CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > FLUENT

Low pressure drop in duct compared to experimental values

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   July 20, 2021, 14:03
Default Low pressure drop in duct compared to experimental values
  #1
New Member
 
Kevin Williams
Join Date: Jan 2016
Location: United Kingdom
Posts: 25
Rep Power: 7
firestone9x is on a distinguished road
Hello all,

Experimental set-up:
I have a basic model that consists of a rectangular duct that has a sudden contraction to a smaller rectangular channel and then a sudden expansion back to the larger rectangular duct. The flow is driven by a centrifugal blower fan at the inlet and the velocity is measured after using flow straighteners. The outlet is exposed to the atmosphere and pressure is measured before contraction and after expansion using a differential pressure transducer.
Reynolds Number in the larger duct is around 1500 to 3900 and in the smaller duct it's around 2,200 to 11,600

CFD set-up:
I have replicated the same boundary conditions in Fluent with a velocity inlet and pressure outlet. I am also using a k-w SST model with a yplus of 5 for my 3D grid and performing a steady simulation with the coupled scheme.

In Fluent I get a pressure drop 3 times lower than the experiment and I am running out of ideas as to why this is happening.
Right now I think this might have something to do with the pressure measurement since the pressure drop decreases slightly if I swap out the blower fan for a smaller one.

I would appreciate some advice.

Thanks in advance.

Last edited by firestone9x; July 21, 2021 at 09:58.
firestone9x is offline   Reply With Quote

Old   July 20, 2021, 19:52
Default
  #2
Senior Member
 
Lorenzo Galieti
Join Date: Mar 2018
Posts: 209
Rep Power: 9
LoGaL is on a distinguished road
Reynolds number = 2000 and you are using a turbulence model. Sounds suspicious, is the flow turbulent or not?
LoGaL is offline   Reply With Quote

Old   July 21, 2021, 09:56
Default
  #3
New Member
 
Kevin Williams
Join Date: Jan 2016
Location: United Kingdom
Posts: 25
Rep Power: 7
firestone9x is on a distinguished road
Quote:
Originally Posted by LoGaL View Post
Reynolds number = 2000 and you are using a turbulence model. Sounds suspicious, is the flow turbulent or not?
Yes, you are definitely right. A laminar model should be used for low Re.
I should have been more specific, my apologies.

My Re range is from 2000 till 11,600. At the max Reynolds Number, the experimental pressure drop is still 1.7 times higher than CFD.
firestone9x is offline   Reply With Quote

Old   July 21, 2021, 11:01
Default
  #4
Senior Member
 
Lorenzo Galieti
Join Date: Mar 2018
Posts: 209
Rep Power: 9
LoGaL is on a distinguished road
Did you run without turbulence model?
LoGaL is offline   Reply With Quote

Old   July 21, 2021, 11:41
Default
  #5
New Member
 
Kevin Williams
Join Date: Jan 2016
Location: United Kingdom
Posts: 25
Rep Power: 7
firestone9x is on a distinguished road
Quote:
Originally Posted by LoGaL View Post
Did you run without turbulence model?
Yes, I ran a Laminar model and the pressure was just 7 Pa less when compared to the turbulence model but still 3 times lower than experimental data.
firestone9x is offline   Reply With Quote

Old   July 22, 2021, 04:19
Default
  #6
Senior Member
 
Lorenzo Galieti
Join Date: Mar 2018
Posts: 209
Rep Power: 9
LoGaL is on a distinguished road
So first thing, switch off that turbulence model, itís really horrible to use it at such low Re. Remember that laminar model is actually bare Navier Stokes equations, which already describe the turbulence physics. So for such mild to non existent turbulence levels, you donít need RANS.

After that, can you show me your mesh? Did you extend your inlet so as to have developed flow at the entrance of the region of interest?

Also, did you do mesh independence studies? Can you show me a plot?
LoGaL is offline   Reply With Quote

Old   July 24, 2021, 23:08
Default
  #7
New Member
 
Kevin Williams
Join Date: Jan 2016
Location: United Kingdom
Posts: 25
Rep Power: 7
firestone9x is on a distinguished road
Sorry for the late reply. I have switched off the turbulence models when running these simulations.

My inlet is 3.5D. You can see a picture of the mesh in the attachments labelled 'mesh-1' and 'mesh-2'.

