Reverse flow far above outlet

swadejaxsun · January 31, 2018, 14:02

Hi,

I have a simple cylindrical tank with a pipe at the bottom to drain it. I'm controlling the mass flow and gravity is assisting. It's mostly water with air above it.

I'm getting fluid flow above my mass flow outlet above the liquid surface. This is causing waves/"bubbles" in the fluid surface of my simulation (lots of recirculation). I've tried resolving this using the extruder mesher, but it didn't help.

Why would here be movement in the air above the water due to a mass flow outlet?

fluid23 · February 1, 2018, 10:37

Sometimes using the mass flow inlet as an outlet can be sort of sketchy. The mass flow inlet is essentially varying back pressure to achieve your target flow rate. This could lead to a pulsing effect. How far did you extrude? You may have to go a little further. You might also try using the pressure outlet with mass flow specification option. That is also typically a little more gentle and quicker to converge.

swadejaxsun · February 1, 2018, 15:51

Thanks, Matt.

I extruded 20 inches and it still has these massive velocities within the air. It's actually pushing the water down faster than I'd expect. A non-physical response for sure, but it's just weird. I can run the same thing in Fluent and no issues like this.

That's what I initially wanted to do is have the pressure outlet, but I have a pump generating the mass flow and so I'm not sure what my set pressure would be.

fluid23 · February 1, 2018, 15:57

If you specify mass flow option then you can define a pressure range and target mass flow. The boundary condition will take care of finding the true pressure for you that gives you the mass flow you are dictating (assuming it can be found).

fluid23 · February 1, 2018, 15:57

It is basically like specifying a mass flow inlet as an outlet (i.e. negative mass flow) but is more stable and faster to converge.

swadejaxsun · February 1, 2018, 17:33

Ok, I thought I had to get that pressure value very precise. That's good to know.

I'm guessing the closer it is to the actual pressure the sooner the simulation will reach an equilibrium at the proper mass flow rate? Or does a wider range influence that more?

fluid23 · February 1, 2018, 17:35

I am not sure if that is the case. A wider range just gives more flexibility to the solver, but it also increases the likely hood of divergence. Whether or not it gets there 'faster', I am not sure.

swadejaxsun · February 1, 2018, 19:17

Ok so the problem now is that the mass flow is fluctuating using a pressure outlet. It reached the level I wanted it to, and then as the tank began to drain, the mass flow slowly began to drop and miss the target. Plenty of fluid left to keep it where I wanted it though.

swadejaxsun · February 2, 2018, 10:36

Nevermind, I got the mass flow inlet to work as an outlet.

If this isn't revelatory to you experts, it is to me, but thought I should document it.

If you're using multiphase flow, you need to define the volume mass fraction within the outlet BC. I was assuming that the system understood that since the outlet was interfaced with the water that it wouldn't try to move the air. Appears that that isn't so. It seemed redundant, but as it turns out necessary to get a stable flow out of the outlet.

Region > Boundaries > Outlet > Physics Values > Volume Fraction > Set to Composite > set value of 1 for phase at interface with outlet, and set other phase to 0.

fluid23 · February 2, 2018, 17:04

Good catch... I didn't even consider that.

That being said, I would still shy away from using a mass flow inlet as an outlet unless you can't get the pressure outlet w/ mass flow specification to work.

January 31, 2018, 14:02	Reverse flow far above outlet	#1
swadejaxsun New Member Join Date: Dec 2017 Posts: 12 Rep Power: 8	Hi, I have a simple cylindrical tank with a pipe at the bottom to drain it. I'm controlling the mass flow and gravity is assisting. It's mostly water with air above it. I'm getting fluid flow above my mass flow outlet above the liquid surface. This is causing waves/"bubbles" in the fluid surface of my simulation (lots of recirculation). I've tried resolving this using the extruder mesher, but it didn't help. Why would here be movement in the air above the water due to a mass flow outlet? Last edited by swadejaxsun; January 31, 2018 at 14:53. Reason: Better problem description

