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

Question about layer additionremove

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 20, 2006, 18:19
Default When a layer of cells are adde
  #1
liu
Senior Member
 
Xiaofeng Liu
Join Date: Mar 2009
Location: State College, PA, USA
Posts: 118
Rep Power: 8
liu is on a distinguished road
When a layer of cells are added to the domain, how are the variables (such as velocity, pressure) defined? Are they just the copy from the master cells?
__________________
Xiaofeng Liu, Ph.D., P.E.,
Assistant Professor
Department of Civil and Environmental Engineering
Penn State University
223B Sackett Building
University Park, PA 16802


Web: http://water.engr.psu.edu/liu/
liu is offline   Reply With Quote

Old   February 20, 2006, 18:27
Default Sorry, I got another related q
  #2
liu
Senior Member
 
Xiaofeng Liu
Join Date: Mar 2009
Location: State College, PA, USA
Posts: 118
Rep Power: 8
liu is on a distinguished road
Sorry, I got another related question.
How about the values on the newly added faces? Are they evaluated immediately after they are added to the domain? Or should we force that process somewhere.

I got some discontinuity when I tried to solve scalar transport equation after a layer of cells are added.
Here is a picture. A object is moving on the floor. The scalar field is not so smooth.

__________________
Xiaofeng Liu, Ph.D., P.E.,
Assistant Professor
Department of Civil and Environmental Engineering
Penn State University
223B Sackett Building
University Park, PA 16802


Web: http://water.engr.psu.edu/liu/
liu is offline   Reply With Quote

Old   February 20, 2006, 20:10
Default Hi Xiaofeng, You need to be
  #3
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
Hi Xiaofeng,

You need to be a bit careful about this. There's something clearly wrong with the solution, but you may be looking at the wrong place.

For starters, for all points/faces/cells that are added to the geometry, there is a "parent" object, i.e. you can add a cell (say) from a parent point, a parent face etc. When the interpolation is done, the initial value in the new cell will be interpolated from the values around the parent. Thus, in cases where a cell is inserted off a point, all old cell values around the point are used for interpolation. In layer addition, cells are added off master faces; when the master face is internal, the old-time value is obtained by interpolation from old cells around it.

However, in reality, the old-time values for the added cells do not get used at all. This is because the cells are added in such a way that the "old-time" volume is zero and this multiplies the old-time value, giving zero. The actual work is done by the mesh motion algorithm, where the motion flux (volume swept by the face in motion) deals with the change in volume. Therefore, the new solution "mapping" (there's no mapping, really) will actually be obtained by the mesh motion algorithm.

It seems to me you've got a problem with the old-time and new-time volume and motion fluxes - please check in the scalar transport equation.

Enjoy,

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   February 21, 2006, 16:46
Default I tried again. Bad thing happ
  #4
liu
Senior Member
 
Xiaofeng Liu
Join Date: Mar 2009
Location: State College, PA, USA
Posts: 118
Rep Power: 8
liu is on a distinguished road
I tried again.
Bad thing happened just after the topological change. Here is the pictures.
Before the topological change. The object on the floor moved to the left for several steps and everything seems fine.


But when the topological change happens, it seems the flux are not valid for the newly added faces.

__________________
Xiaofeng Liu, Ph.D., P.E.,
Assistant Professor
Department of Civil and Environmental Engineering
Penn State University
223B Sackett Building
University Park, PA 16802


Web: http://water.engr.psu.edu/liu/
liu is offline   Reply With Quote

Old   February 21, 2006, 17:07
Default Another find. If I don't so
  #5
liu
Senior Member
 
Xiaofeng Liu
Join Date: Mar 2009
Location: State College, PA, USA
Posts: 118
Rep Power: 8
liu is on a distinguished road
Another find.

If I don't solve the scalar transport equation at the topological change step, every thing seems ok. I believe that flux information is not right at the topological change step for scalar transport. After that step, fluid flow evolved and these flux are constructed right.
__________________
Xiaofeng Liu, Ph.D., P.E.,
Assistant Professor
Department of Civil and Environmental Engineering
Penn State University
223B Sackett Building
University Park, PA 16802


Web: http://water.engr.psu.edu/liu/
liu is offline   Reply With Quote

Old   February 21, 2006, 17:18
Default That makes sense: you did not
  #6
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
That makes sense: you did not re-calculate the fluxes, right? I don't know which solver you have built this into, but the flux field at the point where you form the scalar transport equation is wrong/not up to date.

You will need to study and understand the top-level solver to find out where to insert the additional transport equation becaus enow it's in the wrong place.

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   February 21, 2006, 17:26
Default No, I didn't instruct the code
  #7
liu
Senior Member
 
Xiaofeng Liu
Join Date: Mar 2009
Location: State College, PA, USA
Posts: 118
Rep Power: 8
liu is on a distinguished road
No, I didn't instruct the code to re-calculate the fluxes.
The code I am modifying is settlingFoam. I want to model the effect of moving object on the sedimentation process.
The basic steps are following:
1. moveAndMorph() the mesh
2. solve alpha scalar transport equation (pictures shown above)
3. solve the flow field (PISO loop).

NOW I know why the flux is not right. That's because I solved scalar transport equation BEFORE the PISO loop. I will try it again.

Thanks Hrv.
__________________
Xiaofeng Liu, Ph.D., P.E.,
Assistant Professor
Department of Civil and Environmental Engineering
Penn State University
223B Sackett Building
University Park, PA 16802


Web: http://water.engr.psu.edu/liu/
liu 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
"Shear layer" vs. "mixing layer"- Difference mazadeh Main CFD Forum 5 April 10, 2009 10:17
"Shear layer" vs. "mixing layer"- Difference mazadeh FLUENT 2 April 18, 2008 14:46
Boundary Layer question Jason Mc Beth FLUENT 6 January 23, 2008 06:11
question on bounday layer modeling Wen Long Main CFD Forum 2 November 12, 2005 18:29
Boundary Layer Question P. Birken Main CFD Forum 4 March 7, 2003 08:19


All times are GMT -4. The time now is 21:54.