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

Solution Divergence because of BC?

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 30, 2016, 06:06
Unhappy Solution Divergence because of BC?
  #1
New Member
 
kengo
Join Date: Sep 2015
Posts: 2
Rep Power: 0
Kengo is on a distinguished road
Hi, everyone.

I am solving for external flow of airfoil in 2D using the pisoFoam solver.

It consists of a airfoil in a rectangular domain.

I use the following BC.

Pressure BC
inlet:fixedValue
outlet:advective
top_and_bottom:zero-Gradient(slip)
airfoil:zeroGradient
front_and_back:empty

Velocity BC
inlet:fixedValue
outlet:advective
top_and_bottom:slip
airfoil:no-slip
fron_and_back:empty

My question is
1.When I use following BC it works fine but why above BC doesn't work?
2.It's impossible to use fixedValue of pressure and velocity at inlet?

Pressure BC
inlet:zeroGradient
outlet:fixedMean
top_and_bottom:zero-Gradient(slip)
airfoil:zeroGradient
front_and_back:empty

Velocity BC
inlet:fixedValue
outlet:advective
top_and_bottom:slip
airfoil:no-slip
fron_and_back:empty

Thanks for the help.
Kengo is offline   Reply With Quote

Old   October 14, 2016, 05:54
Default
  #2
Super Moderator
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,843
Blog Entries: 6
Rep Power: 32
Tobi has a spectacular aura aboutTobi has a spectacular aura about
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Dear Kengo,

based on the fact that you are solving a linear set of equations for incompressible stuff, your over predict the matrix system, if you apply fixedValue for p and U on the inlet. Finally, there are infty of solutions and hence, your solver should blow up. If you are lucky you get some solution but this is not really accurate and can be non-physical, too. Your question is just related to numerics and how to solve linear systems (matrices). However, you can ask yourself if you set the velocity and pressure at the inlet and adjust the pressure and velocity at the outlet, how many different solutions there are. Hopefully you will realize that you can just play around with the pressure and velocity at the outlet to fulfill the mass conservation. That's, as I already told, the problem in setting up your simulation. If you would simulate some compressible case, it may work. In general, you should think about the case, the numerical behavior and maybe about the characteristics of the problem.

I hope you get the answer out of mine.
__________________
Keep foaming,
Tobias Holzmann
Tobi is offline   Reply With Quote

Old   November 4, 2016, 01:55
Default
  #3
New Member
 
kengo
Join Date: Sep 2015
Posts: 2
Rep Power: 0
Kengo is on a distinguished road
Dear Tobi,

Your answer helps me a lot thanks.
And besides I write here what I noticed about those problem.

The mesh type OpenFoam uses is not a staggered grid but a collocated grid.
All variables are defined at the center of control volume nevertheless I gave pressure and velocity at the same point(inlet). That is why my simulation diverged, right?
Kengo is offline   Reply With Quote

Old   November 8, 2016, 21:10
Default
  #4
Senior Member
 
khedar
Join Date: Oct 2016
Posts: 110
Rep Power: 2
khedar is on a distinguished road
fvMesh (openfoam) uses staggered grid, since this is based on fvm and has some parameters at the cell centers and others at the cell face centers.
khedar is offline   Reply With Quote

Old   December 10, 2016, 20:50
Default
  #5
Super Moderator
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,843
Blog Entries: 6
Rep Power: 32
Tobi has a spectacular aura aboutTobi has a spectacular aura about
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
To make things clear, FOAM stores everything at the cell center (not staggered). However, you can get rid of the problem with some mathematical expression/method (forgot the name). This method is (i guess) implemented in the toolbox. Otherwise it would not be so stable. I might ask my colleague for the theory name.

Sent from my HTC One mini using CFD Online Forum mobile app
__________________
Keep foaming,
Tobias Holzmann
Tobi is offline   Reply With Quote

Old   December 11, 2016, 04:47
Default
  #6
Super Moderator
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,843
Blog Entries: 6
Rep Power: 32
Tobi has a spectacular aura aboutTobi has a spectacular aura about
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
-> Rhie Chow Interpolation - fluxes at the faces.

Sent from my HTC One mini using CFD Online Forum mobile app
__________________
Keep foaming,
Tobias Holzmann
Tobi is offline   Reply With Quote

Reply

Tags
divergence.bc.pisofoam.

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
Divergence in non-Newtonian fluid UDF moabdi FLUENT 0 June 23, 2016 11:30
Converging the solution aja1345 FLUENT 10 June 26, 2015 18:00
Divergence problem Smaras FLUENT 13 February 21, 2013 06:03
3d vof Smaras FLUENT 2 February 19, 2013 07:58
Divergence in 8 node parallel solution hypete FLUENT 0 October 14, 2010 04:01


All times are GMT -4. The time now is 19:14.