-140 kPa pressure, how is it possible?

Water · November 14, 2016, 18:55

Hi everyone,

I am modeling an open channel flow using Fluent. When I plot floor pressure on a chart, one location shows -140 kPa pressure. How can pressure be less than absolute 0 pressure? The channel bed is 20 m wide, and I use 0.5m tet mesh on the bed.

Thanks!

CFD-fellow · November 15, 2016, 23:24

Hi
According to my experience in turbo machinery modeling when the water tends to cavitate at the suction side of blade, if u dont activate cavitation and multiphase simulation then the pressure in that part is unreal.
I think fluent and other codes are not limited by absolute pressure 0, so the codes dont know reality.
Anyway in your simulation I think it is because of convergence problem. Check velocity contour in that part and see if the velocity is unnaturally high in that place.

Kushal Puri · November 16, 2016, 09:20

What boundary conditions and models u are using.

Water · November 20, 2016, 06:05

Sorry for the late reply. I use VOF model, velocity inlet for inlet BC and pressure outlet for outlet BC.

CFD -Fellow: the velocity on that edge is the highest within the channel, and I expected the pressure is about -80 to -100 kPa only.

Kushal Puri · November 20, 2016, 08:44

What is ur operating pressure and operating density boundary condition

Water · November 21, 2016, 00:52

I use atmospheric pressure 101.3 KPa and air density 1.225 kg/m^3

LuckyTran · November 21, 2016, 13:59

There is a default limiter on Minimum Absolute Pressure of 1 pascal. Unless you see this error message, then the absolute pressure isn't less than 0.

Why don't you just plot the absolute pressure?

Pay attention to the reference location. You are specifying the operating pressure and operating density at that location. Is gravity enabled? I think it is because otherwise there is no operating density.

The pressure plot display in Fluent does not include the hydrostatic component (because Fluent redefines pressure based on the reference pressure and density). As you go down in elevation, the hydrostatic component adds (but it is missing in the display). If you wanted absolute pressure, you should have plotted it.

Water · November 22, 2016, 00:36

Hi Lucky Tran,

Thanks for your comment. I specified reference pressure (101.3 kPa) at the default location (x,y,z = 0), and this point is actually on the channel bed, not in the atmosphere, this may be the reason why I got the wrong value of pressure.

Kushal Puri · November 23, 2016, 12:22

Quote:

Originally Posted by Water

I use atmospheric pressure 101.3 KPa and air density 1.225 kg/m^3

You need to define the operating density of the working fluid (like for water 998 at desired temperature)

Water · November 23, 2016, 21:01

Why do we need to use water density for operating density? I think we always use the lighter fluid density and in this case it's air density.

November 14, 2016, 18:55	-140 kPa pressure, how is it possible?	#1
Water New Member James N Join Date: Nov 2016 Posts: 14 Rep Power: 9	Hi everyone, I am modeling an open channel flow using Fluent. When I plot floor pressure on a chart, one location shows -140 kPa pressure. How can pressure be less than absolute 0 pressure? The channel bed is 20 m wide, and I use 0.5m tet mesh on the bed. Thanks! Last edited by Water; November 14, 2016 at 20:07.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Wind tunnel Boundary Conditions in Fluent	metmet	FLUENT	6	October 30, 2019 12:23
Periodic flow using Cyclic - comparison with Fluent	nusivares	OpenFOAM Running, Solving & CFD	30	December 12, 2017 05:35
Outlet pressure	aja1345	FLUENT	5	August 18, 2015 11:02
Calculation of the Governing Equations	Mihail	CFX	7	September 7, 2014 06:27
Unsteady pressure differential between inlet and outlet of the pipe for single phase	joshi20h	FLUENT	0	September 26, 2012 12:41

November 15, 2016, 23:24		#2
CFD-fellow Senior Member Behrooz Jamshidi Join Date: Apr 2013 Posts: 110 Rep Power: 13	Hi According to my experience in turbo machinery modeling when the water tends to cavitate at the suction side of blade, if u dont activate cavitation and multiphase simulation then the pressure in that part is unreal. I think fluent and other codes are not limited by absolute pressure 0, so the codes dont know reality. Anyway in your simulation I think it is because of convergence problem. Check velocity contour in that part and see if the velocity is unnaturally high in that place.

November 16, 2016, 09:20		#3
Kushal Puri Senior Member Kushal Puri Join Date: Nov 2013 Posts: 182 Rep Power: 12	What boundary conditions and models u are using.

November 20, 2016, 06:05		#4
Water New Member James N Join Date: Nov 2016 Posts: 14 Rep Power: 9	Sorry for the late reply. I use VOF model, velocity inlet for inlet BC and pressure outlet for outlet BC. CFD -Fellow: the velocity on that edge is the highest within the channel, and I expected the pressure is about -80 to -100 kPa only.

November 20, 2016, 08:44		#5
Kushal Puri Senior Member Kushal Puri Join Date: Nov 2013 Posts: 182 Rep Power: 12	What is ur operating pressure and operating density boundary condition

November 21, 2016, 00:52		#6
Water New Member James N Join Date: Nov 2016 Posts: 14 Rep Power: 9	I use atmospheric pressure 101.3 KPa and air density 1.225 kg/m^3

November 21, 2016, 13:59		#7
LuckyTran Senior Member Lucky Join Date: Apr 2011 Location: Orlando, FL USA Posts: 5,674 Rep Power: 66	There is a default limiter on Minimum Absolute Pressure of 1 pascal. Unless you see this error message, then the absolute pressure isn't less than 0. Why don't you just plot the absolute pressure? Pay attention to the reference location. You are specifying the operating pressure and operating density at that location. Is gravity enabled? I think it is because otherwise there is no operating density. The pressure plot display in Fluent does not include the hydrostatic component (because Fluent redefines pressure based on the reference pressure and density). As you go down in elevation, the hydrostatic component adds (but it is missing in the display). If you wanted absolute pressure, you should have plotted it.

November 22, 2016, 00:36		#8
Water New Member James N Join Date: Nov 2016 Posts: 14 Rep Power: 9	Hi Lucky Tran, Thanks for your comment. I specified reference pressure (101.3 kPa) at the default location (x,y,z = 0), and this point is actually on the channel bed, not in the atmosphere, this may be the reason why I got the wrong value of pressure.

November 23, 2016, 21:01		#10
Water New Member James N Join Date: Nov 2016 Posts: 14 Rep Power: 9	Why do we need to use water density for operating density? I think we always use the lighter fluid density and in this case it's air density.