CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Community Contributions > OpenFOAM CC Toolkits for Fluid-Structure Interaction

[solids4Foam] HronTurekFSI3: Force calculation for the fsi tutorial, problems with validation

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

Like Tree3Likes
  • 1 Post By salachnaj
  • 2 Post By salachnaj

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   December 7, 2020, 16:59
Default HronTurekFSI3: Force calculation for the fsi tutorial, problems with validation
  #1
New Member
 
Justyna Salachna
Join Date: Dec 2019
Posts: 3
Rep Power: 3
salachnaj is on a distinguished road
Dear all,

I am trying to perform a validation of the solids4Foam based on the HronTurekFSI3 benchmark. I started the case basing on the tutorial added to the solids4Foam. First of all, I noticed that the force function in the controldict file has an incorrect value of rhoInf; I guess it should be 1000? and calcualtes force solely over the plate, not the plate + cylinder.

More importantly the force.gnuplot file, designed to plot the forces divide the force value over 0.015, and in that manner we reach the expected values of lift and drag. The units are set to [N]. Why we need to divide the forces over 0.015? Is it related to the solids4foam? Maybe somebody has already encounter the same problem?

I am enclosing a file with the results for the drag calculation for the fluid part of the benchmark (CFD3). The solids4Foam solver gives comparable results only when I divide over 0.015. Is the 0.015 realted to the area of the cylinder and the plate?



I tried to set to calculate the force coefficients instead, but I get information:

'Unknown function type forceCoeffs'

Is there any way to get force coefficients with use of solids4foam?

Here is the controlDict file part related to the force calculation. I added my comments in the parts where in my opinion needs to be updated.

plot [0.01:] "< sed s/[\\(\\)]//g ./forces/0/forces.dat" using 1$2+$5)/0.015
forces
{
type forces;
functionObjectLibs ( "libforces.so" );
outputControl timeStep;
outputInterval 1;
patches (plate); / /(plate cylinder)?
pName p;
UName U;
rhoName rhoInf;
log true;
rhoInf 100; //should be 1000?
CofR (0.5 0.1 0);

region fluid;
}
);

Please let me know, if someone of you encounter similar doubts.

Best regards, Justyna
W Mao likes this.

Last edited by salachnaj; December 9, 2020 at 12:55.
salachnaj is offline   Reply With Quote

Old   December 9, 2020, 12:54
Default
  #2
New Member
 
Justyna Salachna
Join Date: Dec 2019
Posts: 3
Rep Power: 3
salachnaj is on a distinguished road
Hi,
I received an anwer to my problem from Philip Cardiff, here it is:

"Hi Justyna,

The reason for dividing by 0.015 Is because the domain is 0.015 m thick in the Z direction, so dividing by 0.015 gives us the force per unit depth i.e. for a depth of 1 m (as specified in the paper).

You then might wonder why was the model setup to use a thickness of 0.015 m since it is 2-D and it should not matter. I think the reason for this is twofold:
- The model would be awkward to manipulate in ParaView if the Z dimension was 1 m
- (I think, but I would need to double-check) Interface geometrical tolerances depend on the size of the interface faces; if we used a model with such long faces in the Z direction, it may result in artificially large tolerances, so it is better to choose a Z dimension similar to the X/Y dimensions. "

I hope that helps! Regards, Justyna
bigphil and W Mao like this.
salachnaj is offline   Reply With Quote

Reply

Tags
hronturekfsi3, solids4foam

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
[ICEM] Problems with coedge curves and surfaces tommymoose ANSYS Meshing & Geometry 6 December 1, 2020 11:12
Problems of running Oscillating plate tutorial vovogoal CFX 20 February 4, 2016 07:03
Needed Benchmark Problems for FSI Mechstud Main CFD Forum 4 July 26, 2011 12:13
Two-phase air water flow problems by activating Wall Lubrication Force challenger85 CFX 5 November 5, 2009 05:44
how to extend FSI 2D codes to 3D, need advises abouziar Main CFD Forum 1 May 30, 2008 04:08


All times are GMT -4. The time now is 13:46.