# Hydro Penstock Boudary conditions

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

 November 29, 2011, 16:50 Hydro Penstock Boudary conditions #1 New Member   Claude Munger Poirier Join Date: Nov 2011 Posts: 3 Rep Power: 7 Sponsored Links Good Afternoon All, I am doing a Steady State CFD analysis of a Hydro Penstock Y connexion both pipes have 11 ft in diam. Connexion is at 62 degrees. Two Inlets and One Outlet with ANSYS 13. For boundary conditions I am giving the Velocities at inlet 1 and 2. At the outlet (0nly one) I am putting a zero Pressure. Some of my collegues are arguing that I should also input the elevation of all inlets and the outlet to take into account the weight of the water body. Moreover, they want me to give a non-zero pressure value at the outlet since I am not under atmospheric pressure. Are they correct and am I wrong. (inlet velocities are 4 and 5 m/sec) differential in elevation is about 20 meter or 60 ft. Thank you for your help - A Boundary lost friend

 November 29, 2011, 17:23 #2 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,718 Rep Power: 106 The question is whether the head makes any difference. Do you have buoyancy, variable fluid properties or some fluid path which is affected by the head pressure? If so then better include it. If not then you can ignore it and your pressure field will be pressure relative to the local hydrostatic pressure. STAC likes this.

 November 29, 2011, 19:56 More Info #3 New Member   Claude Munger Poirier Join Date: Nov 2011 Posts: 3 Rep Power: 7 The water head at the outlet is 73 meters static pressure. There are no buoyancy and water flow is almost laminar not turbelent. My goal is only to check if there is a case where I may have cavitation nothing more. But they are stubbern with that outlet pressure because the penstock continue for almost 100 m before reaching atmospheric pressure. The outlet boundaries are the only concern for my results to be accepted. so If it is required I will impose the pressure but I think it is a mistake.

 November 30, 2011, 05:59 #4 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,718 Rep Power: 106 Why do you say the flow is "almost laminar"? For a 11ft diameter duct with water that would mean a flow of no faster than about 1 mm/s. Unless you are modelling these low flow velocities then your flow is turbulent. I never said to apply a pressure boundary condition. You apply what ever boundary conditions describe the flow best. What I was talking about is whether the hydrostatic head would offset your results or not.

 November 30, 2011, 11:26 #5 Member   Join Date: Dec 2009 Posts: 57 Rep Power: 9 If you want to model cavitation, your colleagues are right I think. The static pressure levels may be relative to reference and to eachother, but vapor pressure is an absolute value. If the static head at the inlets is higher, it will have to drop more to induce cavitation.

 November 30, 2011, 17:57 #6 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,718 Rep Power: 106 There is a big difference between checking whether cavitation is possible and modelling cavitation. Checking if cavitation is possible can be done with a simple model with no hydrostatic pressure. You just check whether the pressure is below the vapour pressure, with an offset for the local hydrostatic pressure. You do not need to model the hydrostatic pressure to do this. Modelling the cavitation is a different matter. Then you do need to include the hydrostatic pressure in the model. STAC likes this.

 December 1, 2011, 08:38 #7 Member   Join Date: Dec 2009 Posts: 57 Rep Power: 9 Obviously.

 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 dada1204 FLUENT 2 May 1, 2012 17:06 STAC Main CFD Forum 0 November 29, 2011 16:16 Fan Main CFD Forum 10 September 9, 2006 12:24 James Main CFD Forum 3 July 20, 2005 02:44 srijit goswami Main CFD Forum 3 January 27, 2001 08:28