As for the mesh independence study. Please see the attached image labelled 'mesh-independence.
Attached Images
File Type: jpg mesh-1.jpg (85.9 KB, 20 views)
File Type: jpg mesh-2.jpg (103.2 KB, 16 views)
File Type: jpg mesh-independence.jpg (44.7 KB, 12 views)
firestone9x is offline   Reply With Quote

Old   July 26, 2021, 15:36
Default
  #8
Senior Member
 
Lorenzo Galieti
Join Date: Mar 2018
Posts: 209
Rep Power: 9
LoGaL is on a distinguished road
Hi, if that is the finest mesh, out of which you are getting the pressure drop, then I really think it is a problem of mesh independence because itís coarse, especially at the two ends of the small channel ( where you will have a very large velocity gradient) and even in the small channel itself
LoGaL is offline   Reply With Quote

Old   July 27, 2021, 14:59
Default
  #9
New Member
 
Kevin Williams
Join Date: Jan 2016
Location: United Kingdom
Posts: 25
Rep Power: 7
firestone9x is on a distinguished road
Good point, I went back to my mesh and refined the inlet and outlet ends of the small channel as you mentioned. The pressure drop didn't seem to change.

From the experiment side, I replaced the small CFM blower with one that had twice the CFM and noticed that my pressure drop readings were now 100 Pa higher. In my setup, I'm measuring the differential pressure across the small channel with two pitot tubes and this should remain the same if I swap fans. In both tests, the velocity is kept constant.

Is there something I am missing out on?
firestone9x is offline   Reply With Quote

Old   July 28, 2021, 08:00
Default
  #10
Senior Member
 
Lorenzo Galieti
Join Date: Mar 2018
Posts: 209
Rep Power: 9
LoGaL is on a distinguished road
No man, you misunderstand me, the mesh you are showing is bad so I donít expect anything good to come out of it. All those sharp aspect ratio transitions, the overall coarseness. Is the boundary layer solved? Did you check it? You should really mesh work on that.
Other than that, I donít see what could go wrong with a laminar model, an inlet and an outlet. Which boundary conditions are you imposing? How are you obtaining the pressure drop (area average total pressure?)
LoGaL is offline   Reply With Quote

Old   July 28, 2021, 13:53
Default
  #11
New Member
 
Kevin Williams
Join Date: Jan 2016
Location: United Kingdom
Posts: 25
Rep Power: 7
firestone9x is on a distinguished road
Okay. I'll work on improving the mesh based on your suggestions.
I do have inflation layers with a Yplus of 1.5 to resolve the boundary layer. However, I will change my first layer thickness to see if this affects the solution.

As for BCs; I have a velocity inlet (experimental measurements with a hotwire) and a pressure outlet at 0 Pa. I used the area-weighted average of 'static pressure' at the inlet to find my pressure drop.
firestone9x is offline   Reply With Quote

Old   July 28, 2021, 15:52
Default
  #12
Senior Member
 
Lorenzo Galieti
Join Date: Mar 2018
Posts: 209
Rep Power: 9
LoGaL is on a distinguished road
You should measure total pressure, non static one. Try changing that and maybe it works despite the mesh .
LoGaL is offline   Reply With Quote

Old   July 29, 2021, 21:10
Default
  #13
New Member
 
Kevin Williams
Join Date: Jan 2016
Location: United Kingdom
Posts: 25
Rep Power: 7
firestone9x is on a distinguished road
The difference between total and static pressure was negligible, unfortunately.
I think any further mesh refinement will not change the solution.

However, I changed my anemometer and recorded a higher velocity reading and now my CFD pressure data is close to experiments.
Now there is one pending question, which pressure readings are right since the small CFM fan is close to the CFD data but the larger one is almost twice the pressure drop of the smaller CFM fan even though the velocity is the same.

Is there a special BC that has to be implemented in CFD?
firestone9x is offline   Reply With Quote

Old   July 30, 2021, 07:49
Default
  #14
Senior Member
 
Lorenzo Galieti
Join Date: Mar 2018
Posts: 209
Rep Power: 9
LoGaL is on a distinguished road
Hold on, can you explain better?

You tried two different fans pushing air in the duct. At the inlet of the duct you measured velocity with an anemometer. You also measured the pressure before and after the duct with some pressure probes.

