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

Setting Gravity for a VERTICAL flow

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 22, 2017, 09:34
Default Setting Gravity for a VERTICAL flow
  #1
New Member
 
Leo
Join Date: Jul 2014
Posts: 13
Rep Power: 11
LeandroGSS is on a distinguished road
Hello everyone,

Keeping it short and simple: How do I consider gravity in a CFX simulation? I have an one-phase-flow but it is strong affect by quote differences, it means, the flow is vertical (from the bottom to the top - which in my flow means the gravity would be -9.81 in the Y direction).

Going further into details:
I had of course searched for an answer last week and I read about activating "buoyancy effects" and so I have been doing this whole week. Now I was checking for plausibility and my flow is not plausible at all. I mean, changing the value of gravity acceleration in the buoyancy conditions makes no difference in my flow. Even considering gravity in + ou - Y or X-Axis or changing its value to 2, 10, 100 m/s² makes absolute no difference. So Buoyancy is not the point here.

Thank you in advance!
LeandroGSS is offline   Reply With Quote

Old   February 22, 2017, 10:42
Default
  #2
New Member
 
Leo
Join Date: Jul 2014
Posts: 13
Rep Power: 11
LeandroGSS is on a distinguished road
Quick update: I've just created a Subdomain and there I have defined a "Momentum Source" equal to rho*g (in my case 997 kg m-3 * 9.81 m s-1 = 9780 kg m-2 s-2).
Now my results make no sense, streamlines and velocity on plane seem very weird.
Was it a wrong guess?
LeandroGSS is offline   Reply With Quote

Old   February 22, 2017, 17:38
Default
  #3
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,665
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
What does gravity do in your flow? Do you have pressure dependent material properties (such as density a function of pressure)? You have stated it is a single phase flow so you do not have free surface effects.
ghorrocks is offline   Reply With Quote

Old   February 22, 2017, 21:37
Default
  #4
New Member
 
Leo
Join Date: Jul 2014
Posts: 13
Rep Power: 11
LeandroGSS is on a distinguished road
Hello Glenn, thanks for the attention.

My flow hast a strong elevation change (Delta H).
If we consider the Bernoulli's equation, I wonder if and how CFX considers the term "rho*g*Delta h" from Bernoulli when solving my case.

Giving möge details: I have one inlet (in the bottom), which I define with a known mass flow, and a single Outlet (in the top), which a define with a Static Pressure = 0 (Opening Pressure and Dirn).
LeandroGSS is offline   Reply With Quote

Old   February 22, 2017, 22:28
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,665
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Unless the pressure affects the fluid then you should not model this with buoyancy. This is why the results you have been getting so far are weird. You should model this with no gravity and in post-processing add a hydrostatic pressure to the results (which will just be a linear function against height). You will need to account for the hydrostatic head in any pressure boundaries you apply.

So in your case do the simulation with no gravity and use the outlet at the top with pressure =0. In post-processing define a variable which is just the hydrostatic pressure and add it to the pressure from the simulation result.
ghorrocks is offline   Reply With Quote

Old   February 24, 2017, 05:54
Default
  #6
New Member
 
Leo
Join Date: Jul 2014
Posts: 13
Rep Power: 11
LeandroGSS is on a distinguished road
Hello,

Thank you.
I did what you recommended in post-processing and it worked pretty well.

What seems a little bit "not intuitive" for me is that the gravity will have no effect at all in the internal flow, but only in the total pressure of the system (which is added just in the end, after the simulation).

I attached a figure to this reply. There you see a rough sketch of my system. It is like a cuboid, inlet in the bottom, outlet at the top. So, it means, doesn't matter how we stand this cuboid in the ground, it will have absolutely no effect in the internal flow??? (for example, what if the gravity in this picture was not in -y but instead in + or -z ?).
Attached Images
File Type: png Model.png (31.5 KB, 73 views)
LeandroGSS is offline   Reply With Quote

Old   February 24, 2017, 06:50
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,665
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Be careful with the word "total pressure". In high speed flows this is defined as the static pressure plus the dynamic pressure. A better description for your case is absolute pressure.

