, 2013, 08:17 #7 Member   Marco Antonio Join Date: Nov 2012 Posts: 46 Rep Power: 6 Glen if it works and i have a multiphase sim how can i set 2 reference points for 2 domains?

 June 29, 2013, 08:24 #8 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,853 Rep Power: 107 If what works? And what does a multiphase simulation and 2 domains have to do with 2 reference points?

 June 29, 2013, 14:10 #9 Member   Marco Antonio Join Date: Nov 2012 Posts: 46 Rep Power: 6 Basically, the model is always the same i spoke about some threads ago. At 1 and 2 we have periodic conditions, and i want P > P0 to be set at a medium value with a small but yet present Delta P along x. This is why i do need the pressure medium value in Fluid domain to stay at P and not only define the Delta P. I know this would not be periodical in truth, but i guess this is the most appropriate condition since the delta P is very small and i expect the velocity field to be the same at 1 and 2. Thanks in advance.

 June 29, 2013, 19:08 #10 Senior Member   Chris DeGroot Join Date: Nov 2011 Location: Canada Posts: 388 Rep Power: 8 CFX uses certain pressure conditions for fluid porous interfaces, so if you were to specify different pressures on 1 and 2 the simulation will likely not converge because these will conflict with what the interface conditions are trying to do. Just set the delta p and the solver will figure out the correct pressure jump (if any) across the interface. Look up the expert parameter "porous cs descretisation option" for the 3 different options.

 June 30, 2013, 12:53 #11 Member   Marco Antonio Join Date: Nov 2012 Posts: 46 Rep Power: 6 The pressure jump is due to physics.. Is there a way to define periodic bc while keeping a medium pressure value of phase 1? Because it's due to that, that a flow to porous side applies. The SIM is transient

 June 30, 2013, 13:02 #12 Senior Member   Chris DeGroot Join Date: Nov 2011 Location: Canada Posts: 388 Rep Power: 8 Maybe it would help if you explained a little bit more what you are trying to model. If the flow is purely along the direction of the duct, i.e. no flow through the fluid-porous interface, then the pressures on either side of the interface should be the same... to try to apply different pressure on the periodic boundaries would be working against the physics. Such a simulation won't converge. It seems like you are overcomplicating a simple simulation by trying to force the pressures to be different. Can you explain why you think the pressures should be different? To me this just looks like a transient version of the Beavers and Joseph problem where the flow is driven by a constant pressure gradient in both the fluid and porous regions. It's possible I'm misunderstanding what you are trying to do, however, hence the request for clarification.

 June 30, 2013, 13:20 #13 Member   Marco Antonio Join Date: Nov 2012 Posts: 46 Rep Power: 6 Resin infusion, vacuum assisted. We have a flow along x due delta P and a flow from fluid to porous domain due to vacuum which means we have smaller pressure inside the porous medium while the resin's outside at higher press

 July 1, 2013, 13:17 #14 Senior Member   Chris DeGroot Join Date: Nov 2011 Location: Canada Posts: 388 Rep Power: 8 Ok, I do see now why you need a different pressure in the porous zone because of the vacuum that is supposed to draw the resin in. In this case, I would suggest that a periodic boundary condition is not a good choice. If it is still drawing fluid into the porous region it's not periodic anyways. I would probably prefer static pressure conditions on the outlets (which can be different) and mass flow conditions at the inlets if possible.

 July 2, 2013, 04:58 #15 Member   Marco Antonio Join Date: Nov 2012 Posts: 46 Rep Power: 6 Thanks Chris.

 August 18, 2016, 07:47 Pressure Jump #16 New Member   cfd_guy Join Date: Apr 2014 Location: Munich, Germany Posts: 21 Rep Power: 5 Hi there, I am trying to characterize the drag of my system with and without a compressor. For an initial approximation I intend to model the compressor as a porous domain. I know the compressor pressure ratio before hand. Any previous experience doing this with CFX. Its a compressible flow. Best Regards

 August 18, 2016, 18:38 #17 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,853 Rep Power: 107 I have not seen any porous models which look like the performance curve of a compressor. The normal way of doing this is with a momentum source term where you map the flow rate to a pressure rise/drop and implement the pressure rise/drop as a source term. Then the compressor is modelled using its performance curve.

 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 Honey FLUENT 1 October 17, 2012 06:06 Honey FLUENT 0 September 19, 2012 03:21 MASOUD Fluent UDF and Scheme Programming 0 June 5, 2010 00:49 KM CFX 2 December 17, 2007 21:50 HB &DS CFX 0 January 9, 2000 14:19

All times are GMT -4. The time now is 16:32.