This offering is not approved or endorsed by ESI Group or ESI-OpenCFD®,
the producer of the OpenFOAM® software and owner of the OpenFOAM® trade mark.
top
logo


New Release: foam-extend-3.0 "Jeju" The Extend Project is proud to announce the new release of the community fork of OpenFOAM®: foam-extend-3.0 [link]!
CoCoons Project - Community-driven Documentation of OpenFOAM® Technology! For more information have a look at www.cocoons-project.org!
Dear FOAMers: the Workshop Committee would like to invite you to the 9th International OpenFOAM® Workshop to be held 23-26 June 2014 in Zagreb, Croatia. [link].
Welcome, Guest
Please Login or Register.  Lost Password?
Optimization with OpenFOAM® Group Forum: All users which use OpenFOAM® for optimization are welcome!
Go to bottomPage: 1234
TOPIC: starting a discussion
#182
Re:starting a discussion 3 Years ago Karma: 0
Hey Ben,
the adjoint solver is not written into OpenFOAM®. I got a piece of code which was written for OpenFOAM® and could integrate it into my version.
I do not know if it is planned to integrate an adjoint solver into the standard version of OpenFOAM®....
Anne Lincke
Fresh Boarder
Posts: 14
graphgraph
User Offline Click here to see the profile of this user
The administrator has disabled public write access.
 
#183
Re:starting a discussion 3 Years ago Karma: 0
@ Ben: The adjoint solver is not part of the standard OpenFOAM® version. I got a piece of code written for OpenFOAm and integrated it into my version. It is a SIMPLE solver which solves for the primary Navier Stokes equations and foe the adjoint equations.

@ Guido: I know this paper. What is described in the paper is quite similar to what we are doing. Do you also want to solve adjoint equations with OpenFOAM®? It is also important to implement new boundary conditions for the adjoint variables which depend on the objective function. This might also be the problem in the thread www.cfd-online.com/Forums/openfoam-solvi...r-flow-problems.html

which you were mentioning....
Anne Lincke
Fresh Boarder
Posts: 14
graphgraph
User Offline Click here to see the profile of this user
The administrator has disabled public write access.
 
#184
Re:starting a discussion 3 Years ago Karma: 0
Has anybody used the DAKOTA Project for optimization at all (dakota.sandia.gov/)? I see that Engys is involved with it and I've seen it mentioned a couple of times before when it comes to optimizing CFD based models.
Ben Kenney
Fresh Boarder
Posts: 3
graphgraph
User Offline Click here to see the profile of this user
The administrator has disabled public write access.
 
#185
Re:starting a discussion 3 Years ago Karma: 1
Hi,
I have been using DAKOTA coupled with OpenFOAM® quite extensively for both CAD-driven and surface morphing shape optimisation. DAKOTA is quite robust and efficient and we use it on a daily basis as standard optimisation tool.
Paolo
Paolo Geremia
Fresh Boarder
Posts: 3
graphgraph
User Offline Click here to see the profile of this user
The administrator has disabled public write access.
 
#186
Re:starting a discussion 3 Years ago Karma: 0
Hi Paolo,
Can you explain how to couple the DAKOTA and OpenFOAM®??? I have been successful in installing DAKOTA ver 5.0 and openFOAM-1.7.x.Also, can you share a case as tutorial !!

Thanks

Arvind
Arvind Arya
Fresh Boarder
Posts: 5
graphgraph
User Offline Click here to see the profile of this user
The administrator has disabled public write access.
 
#187
Re:starting a discussion 3 Years ago Karma: 1
Hi Arvind,

Here is a typical sequence of steps required to couple DAKOTA with OpenFOAM®:

1. Create the DAKOTA input deck file including the variables, objectives, etc.

2. Create a parametric OpenFOAM® model where each variable is marked with curly brackets, like in the following:
inlet
{
type fixedValue;
value uniform ( {Uin} 0 0 );
}
where Unin defines a parametric inlet velocity in this case.

3. Create a shell script which performs the following tasks:
- pre-processing tasks (e.g. copy the OpenFOAM® template case working directory)
- update the OpenFOAM® parametric input file(s) by using Dprepro utility provided by DAKOTA
- create the mesh
- run OpenFOAM®
- read the results

Here is a sample script to run OpenFOAM® from within DAKOTA (i.e. "run_openfoam.sh"):

# $1 is params.in FROM Dakota
# $2 is results.out returned to Dakota

# Add pre-processing commands here

# Update OpenFOAM® parametric file (i.e. "U") by reading from template (i.e. ("U.template") using Dprepro utility
dprepro $1 U.template U

# Run snappyHexMesh or other to create mesh
snappyHexMesh

# Run OpenFOAM®
simpleFoam

# Copy the OpenFOAM® results back to DAKOTA
mv openfoam_results.dat $2


Remarks: make sure the relevant output response(s) (e.g. pressure drop) are written to a proper text file (e.g. "openfoam_results.dat") for later reuse in DAKOTA.

4. In the DAKOTA input deck file, use the following specifications for the interface section:

interface,
system
analysis_driver = './run_openfoam.sh'
parameters_file = 'params.in'
results_file = 'results.out'

Paolo
Paolo Geremia
Fresh Boarder
Posts: 3
graphgraph
User Offline Click here to see the profile of this user
The administrator has disabled public write access.
 
Go to topPage: 1234
Joomla SEO powered by JoomSEF


bottom
top

OpenFOAM®-Extend World

You need to upgrade your Flash Player

bottom
Legal | Imprint
©Copyright 2014 The OpenFOAM® Extend Project 

Powered by Joomla! Designed by Joomla Templates, ecommerce web hosting, Thanks to J! Developer Goran Gligorin for support! Joomla SEF URLs by Artio. Powered by Staff Master v0.9.8 Valid: XHTML and CSS

Friends Online

porno
Protected by Spam Fighter