You changed anemometer and now CFD and exp. data match for the small fan

You are saying that with the big fan CFD and exp. data do not match for the big fan.

What do you mean when you say the velocity is the same?
LoGaL is offline   Reply With Quote

Old   August 2, 2021, 23:18
Default
  #15
New Member
 
Kevin Williams
Join Date: Jan 2016
Location: United Kingdom
Posts: 25
Rep Power: 7
firestone9x is on a distinguished road
I measure the velocity at the inlet of the duct.
And the differential pressure is measured before and after the channel with two pitot tubes connected to a differential pressure transducer.

Now, I have two anemometers, the new one reads a higher velocity than the old one. So the higher velocity inputted in CFD will result in a higher differential pressure that matches with the experimental data for the small fan.

However, when I swap out the small fan with a big fan, the experimental differential pressure is higher than the small fan differential pressure.
When I said the same velocity I was referring to maintaining the same flow velocity at the inlet of the duct for both fans which should result in the same static pressure.
firestone9x is offline   Reply With Quote

Old   August 4, 2021, 05:55
Default
  #16
Senior Member
 
Lorenzo Galieti
Join Date: Mar 2018
Posts: 209
Rep Power: 9
LoGaL is on a distinguished road
I don't get how a larger fan would give the same velocity and the same static pressure. If the duct area stays the same, I would expect either the velocity or pressure to be higher
LoGaL is offline   Reply With Quote

Old   August 4, 2021, 15:05
Default
  #17
New Member
 
Kevin Williams
Join Date: Jan 2016
Location: United Kingdom
Posts: 25
Rep Power: 7
firestone9x is on a distinguished road
Those were my exact thoughts.
Unless the turbulence intensity at the inlet is different due to larger and different blade geometry. But I have flow straighteners before my anemometer in all test cases.
firestone9x is offline   Reply With Quote

Old   August 4, 2021, 19:27
Default
  #18
Senior Member
 
Lorenzo Galieti
Join Date: Mar 2018
Posts: 209
Rep Power: 9
LoGaL is on a distinguished road
I was wondering whether the absolute pressure value stays the same inside the duct? Not the differential one. This might make sense to me, because this larger fan has to force more mass flow in (and also provide a different pressure jump) which for the same duct means more absolute pressure. This in turn raises the density of the flow, which increases the turbulence levels.

Is the discharge pressure of the duct known? Ambient perhaps? Do you know any absolute pressure value? It is true that for low Mach flow (ie incompressible) differential pressures matters, but you need the correct density value, which in turn depends from absolute pressure value.

Basically this larger fan must change something in the inflow conditions in your exp setup, and if we donít know what is changing, we wonít reproduce the results
LoGaL is offline   Reply With Quote

Old   August 5, 2021, 11:31
Default
  #19
New Member
 
Kevin Williams
Join Date: Jan 2016
Location: United Kingdom
Posts: 25
Rep Power: 7
firestone9x is on a distinguished road
I think you might be right. Since the density is increasing, the absolute pressure would increase and therefore I will need to calculate a gauge pressure in addition to the velocity value at the inlet.
However, I'm surprised that the flow would be compressible at such low velocities but then again the larger fan is forcing a lot of air through a small channel.

Yes, the discharge pressure is measured to be atmospheric.

I would need to get an absolute pressure sensor to get those values and then repeat the simulations.
firestone9x is offline   Reply With Quote

Old   August 5, 2021, 12:45
Default
  #20
Senior Member
 
Lorenzo Galieti
Join Date: Mar 2018
Posts: 209
Rep Power: 9
LoGaL is on a distinguished road
If your velocity does not change with the larger fan, there has to be higher pressure or I canít see how you could pass more air 🥲.
LoGaL is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

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 Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Wind tunnel Boundary Conditions in Fluent metmet FLUENT 6 October 30, 2019 12:23
OpenFOAM - cyclicAMI Pressure drop result variation Vishsel OpenFOAM 0 May 31, 2019 02:47
Computed Pressure Drop is lower than experimental data Ash Kot FLUENT 2 May 17, 2017 09:41
How to study pressure drop of continous phase in VOF model sajeesh FLUENT 4 February 5, 2014 22:01
Hydrostatic pressure in 2-phase flow modeling (long) DS & HB Main CFD Forum 0 January 8, 2000 15:00


All times are GMT -4. The time now is 05:17.