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

Gravity problem in CFX

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

Like Tree1Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   January 28, 2011, 01:08
Default Gravity problem in CFX
  #1
New Member
 
Ricky Chen
Join Date: Jan 2011
Location: Vancouver
Posts: 17
Rep Power: 6
ssbear is on a distinguished road
Hi everyone,

I'm new to CFD and I'm now trying to make a water intake model. In my model, the inlet is set to be 3 m/s (normal speed) and the outlet is also set to be 3m/s (normal speed). For the gravity effect, I used two ways to simulate it:

1. free surface model as shown in tutorial 7
2. single-phase model with sub-domain to simulate the gravity (general momentum source)

Now the resutls of both ways are quite different and I'm just wondering which one makes more sense ?

Thanks in advance for any advice!!
Attached Images
File Type: jpg Model.jpg (40.2 KB, 46 views)
File Type: jpg free surface .jpg (46.2 KB, 80 views)
File Type: jpg single phase.jpg (82.5 KB, 65 views)
ssbear is offline   Reply With Quote

Old   January 28, 2011, 04:21
Default
  #2
Senior Member
 
Matthias Voß
Join Date: Mar 2009
Location: Berlin, Germany
Posts: 446
Rep Power: 11
mvoss is on a distinguished road
hi,
do you want to compare multiphase vs. singlephase?

Btw. you can set the gravity without any subdomain by just setting the vector properly (look up gravity in the help).

neewbie
mvoss is offline   Reply With Quote

Old   January 28, 2011, 06:29
Default
  #3
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
You model gravity using the gravity option. Forget about source terms, it is already in there, you just need to activate it.

Your boundary conditions are probably poorly defined as pressure is not set anywhere. You need to set a pressure somewhere.
ghorrocks is offline   Reply With Quote

Old   January 29, 2011, 01:42
Default
  #4
New Member
 
Ricky Chen
Join Date: Jan 2011
Location: Vancouver
Posts: 17
Rep Power: 6
ssbear is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
You model gravity using the gravity option. Forget about source terms, it is already in there, you just need to activate it.

Your boundary conditions are probably poorly defined as pressure is not set anywhere. You need to set a pressure somewhere.
Quote:
Originally Posted by neewbie View Post
hi,
do you want to compare multiphase vs. singlephase?

Btw. you can set the gravity without any subdomain by just setting the vector properly (look up gravity in the help).

neewbie
neewbie and ghorrocks,

Thanks for your advice. I'm not comapring multi-phase vs single-phase. It's just I don't know how to set the gravity effect properly. As you know, for single-phase, in the domain setting we can only find Boussinesq Model for buoyancy, which is not useful in my case. And I don't know other way other than using sub-domain to define gravity in single-phase model (which I found in one of ghorrocks's old thread).

I've been stuk here for a while and the help in CFX doesnt explain too much either. It will be appreciated if you guys can show me how to do it in a little more detail.

Thanks!!
ssbear is offline   Reply With Quote

Old   January 29, 2011, 07:02
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
For a single phase what would gravity affect? I think you will find gravity has no effect when you simplify it to single phase.

Gravity affects a multiphase (free surface) simulation by pulling the heavy fluid to the bottom. You definitely need gravity in this case. Activate it simply by setting the gravity vector. An example is the flow over a bump tutorial example.
ghorrocks is offline   Reply With Quote

Old   January 29, 2011, 15:54
Default
  #6
New Member
 
Ricky Chen
Join Date: Jan 2011
Location: Vancouver
Posts: 17
Rep Power: 6
ssbear is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
For a single phase what would gravity affect? I think you will find gravity has no effect when you simplify it to single phase.

Gravity affects a multiphase (free surface) simulation by pulling the heavy fluid to the bottom. You definitely need gravity in this case. Activate it simply by setting the gravity vector. An example is the flow over a bump tutorial example.

Thanks for your reply, ghorrocks. My question and main purpose right now is find the easiest way to simulate the flow in my case. Apparently to me single-phase flow is simpler than free surface flow. Another reason I don't prefer free surface model is that it can't simulate the particle tracking which I will be doing later on.

My problem for the single-phase model is if I don't set the gravity effect , the flow pattern doesn't make sense to me (please see the attached figure). So I was looking for a way to add gravity in single-phase model in this forum and the only way I found is to use the sub-domain.