The gravity direction will affect the pressure difference between the inlet and outlet as the height difference changes. Then the internal flow is just driven by the pressure difference.
ghorrocks is offline   Reply With Quote

Old   February 24, 2017, 07:45
Default
  #8
New Member
 
Leo
Join Date: Jul 2014
Posts: 13
Rep Power: 11
LeandroGSS is on a distinguished road
Quote:
"Then the internal flow is just driven by the pressure difference."
Ok, I definitely agree with that.
But what if am I modeling my boundaries with mass flow rate? Let's imagine two situations (for the picture above):

A: horizontal flow (gravity z axis)
Inlet: 0.01 L/s
Outlet: Opening Pressure 0 Pa

B: vertical flow (gravity -y axis)
Inlet (bottom): also 0.01 L/s
Outlet: Also Opening Pressure 0 Pa (because this outlet is set on the top)

So, is it right that both flows look exactly the same, or am I modeling my boundaries wrong?
LeandroGSS is offline   Reply With Quote

Old   February 25, 2017, 06:48
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,665
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
There will be a small difference between your two cases due to the hydrostatic pressure difference across the pressure boundary. But it will be a small difference, overall the two simulations will be very similar.
ghorrocks is offline   Reply With Quote

Old   February 28, 2017, 03:55
Default
  #10
New Member
 
Leo
Join Date: Jul 2014
Posts: 13
Rep Power: 11
LeandroGSS is on a distinguished road
Thank you.
So, just correct me if I am wrong: I can model my boundaries the way I am doing, with mass flow at the inlet and opening 0 Pa at the outlet, and since two simulations are very similar, I don't need to worry about anything.

Thank you for your help.
LeandroGSS is offline   Reply With Quote

Old   February 28, 2017, 05:26
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,665
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
I would not say "I don't need to worry about anything". There is always something to worry about

You should check that this assumption is valid. Do a sensitivity check on it and see if it makes any difference. If it makes no difference then you can stop worrying.
ghorrocks is offline   Reply With Quote

Old   March 6, 2017, 04:55
Default
  #12
New Member
 
Leo
Join Date: Jul 2014
Posts: 13
Rep Power: 11
LeandroGSS is on a distinguished road
Alright!
So, I did a sensitivity check and it's true, it makes apparently no difference.
Thank you so much Ghorrocks!
LeandroGSS is offline   Reply With Quote

Old   May 10, 2019, 19:08
Unhappy
  #13
New Member
 
Newfoundland and Labrador
Join Date: May 2019
Posts: 1
Rep Power: 0
mizanurpe is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Unless the pressure affects the fluid then you should not model this with buoyancy. This is why the results you have been getting so far are weird. You should model this with no gravity and in post-processing add a hydrostatic pressure to the results (which will just be a linear function against height). You will need to account for the hydrostatic head in any pressure boundaries you apply.

So in your case do the simulation with no gravity and use the outlet at the top with pressure =0. In post-processing define a variable which is just the hydrostatic pressure and add it to the pressure from the simulation result.
would you please tell me how can I add the gravity after simulation? I am facing same problem the gravity effect is not working.
mizanurpe is offline   Reply With Quote

Old   May 11, 2019, 06:35
Default
  #14
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,665
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
hydrostatic pressure is simply density*g*height, so you can easily add that in post processing if you like. But you can only do this if the free surface is level.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks 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
Vertical Pipe water flow Goutam FLUENT 0 April 30, 2014 09:25
Laminar vertical flow with interFoam idefix OpenFOAM Running, Solving & CFD 4 February 19, 2014 03:38
coupling vof with single phase flow and gravity term alame005 Main CFD Forum 7 August 6, 2013 12:02
coupling vof with single phase flow and gravity term alame005 Main CFD Forum 0 August 2, 2013 15:37
Cells with t below lower limit Purushothama Siemens 2 May 31, 2010 22:58


All times are GMT -4. The time now is 04:07.