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

Question from tutorial: Buoyant flow in a partitioned cavity

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 28, 2010, 05:48
Exclamation Question from tutorial: Buoyant flow in a partitioned cavity
  #1
New Member
 
Noppawit Sippawit
Join Date: Oct 2010
Posts: 14
Rep Power: 7
noppawit is on a distinguished road
Hello,

I'm trying to simulate a case really similar to the tutorial of Buoyant flow in a Partitioned cavity (Chapter 8).

From the tutorial, the air (Material: Air at 25 C) is initially at 5C and one side is heated up with fixed temperature of 75C and the opposite side is maintained at 5C.







From the result, why the pressure changes not so much? In my opinion refers to ideal gas law, the pressure should increase about 0.25atm. If I want to see 0.25atm increasing, how can I do? And also, what is the different between "Total Pressure" and "Pressure"?

Thank you so much.
Noppawit
noppawit is offline   Reply With Quote

Old   October 28, 2010, 18:14
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 11,565
Rep Power: 90
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F
ghorrocks is offline   Reply With Quote

Old   October 31, 2010, 22:00
Default
  #3
New Member
 
Noppawit Sippawit
Join Date: Oct 2010
Posts: 14
Rep Power: 7
noppawit is on a distinguished road
Does anyone know how to maintain constant volume?
noppawit is offline   Reply With Quote

Old   October 31, 2010, 22:05
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 11,565
Rep Power: 90
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
? In a closed cavity if you don't move the mesh you keep a constant volume.
ghorrocks is offline   Reply With Quote

Old   October 31, 2010, 22:21
Default
  #5
New Member
 
Noppawit Sippawit
Join Date: Oct 2010
Posts: 14
Rep Power: 7
noppawit is on a distinguished road
Thank you for your replies, I'm afraid that I still don't understand why my case doesn't follow Ideal Gas Law. Since you've mentioned that static mesh, volume is constant.
When I heat the gas, it should follow \frac{P_{1}}{T_{1}}=\frac{P_{2}}{T_{2}}. But from the simulation, it doesn't follow. From my understanding after I switched material to "Air Ideal Gas", CFX calculate the density of air after change in temperature, and it uses calculated density to calculate pressure. I tried to initialize the initial (static) pressure, also vary this initial pressure -->> the result is still the same (very small change in pressure).

Since my gas is a kind of gas expansion, how can I do it?
noppawit is offline   Reply With Quote

Old   November 1, 2010, 10:44
Default
  #6
Senior Member
 
Michael P. Owen
Join Date: Mar 2009
Posts: 195
Rep Power: 8
michael_owen is on a distinguished road
Are you running in steady state, or transient?
michael_owen is offline   Reply With Quote

Old   November 1, 2010, 10:54
Unhappy
  #7
New Member
 
Noppawit Sippawit
Join Date: Oct 2010
Posts: 14
Rep Power: 7
noppawit is on a distinguished road
I have tried both of them. But they are the same, I mean they don't follow ideal gas law. From my result above is transient, at 2s.
noppawit is offline   Reply With Quote

Old   November 1, 2010, 10:57
Default
  #8
Senior Member
 
Michael P. Owen
Join Date: Mar 2009
Posts: 195
Rep Power: 8
michael_owen is on a distinguished road
Are you setting the pressure level?
michael_owen is offline   Reply With Quote

Old   November 1, 2010, 11:03
Default
  #9
New Member
 
Noppawit Sippawit
Join Date: Oct 2010
Posts: 14
Rep Power: 7
noppawit is on a distinguished road
I really don't know what is pressure level? Where should I set it?

If you mean the initialization, I've already tried. But the result is still the same. I tried with 1atm, 2atm,.. in the box of static pressure.
noppawit is offline   Reply With Quote

Old   November 1, 2010, 11:39
Default
  #10
Senior Member
 
Michael P. Owen
Join Date: Mar 2009
Posts: 195
Rep Power: 8
michael_owen is on a distinguished road
The model is not conserving mass.

1. Make sure you are using Air Ideal Gas, and NOT Air at 25 C.
2. Run in Transient
3. Make sure that your Heat Transfer option (Domain definition, Fluid Models tab) is set to Total Energy OR
3a. If you use the Thermal Energy option, make sure that you set the minimum number of coefficient loops (Solver Control, Basic Settings tab) to 2
4. On the Solver Control, Basic Settings tab, check on Conservation Target. The default setting may be to loose for a transient simulation with a lot of time steps. Lower it if your mass conservation is poor.
4. On the Advanced Options tab of the Solver Control, check on Pressure Level Information and check on Compressible Transient Option.
michael_owen is offline   Reply With Quote

Old   November 2, 2010, 11:31
Default
  #11
New Member
 
Noppawit Sippawit
Join Date: Oct 2010
Posts: 14
Rep Power: 7
noppawit is on a distinguished road
Thank you for your reply. I'm trying on michael_owen's method. Roughly, the pressure increases about 2000Pa.
noppawit is offline   Reply With Quote

Old   March 18, 2014, 12:06
Default
  #12
Member
 
Join Date: Apr 2010
Location: Pisa / Italy
Posts: 57
Rep Power: 7
Atze is on a distinguished road
Quote:
Originally Posted by michael_owen View Post
The model is not conserving mass.

1. Make sure you are using Air Ideal Gas, and NOT Air at 25 C.
2. Run in Transient
3. Make sure that your Heat Transfer option (Domain definition, Fluid Models tab) is set to Total Energy OR
3a. If you use the Thermal Energy option, make sure that you set the minimum number of coefficient loops (Solver Control, Basic Settings tab) to 2
4. On the Solver Control, Basic Settings tab, check on Conservation Target. The default setting may be to loose for a transient simulation with a lot of time steps. Lower it if your mass conservation is poor.
4. On the Advanced Options tab of the Solver Control, check on Pressure Level Information and check on Compressible Transient Option.

Hi,

I've the same problem in a steady state simulation. How can I change this setting for my case?

thank you
Atze is offline   Reply With Quote

Old   March 18, 2014, 17:53
Default
  #13
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 11,565
Rep Power: 90
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
It is a transient only option. You should not need to do this sort of thing. Can you explain your problem more fully? I bet there is another more important problem causing it.
ghorrocks is offline   Reply With Quote

Old   March 19, 2014, 03:18
Default
  #14
Member
 
Join Date: Apr 2010
Location: Pisa / Italy
Posts: 57
Rep Power: 7
Atze is on a distinguished road
Hi Glenn,

I answered you in another post. By the way my problem is the same of noppawit but in steady state. I tried this tutorial but internal Absolute Pressure doesn't change with temperature
Atze 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
Urgent: Unsteady 3-D supersonic cavity flow Min-Sung Kang FLUENT 3 April 6, 2014 09:50
basic blockMesh : manipulate the lid-driven cavity flow tutorials Lexa OpenFOAM Meshing & Mesh Conversion 2 November 12, 2009 22:15
CFX gravity driven free surface flow tutorial mechovator CFX 37 July 27, 2009 10:28
Supersonic Flow over a Cavity (coodles): Maximum Iterations Exceeded sushant OpenFOAM Running, Solving & CFD 0 April 9, 2009 02:52
Question on 3D potential flow Adrin Gharakhani Main CFD Forum 13 June 21, 1999 05:18


All times are GMT -4. The time now is 13:31.