Negative pressure problem

FrankW · July 7, 2014, 03:07

Hallo hwangpo,

i don't know if its correct but in a model with your dimmensons i would use gravity in the simulation. If think its a gravity driven flow. An then you will get the right pressure without any factors.
And yes, you can get cavitation on such flows

hwangpo · July 7, 2014, 03:47

Quote:

Originally Posted by FrankW

Hallo hwangpo,

i don't know if its correct but in a model with your dimmensons i would use gravity in the simulation. If think its a gravity driven flow. An then you will get the right pressure without any factors.
And yes, you can get cavitation on such flows

I set the pressure inlet in which I think gravity is considered. Actually i do not know how can i model what u said, using buoyancy model or something? Let me know if i got u wrong

thank u

FrankW · July 7, 2014, 04:20

Look at the tutorial "Free surface flow over a bump". You don't need use 2 fluids but you can use the CEL expressions for water. Also you have to adapt the coordinate expressions. In your case z-axis.

hwangpo · July 7, 2014, 05:08

alright
thank u
im looking into that.

ghorrocks · July 7, 2014, 05:59

Gravity will only have an effect if something is a function of gravity. That is usually a variable density, either as multiphase, or density a function of temperature for buoyant flows. If nothing is a function of it then adding gravity will do nothing.

Blanco · July 7, 2014, 06:13

From my understandings you have imposed a pressure on your opening inlet boundaries and you have used that b.c. to pressurize the fluid "as if" the gravity was turned on. If I think of a static fluid basin and I look at the pressure at the bottom of it, then you have p=ro*g*h if gravity is turned on and atmospheric pressure is acting on the fluid free surface, p=p1 if gravity is turned off and a pressure boundary (e.g. opening b.c.) is imposed on the free surface, and in order to do thing correctly that b.c. should be p1=ro*g*h as you did.

My concern is related to the outlet...you have imposed 0 relative pressure there, so atmospheric absolute pressure is acting on the outlet. Is this boundary consistent with your experimental setup, or do you have a basin at the exit of the pipe? 2nd, is the outlet velocity coming from CFD comparable with the experimental velocity?

ghorrocks · July 7, 2014, 06:34

If you have activated buoyancy the pressure variable includes the static head. As long as density is constant then you do not need to account for static head.

And this is why, unless you are running a multiphase simulation or density is not constant then you should not activate gravity. In a single phase constant density flow gravity does not contribute so do not include it.

hwangpo · July 7, 2014, 07:05

thank you for your nice suggestions and insightful comments.

I did not use the buoyancy option in the model and set the inlet as opening boundary with a constant pressure which is calculated from water head difference between water surface and outlet centerline. BTW, the outlet B.C. is static pressure=0. The relative pressure is 1 atm, so the outlet is kind of outflow or something. Is this right?

Please let me know if I made mistakes.

FrankW · July 7, 2014, 08:58

Quote:

Originally Posted by ghorrocks

Gravity will only have an effect if something is a function of gravity. That is usually a variable density, either as multiphase, or density a function of temperature for buoyant flows. If nothing is a function of it then adding gravity will do nothing.

Right, i was wrong.

Blanco · July 7, 2014, 09:35

Yes the outlet is correctly set if you have a pipe that is connected to the ambient without any basin. If you have your liquid that is coming out from the pipe like a waterfall than it is ok. If you have something that will oppose resistance to the flow (e.g. a basin that acts like a reservoir) than you have to include it, and it will increase the pressure in the pipe (maybe you won't get cavitation anymore).

Bak16 · October 25, 2023, 09:15

Hello, I have the same problem as you and refining the mesh didn't help. Did you manage to solve this eventually? There are just a couple of elements with this negative pressure and I initially use incompressible flow and the solver can deal with it. However, when I add a compressible phase to actually simulate the cavitation the solver crashes, and I think its because of this negative pressure.

ghorrocks · October 25, 2023, 18:02

Yes, a negative pressure is numerically OK in incompressible flow, but will cause a crash in compressible flow.

Are you getting negative absolute pressure or negative pressure? I assume you mean absolute pressure.

If you are confident your simulation is accurate, you are getting a negative absolute pressure and your fluid is a liquid then it means the liquid would cavitate and you need to add a cavitation model.

Or is your fluid a gas and you are getting negative absolute pressures?

Bak16 · October 25, 2023, 20:56

Yes it is an absolute pressure (my reference pressure is 0 Pa). I have a pure incompressible liquid (Water) and I get negative pressures. But the next step is to simulate cavitation where I need to add the vapour phase as well. I fixed the problem by increasing some fillet radius to make the geometry smoother and now there is no negative pressure. Mesh refinement didn't seem to do much, only the improvement of the geometry helped. Thank you so much for your reply.