It would be beautiful if there is an easier way to set the gravity effect in the single phase model. Please let me know.

BTW, by looking at the results from both methods I posted earlier, which one makes more sense to you?

Thanks very much for your advice and I'm looking forward to your reply!!
Attached Images
File Type: jpg Single-phase model.jpg (43.3 KB, 37 views)
ssbear is offline   Reply With Quote

Old   January 30, 2011, 05:39
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
What are you trying to model? You need to tailor the model to what you are trying to achieve. What is the purpose of doing your simulation?
ghorrocks is offline   Reply With Quote

Old   January 30, 2011, 13:37
Default
  #8
New Member
 
Ricky Chen
Join Date: Jan 2011
Location: Vancouver
Posts: 17
Rep Power: 6
ssbear is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
What are you trying to model? You need to tailor the model to what you are trying to achieve. What is the purpose of doing your simulation?
The main purpose of this practise is to simulate the flow in the intake and sediment movement.

I'm now trying to get the correct model, so later on I can change the intake geometry to optimize the flow. I'm a structural engineer and am new to CFD, so sometimes I might have some stupid question...
ssbear is offline   Reply With Quote

Old   January 30, 2011, 17:42
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Does the free surface move? Is it flat?
ghorrocks is offline   Reply With Quote

Old   January 30, 2011, 20:52
Default
  #10
New Member
 
Ricky Chen
Join Date: Jan 2011
Location: Vancouver
Posts: 17
Rep Power: 6
ssbear is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Does the free surface move? Is it flat?

No. There is a little curve at where the geometry trasition. Please see the attached pic, the green line at top is the water surface.
Attached Images
File Type: jpg 5_002.jpg (69.0 KB, 39 views)
ssbear is offline   Reply With Quote

Old   January 31, 2011, 07:19
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
So it is pretty flat. Is the little wobbles in the surface important? If you are modelling sedimentation then I do not think so. In this case you can run this simulation as single phase with a pressure boundary replacing the free surface. Single phase models are much easier and quicker so if this approximation is OK for you it will make things much easier.
ghorrocks is offline   Reply With Quote

Old   January 31, 2011, 14:22
Default
  #12
New Member
 
Ricky Chen
Join Date: Jan 2011
Location: Vancouver
Posts: 17
Rep Power: 6
ssbear is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
So it is pretty flat. Is the little wobbles in the surface important? If you are modelling sedimentation then I do not think so. In this case you can run this simulation as single phase with a pressure boundary replacing the free surface. Single phase models are much easier and quicker so if this approximation is OK for you it will make things much easier.

Thanks, ghorrocks~~
Will let you know when I finish my sediment model.
ssbear is offline   Reply With Quote

Old   January 31, 2011, 17:53
Default
  #13
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Be aware that CFX has limited capabilities in sediment modelling. The lagrangian particle tracking works fine, but it does not have models of sedimentation, picking up of sediment or good packing models. You may be able to develop these models yourself (that is not a task for a beginner!) or you could couple CFX with a discrete element model (DEM) such as EDEM to do the bits CFX cannot.

But I do not know whether this is important to you or not as you have not described your model in sufficient detail. The stuff built into CFX may be fine for you.
ghorrocks is offline   Reply With Quote

Old   February 4, 2011, 03:18
Default
  #14
New Member
 
Ricky Chen
Join Date: Jan 2011
Location: Vancouver
Posts: 17
Rep Power: 6
ssbear is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Be aware that CFX has limited capabilities in sediment modelling. The lagrangian particle tracking works fine, but it does not have models of sedimentation, picking up of sediment or good packing models. You may be able to develop these models yourself (that is not a task for a beginner!) or you could couple CFX with a discrete element model (DEM) such as EDEM to do the bits CFX cannot.

But I do not know whether this is important to you or not as you have not described your model in sufficient detail. The stuff built into CFX may be fine for you.

Thanks, ghorrocks. The feature in CFX is good enough for me for now.

I'm now trying to make the particle tracking model. My BC would be:

Inlet: normal speed = 2.5m/s (same speed for particle)
Outlet: static press = P, where P is the water pressure varies with the depth
Default domain: rough wall with 0.4mm roughness


Does that make sense to you?

