Stable Boundary Conditions

blackbody · May 15, 2010, 03:07

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!!!

ghorrocks · May 15, 2010, 08:01

Have you set the correct reference pressure? Is your boundary pressure correct relative to the reference pressure?

blackbody · May 15, 2010, 12:15

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?

Attesz · May 16, 2010, 13:37

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.

blackbody · May 17, 2010, 10:35

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?

Attesz · May 17, 2010, 10:38

The crash can caused by many other problems! what is the error message?

blackbody · May 17, 2010, 10:45

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

Attesz · May 17, 2010, 10:49

The BC setting seems to be OK. Check your values, units etc. I have no more idea.

ghorrocks · May 17, 2010, 19:46

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.

blackbody · May 18, 2010, 14:03

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!

ghorrocks · May 18, 2010, 20:14

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.

ghorrocks · May 18, 2010, 20:23

Trust me, the problem is caused by numerical round off leading to a convergence problem.

May 15, 2010, 03:07	Stable Boundary Conditions	#1
blackbody Member Join Date: Feb 2010 Posts: 33 Rep Power: 16	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!!!

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Impinging Jet Boundary Conditions	Anindya	Main CFD Forum	25	February 27, 2016 13:58
Problems with boundary conditions for a lowRekOmegaSST turbulence model	cfdmarkus	OpenFOAM Running, Solving & CFD	16	November 14, 2011 05:44
Concentric tube heat exchanger (Air-Water)	Young	CFX	5	October 7, 2008 00:17
Pressure boundary conditions	Lionel S.	Main CFD Forum	1	August 24, 2007 19:03
[Commercial meshers] Trimmed cell and embedded refinement mesh conversion issues	michele	OpenFOAM Meshing & Mesh Conversion	2	July 15, 2005 05:15

May 15, 2010, 08:01		#2
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,848 Rep Power: 144	Have you set the correct reference pressure? Is your boundary pressure correct relative to the reference pressure?

May 15, 2010, 12:15		#3
blackbody Member Join Date: Feb 2010 Posts: 33 Rep Power: 16	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, 13:37		#4
Attesz Senior Member Attesz Join Date: Mar 2009 Location: Munich Posts: 368 Rep Power: 17	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, 10:35		#5
blackbody Member Join Date: Feb 2010 Posts: 33 Rep Power: 16	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, 10:38		#6
Attesz Senior Member Attesz Join Date: Mar 2009 Location: Munich Posts: 368 Rep Power: 17	The crash can caused by many other problems! what is the error message?

May 17, 2010, 10:45		#7
blackbody Member Join Date: Feb 2010 Posts: 33 Rep Power: 16	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, 10:49		#8
Attesz Senior Member Attesz Join Date: Mar 2009 Location: Munich Posts: 368 Rep Power: 17	The BC setting seems to be OK. Check your values, units etc. I have no more idea.

May 17, 2010, 19:46		#9
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,848 Rep Power: 144	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, 14:03		#10
blackbody Member Join Date: Feb 2010 Posts: 33 Rep Power: 16	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, 20:14		#11
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,848 Rep Power: 144	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, 20:23		#12
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,848 Rep Power: 144	Trust me, the problem is caused by numerical round off leading to a convergence problem.