# Stable Boundary Conditions

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

 May 15, 2010, 02:07 Stable Boundary Conditions #1 Member   Join Date: Feb 2010 Posts: 33 Rep Power: 9 Sponsored Links Hi, i'm trying to simulate a 1-1/5 stage turbine. I want to use a profile BC at inlet. But when I use T_tot, velocity x, velocity r, velocity theta, k and epsilon as an inlet profile and average static pressure as an outlet, the solver crashes: "Fatal bounds error detected variable: absolute pressure" how can i use the velocities? because when i use them, i cant specify total pressure at inlet (which i would also have as a profiel data) anymore... what is the way if i want to use T_tot, Velocity -x,-r,-theta, k and epsilon as an inlet profile BC?? Thank you very much!!!

 May 15, 2010, 07:01 #2 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,647 Rep Power: 105 Have you set the correct reference pressure? Is your boundary pressure correct relative to the reference pressure?

 May 15, 2010, 11:15 #3 Member   Join Date: Feb 2010 Posts: 33 Rep Power: 9 I set the reference pressure of the domain to "0 atm". For the inlet I can't specify any pressure (i'm using velocity u, r, theta). There is no option where I can specify for egsample total pressure at inlet. If I use unit velocity direction, than I can specify the pressure at inlet. but not withe the absolut values of the velocity.... At outlet I set 1.1 bar average static pressure... but the solver crashes due to the BC... What can I do?

 May 16, 2010, 12:37 #4 Senior Member     Attesz Join Date: Mar 2009 Location: Munich Posts: 364 Rep Power: 10 Hi, the referece pressure should be set near your operating pressures. I think 0 atm is low for a turbine. You should set at least 1 atm. The relative pressure will be (1.1bar-1atm) of course. And I think, you can not set total pressure and velocity at the inlet together, because the equations will be overconstrained.

 May 17, 2010, 09:35 #5 Member   Join Date: Feb 2010 Posts: 33 Rep Power: 9 so is this a correct way of setting BC: inlet: velocity -u, -r, -theta, T_tot, k, epsilon outlet: average static pressure ??? but when i use this, the solver crashes..... what is wrong?

 May 17, 2010, 09:38 #6 Senior Member     Attesz Join Date: Mar 2009 Location: Munich Posts: 364 Rep Power: 10 The crash can caused by many other problems! what is the error message?

 May 17, 2010, 09:45 #7 Member   Join Date: Feb 2010 Posts: 33 Rep Power: 9 i tried a lot of different BC setups with the same model, and they all worked.. now i wanted to use velocity components (from measurement) for the inlet. when i use velocity components, no pressure at inlet can be deffined anymore... 1st try: inlet: velocity components, t_tot, k, epsilon (profile BC) outlet: massflow -> error! 2nd try: inlet: velocity components, t_tot, k, epsilon (profile BC) outlet: average static pressure -> same error message: "Fatal bounds error detected variable: absolute pressure" what can i do if i want to use velocity componets at inlet? thank you

 May 17, 2010, 09:49 #8 Senior Member     Attesz Join Date: Mar 2009 Location: Munich Posts: 364 Rep Power: 10 The BC setting seems to be OK. Check your values, units etc. I have no more idea.

 May 17, 2010, 18:46 #9 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,647 Rep Power: 105 The error message is simply saying you are trying to get a negative absolute pressure somehow. Based on the sketchy information you have provided I have no idea where, but somewhere in your setup you are asking for a negative absolute pressure.

 May 18, 2010, 13:03 #10 Member   Join Date: Feb 2010 Posts: 33 Rep Power: 9 I set the reference pressure now to 1bar and the outlet average static pressure to 1.1-1=0.1 bar and it worked... but don't really know why... anyhow, thank you guys!

 May 18, 2010, 19:14 #11 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,647 Rep Power: 105 Numerical round-off. If you ran using double precision it probably would have worked. But the better solution is to set a reference pressure more representative of the flow average pressure, which is what you have done.

 May 18, 2010, 19:23 #12 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,647 Rep Power: 105 Trust me, the problem is caused by numerical round off leading to a convergence problem.

 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 Anindya Main CFD Forum 25 February 27, 2016 13:58 cfdmarkus OpenFOAM Running, Solving & CFD 16 November 14, 2011 05:44 Young CFX 5 October 6, 2008 23:17 Lionel S. Main CFD Forum 1 August 24, 2007 18:03 michele OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 2 July 15, 2005 04:15