Looking forward to your suggestions. Thanks very much!
ssbear is offline   Reply With Quote

Old   February 4, 2011, 06:20
Default
  #15
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
If you are modelling this single phase (and from your description so far I think you can) then do not model gravity and do not use a static pressure head on the outlet. Just a single pressure value.

Other than that your model should work. I have no idea if it is appropriate, however - that is for you to decide.
ghorrocks is offline   Reply With Quote

Old   February 6, 2011, 03:27
Default
  #16
New Member
 
Ricky Chen
Join Date: Jan 2011
Location: Vancouver
Posts: 17
Rep Power: 6
ssbear is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
If you are modelling this single phase (and from your description so far I think you can) then do not model gravity and do not use a static pressure head on the outlet. Just a single pressure value.

Other than that your model should work. I have no idea if it is appropriate, however - that is for you to decide.

Thanks, ghorrocks.

Yes, I'm modeling the signle phase.

In my project, the water in this intake structure has a free-surface. The outlet is the submerged penstock that is connecting to the turbine generate which allows a maximum flow of 29 m3/s. Assuming that maximum flow, I set my inlet BC as normal speed = 2.5 m/s, but I'm not sure which pressure value I should use for my outlet BC. Should I just set it to 0 Pa?

Don't know if there's enough information for the problem, but still looking forward to your precious advice.

Thanks~~~
ssbear is offline   Reply With Quote

Old   February 6, 2011, 06:01
Default
  #17
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Do not make boundary conditions up. If you know the outlet flow which connects to a known turbine flow rate, then make that the boundary - so use 29 m3/s on the outlet. Then put a pressure boundary at 0Pa on the inlet and it should work fine.
ghorrocks is offline   Reply With Quote

Old   February 6, 2011, 18:20
Default
  #18
New Member
 
Ricky Chen
Join Date: Jan 2011
Location: Vancouver
Posts: 17
Rep Power: 6
ssbear is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Do not make boundary conditions up. If you know the outlet flow which connects to a known turbine flow rate, then make that the boundary - so use 29 m3/s on the outlet. Then put a pressure boundary at 0Pa on the inlet and it should work fine.

Thanks, ghorrocks!

Will try it and let you know the result.
ssbear is offline   Reply With Quote

Old   February 7, 2011, 02:07
Default
  #19
New Member
 
Ricky Chen
Join Date: Jan 2011
Location: Vancouver
Posts: 17
Rep Power: 6
ssbear is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Do not make boundary conditions up. If you know the outlet flow which connects to a known turbine flow rate, then make that the boundary - so use 29 m3/s on the outlet. Then put a pressure boundary at 0Pa on the inlet and it should work fine.

ghorrocks,

I tried the particle model and there is something that doesn't look right. The particles in the water drop to the buttom of the domain and then climb up the slope... Is that because I didn't set the gravity correct? The particle here is sand (2300 kg/m3) at the diameter of around 1-3mm.

From the flow diagram, it shows that flow is going uphill on the slope, which doesn't make sense to me either...

Sorry for so many questions and thanks for your help.
Attached Images
File Type: jpg 18_001.jpg (41.2 KB, 32 views)
File Type: jpg 18_002.jpg (92.4 KB, 41 views)
ssbear is offline   Reply With Quote

Old   February 7, 2011, 05:37
Default
  #20
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
I do not think you looked at your results very hard.....

The particles are simply falling out of the flow due to their weight and hitting the bottom wall. You have modelled a big separation which results in a reverse flow up the slope. This reverse flow is pulling the sand up the slope.
itachi1002 likes this.
ghorrocks is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Problem in coupling CFX and Ansys for fluid-thermal sim. Jordi CFX 15 June 6, 2015 00:45
CFX pressure in Simulations problem nasdak CFX 1 April 14, 2010 13:22
CFX - Evaporation problem AlessandroD CFX 0 August 18, 2009 06:03
Ansys Workbench (CFX) bucket problem njsavage CFX 1 April 30, 2009 09:51
Can CFX deal with jet impinging problem? prayskyer CFX 1 September 4, 2006 17:04


All times are GMT -4. The time now is 02:54.