October 25, 2023, 18:02		#32
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	Yes, a negative pressure is numerically OK in incompressible flow, but will cause a crash in compressible flow. Are you getting negative absolute pressure or negative pressure? I assume you mean absolute pressure. If you are confident your simulation is accurate, you are getting a negative absolute pressure and your fluid is a liquid then it means the liquid would cavitate and you need to add a cavitation model. Or is your fluid a gas and you are getting negative absolute pressures? __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
[blockMesh] non-orthogonal faces and incorrect orientation?	nennbs	OpenFOAM Meshing & Mesh Conversion	7	April 17, 2013 05:42
Negative Pressure in H2 gas flow and other physical interrogation	FloMol	ANSYS	2	April 9, 2012 19:57
[blockMesh] error message with modeling a cube with a hold at the center	hsingtzu	OpenFOAM Meshing & Mesh Conversion	2	March 14, 2012 09:56
negative pressure	mAx	FLUENT	0	January 25, 2006 14:31
a problem in calculating pressure drop in Fluent?	yu chun	FLUENT	1	May 18, 2004 03:40

July 7, 2014, 03:07		#21
FrankW Member Frank Weise Join Date: Mar 2009 Location: Germany Posts: 55 Rep Power: 17	Hallo hwangpo, i don't know if its correct but in a model with your dimmensons i would use gravity in the simulation. If think its a gravity driven flow. An then you will get the right pressure without any factors. And yes, you can get cavitation on such flows

July 7, 2014, 04:20		#23
FrankW Member Frank Weise Join Date: Mar 2009 Location: Germany Posts: 55 Rep Power: 17	Look at the tutorial "Free surface flow over a bump". You don't need use 2 fluids but you can use the CEL expressions for water. Also you have to adapt the coordinate expressions. In your case z-axis.

July 7, 2014, 05:08		#24
hwangpo Member Ben B. Huang Join Date: Oct 2012 Posts: 54 Rep Power: 13	alright thank u im looking into that.

July 7, 2014, 05:59		#25
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	Gravity will only have an effect if something is a function of gravity. That is usually a variable density, either as multiphase, or density a function of temperature for buoyant flows. If nothing is a function of it then adding gravity will do nothing.

July 7, 2014, 06:13		#26
Blanco Senior Member Blanco Join Date: Mar 2009 Location: Torino, Italy Posts: 193 Rep Power: 17	From my understandings you have imposed a pressure on your opening inlet boundaries and you have used that b.c. to pressurize the fluid "as if" the gravity was turned on. If I think of a static fluid basin and I look at the pressure at the bottom of it, then you have p=rogh if gravity is turned on and atmospheric pressure is acting on the fluid free surface, p=p1 if gravity is turned off and a pressure boundary (e.g. opening b.c.) is imposed on the free surface, and in order to do thing correctly that b.c. should be p1=rogh as you did. My concern is related to the outlet...you have imposed 0 relative pressure there, so atmospheric absolute pressure is acting on the outlet. Is this boundary consistent with your experimental setup, or do you have a basin at the exit of the pipe? 2nd, is the outlet velocity coming from CFD comparable with the experimental velocity?

July 7, 2014, 06:34		#27
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	If you have activated buoyancy the pressure variable includes the static head. As long as density is constant then you do not need to account for static head. And this is why, unless you are running a multiphase simulation or density is not constant then you should not activate gravity. In a single phase constant density flow gravity does not contribute so do not include it.

July 7, 2014, 07:05		#28
hwangpo Member Ben B. Huang Join Date: Oct 2012 Posts: 54 Rep Power: 13	thank you for your nice suggestions and insightful comments. I did not use the buoyancy option in the model and set the inlet as opening boundary with a constant pressure which is calculated from water head difference between water surface and outlet centerline. BTW, the outlet B.C. is static pressure=0. The relative pressure is 1 atm, so the outlet is kind of outflow or something. Is this right? Please let me know if I made mistakes.

July 7, 2014, 09:35		#30
Blanco Senior Member Blanco Join Date: Mar 2009 Location: Torino, Italy Posts: 193 Rep Power: 17	Yes the outlet is correctly set if you have a pipe that is connected to the ambient without any basin. If you have your liquid that is coming out from the pipe like a waterfall than it is ok. If you have something that will oppose resistance to the flow (e.g. a basin that acts like a reservoir) than you have to include it, and it will increase the pressure in the pipe (maybe you won't get cavitation anymore).

October 25, 2023, 09:15		#31
Bak16 New Member Join Date: Jul 2023 Posts: 5 Rep Power: 2	Hello, I have the same problem as you and refining the mesh didn't help. Did you manage to solve this eventually? There are just a couple of elements with this negative pressure and I initially use incompressible flow and the solver can deal with it. However, when I add a compressible phase to actually simulate the cavitation the solver crashes, and I think its because of this negative pressure.

October 25, 2023, 20:56		#33
Bak16 New Member Join Date: Jul 2023 Posts: 5 Rep Power: 2	Yes it is an absolute pressure (my reference pressure is 0 Pa). I have a pure incompressible liquid (Water) and I get negative pressures. But the next step is to simulate cavitation where I need to add the vapour phase as well. I fixed the problem by increasing some fillet radius to make the geometry smoother and now there is no negative pressure. Mesh refinement didn't seem to do much, only the improvement of the geometry helped. Thank you so much for your reply.