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Compressible flow, no data at the outlet	mireis	FLUENT	6	September 3, 2015 03:10
Temperature at a velocity/mass flow outlet	saisanthoshm88	CFX	1	July 8, 2014 19:35
Mass flow inlet and pressure outlet issue	nikhil	FLUENT	5	December 11, 2013 13:30
CAN'T CONVERGE WITH REVERSE FLOW AT OUTLET!	XIAOYI LI	FLUENT	11	September 14, 2012 17:43
CFDesign V11 -- Reverse flow at outlet	maruthiv	Autodesk Simulation CFD	1	June 17, 2011 10:38

February 1, 2018, 10:37		#2
fluid23 Senior Member Matt Join Date: Aug 2014 Posts: 947 Rep Power: 18	Sometimes using the mass flow inlet as an outlet can be sort of sketchy. The mass flow inlet is essentially varying back pressure to achieve your target flow rate. This could lead to a pulsing effect. How far did you extrude? You may have to go a little further. You might also try using the pressure outlet with mass flow specification option. That is also typically a little more gentle and quicker to converge.

February 1, 2018, 15:51		#3
swadejaxsun New Member Join Date: Dec 2017 Posts: 12 Rep Power: 8	Thanks, Matt. I extruded 20 inches and it still has these massive velocities within the air. It's actually pushing the water down faster than I'd expect. A non-physical response for sure, but it's just weird. I can run the same thing in Fluent and no issues like this. That's what I initially wanted to do is have the pressure outlet, but I have a pump generating the mass flow and so I'm not sure what my set pressure would be.

February 1, 2018, 15:57		#4
fluid23 Senior Member Matt Join Date: Aug 2014 Posts: 947 Rep Power: 18	If you specify mass flow option then you can define a pressure range and target mass flow. The boundary condition will take care of finding the true pressure for you that gives you the mass flow you are dictating (assuming it can be found).

February 1, 2018, 17:33		#6
swadejaxsun New Member Join Date: Dec 2017 Posts: 12 Rep Power: 8	Ok, I thought I had to get that pressure value very precise. That's good to know. I'm guessing the closer it is to the actual pressure the sooner the simulation will reach an equilibrium at the proper mass flow rate? Or does a wider range influence that more?

February 1, 2018, 17:35		#7
fluid23 Senior Member Matt Join Date: Aug 2014 Posts: 947 Rep Power: 18	I am not sure if that is the case. A wider range just gives more flexibility to the solver, but it also increases the likely hood of divergence. Whether or not it gets there 'faster', I am not sure.

February 1, 2018, 19:17		#8
swadejaxsun New Member Join Date: Dec 2017 Posts: 12 Rep Power: 8	Ok so the problem now is that the mass flow is fluctuating using a pressure outlet. It reached the level I wanted it to, and then as the tank began to drain, the mass flow slowly began to drop and miss the target. Plenty of fluid left to keep it where I wanted it though.

February 2, 2018, 10:36		#9
swadejaxsun New Member Join Date: Dec 2017 Posts: 12 Rep Power: 8	Nevermind, I got the mass flow inlet to work as an outlet. If this isn't revelatory to you experts, it is to me, but thought I should document it. If you're using multiphase flow, you need to define the volume mass fraction within the outlet BC. I was assuming that the system understood that since the outlet was interfaced with the water that it wouldn't try to move the air. Appears that that isn't so. It seemed redundant, but as it turns out necessary to get a stable flow out of the outlet. Region > Boundaries > Outlet > Physics Values > Volume Fraction > Set to Composite > set value of 1 for phase at interface with outlet, and set other phase to 0.

February 2, 2018, 17:04		#10
fluid23 Senior Member Matt Join Date: Aug 2014 Posts: 947 Rep Power: 18	Good catch... I didn't even consider that. That being said, I would still shy away from using a mass flow inlet as an outlet unless you can't get the pressure outlet w/ mass flow specification to work.