在Docker里把OF里的完整矩阵抓出来了。

程迪

use OpenFOAM in docker

OS: windows 10

Install docker for windows

site: https://www.docker.com/

download: Docker for Windows Installer.exe

edition: most recent stable, for me, it is Docker version 17.09.0, community edition

installation instructions: https://docs.docker.com/docker-for-windows/

test

after completion of the installation, run Docker for Windows. It will cost some time to start the docker engine.

right click "Start" button, choose "Windows Powershell"

docker --version
## Docker version 17.09.0-ce, build afdb6d4
docker-compose --version
## docker-compose version 1.16.1, build 6d1ac219
docker-machine --version
## docker-machine.exe version 0.12.2, build 9371605
docker run hello-world
## 
## Hello from Docker!
## This message shows that your installation appears to be working correctly.
## 
## To generate this message, Docker took the following steps:
##  1. The Docker client contacted the Docker daemon.
##  2. The Docker daemon pulled the "hello-world" image from the Docker Hub.
##     (amd64)
##  3. The Docker daemon created a new container from that image which runs the
##     executable that produces the output you are currently reading.
##  4. The Docker daemon streamed that output to the Docker client, which sent it
##     to your terminal.
## 
## To try something more ambitious, you can run an Ubuntu container with:
##  $ docker run -it ubuntu bash
## 
## Share images, automate workflows, and more with a free Docker ID:
##  https://cloud.docker.com/
## 
## For more examples and ideas, visit:
##  https://docs.docker.com/engine/userguide/
docker ps -a
## CONTAINER ID        IMAGE               COMMAND             CREATED             STATUS                      PORTS               NAMES
## 32a621d46d34        hello-world         "/hello"            24 seconds ago      Exited (0) 23 seconds ago                       clever_agnesi
docker rm 32a621d46d34 #change it to your container ID
## 32a621d46d34 
docker ps -a
## CONTAINER ID        IMAGE               COMMAND             CREATED             STATUS                      PORTS               NAMES

download OpenFOAM image

right click "Start" button, choose "Windows Powershell"

docker pull openfoamplus/of_v1706_centos73 # OF+
# or
docker pull openfoam/openfoam5-paraview54 # OF5
# list images
docker image ls

run OpenFOAM

Right click on the "Docker" icon in the system tray, choose "settings"

Click "Shared drives"

choose any drive you want to share, in my case, I choose C, then click "apply"

you may need to input credentials

use openfoam+1706 as example.

press "WIN+R", input cmd and enter

rem test
docker run --rm -v c:/Users:/data alpine ls /data

rem ONLY `C:/Users` and its subfolders can be mounted
docker run ^
-i -t ^
--name myOFplus_1706 ^
-v c:/Users/dic17007/OpenFOAM:/OF ^
openfoamplus/of_v1706_centos73 ^
bash

rem press `Ctrl+p`, `Ctrl+q` to return without stop the container
docker attach myOFplus_1706

rem press `Ctrl+c` or input `exit` to return and stop the container

Note: you are root user in docker and the password is ofuser2017. Reference

setup the environment:

alias of1706="HOME=/OF source $DOCKER_OPENFOAM_PATH" 
# add to `~/.bashrc`
# echo 'alias of1706="HOME=/OF source $DOCKER_OPENFOAM_PATH"'>>~/.bashrc

run testcase

of1706 #activate openfoam
mkdir -p $FOAM_RUN
run
pwd #/OF/OpenFOAM/-v1706/run
cp $FOAM_TUTORIALS/incompressible/icoFoam/cavity/cavity -r .
cd cavity
foamJob -screen blockMesh
foamJob -screen icoFoam
touch a.foam

## use Ctrl+P, Ctrl+Q to return to `cmd`
## use `docker attach myOFplus_1706`

return to windows, use paraview to do post-process.

modify OpenFOAM solver

replication

run
cd ..
mkdir -p applications/solvers
cd applications/solvers
# I put my solver here.
pwd # /OF/OpenFOAM/-v1706/applications/solvers
cp $FOAM_SOLVERS/incompressible/icoFoam -r .
mv icoFoam myIcoFoam
cd myIcoFoam
mv icoFoam.C myIcoFoam.C
sed -i s/icoFoam/myIcoFoam/g myIcoFoam.C
sed -i s/icoFoam/myIcoFoam/g Make/files
sed -i s/FOAM_APPBIN/FOAM_USER_APPBIN Make/files

make

wmake

test

run
cd cavity
which myIcoFoam
foamJob -screen myIcoFoam

modification

I am trying to output the matrix in COO format ( Coordinate Format). It will be consists of three parts:

AA: non-zero values
JR: row index
JC: column index

According to the definition of Foam::lduMatrix::Amul() function, there are 4 part of scalar matrix:

diagonal terms: JC, JR=1 ... nCells, AA = matrix.diag();
upper terms: JC > JR
1. JR=matrix.lduAddr().upperAddr()[0...mFaces-1]+1
2. JC=matrix.lduAddr().lowerAddr()[0...mFaces-1]+1
3. AA=matrix.upper()
lower terms: JR > JC
1. JR=matrix.lduAddr().lowerAddr()[0...mFaces-1]+1
2. JC=matrix.lduAddr().upperAddr()[0...mFaces-1]+1
3. AA=matrix.lower()
boundary term, only considering single processor problem here. There are 3 types of patch types:
1. geometric (constraint) type.
2. basic
3. derived
In the following program, I assume there is not coupled interface such as processor patch or cyclic patch.

reference: Matrix coupling of different processors

Here is the code.

A c++ library cnpy is used to generate npy or npz file for numpy.

site: https://github.com/rogersce/cnpy
command:

git clone https://github.com/rogersce/cnpy.git
cd cnpy
mkdir build
cd build
cmake .. -DENABLE_STATIC=ON
make 
make install

dumpFvMatrix.H

#pragma once
// added by CatDog
#include<iostream>
#include<fstream>
#include<string>
#include"cnpy.h"

void dumpFvMatrix(string path, const fvScalarMatrix& EqnPtr)
{

	const label nCells = EqnPtr.diag().size();
	const label nFaces = EqnPtr.lower().size();

	const scalar* const __restrict__ diagPtr = EqnPtr.diag().begin();

	const label* const __restrict__ uPtr = EqnPtr.lduAddr().upperAddr().begin();
	const label* const __restrict__ lPtr = EqnPtr.lduAddr().lowerAddr().begin();

	const scalar* const __restrict__ upperPtr = EqnPtr.upper().begin();
	const scalar* const __restrict__ lowerPtr = EqnPtr.lower().begin();
	
	std::vector<scalar> AA(nCells+2*nFaces);
	std::vector<label> JR(nCells+2*nFaces);
	std::vector<label> JC(nCells+2*nFaces);
	
	// diag
	for(label cell=0;cell<nCells;cell++)
	{
		AA[cell]=diagPtr[cell];
		JR[cell]=cell;
		JC[cell]=cell;
	}
	
	for(label face=0;face<nFaces;face++)
	{
		AA[face]=upperPtr[face];
		JR[face]=lPtr[face];
		JC[face]=uPtr[face];
	}
	
	for(label face=0;face<nFaces;face++)
	{
		AA[face]=lowerPtr[face];
		JR[face]=uPtr[face];
		JC[face]=lPtr[face];
	}
	
	cnpy::npz_save(path,"nCells",&nCells,{1},"w");
	cnpy::npz_save(path,"nFaces",&nFaces,{1},"a");
	cnpy::npz_save(path,"AA",&AA[0],{nCells+2*nFaces},"a");
	cnpy::npz_save(path,"JR",&JR[0],{nCells+2*nFaces},"a");
	cnpy::npz_save(path,"JC",&JC[0],{nCells+2*nFaces},"a");
	
	return;
}

in myIcoFoam.C

// ...

#include "fvCFD.H"
#include "pisoControl.H"

#include "dumpFvMatrix.H"

// ...

// Non-orthogonal pressure corrector loop
            while (piso.correctNonOrthogonal())
            {
                // Pressure corrector

                fvScalarMatrix pEqn
                (
                    fvm::laplacian(rAU, p) == fvc::div(phiHbyA)
                );

                pEqn.setReference(pRefCell, pRefValue);

                pEqn.solve(mesh.solver(p.select(piso.finalInnerIter())));

                if (piso.finalNonOrthogonalIter())
                {
                    phi = phiHbyA - pEqn.flux();
                }
				
				if (runTime.timeIndex()==2)
				{
					Info<< "TimeIndex = 2, output matrix pEqn"<<endl;
					dumpFvMatrix("/OF/OpenFOAM/-v1706/run/cavity/pEqn.npz",pEqn);
				}
			}

// ...

options file:

EXE_INC = \
    -I$(LIB_SRC)/finiteVolume/lnInclude \
    -I$(LIB_SRC)/meshTools/lnInclude \
    -I/usr/local/include
EXE_LIBS = \
    -lfiniteVolume \
    -lmeshTools \
    -Wl,-rpath -Wl,/usr/local/lib -lcnpy

python script to read the matrix and find LU-SGS's effectiveness.

import numpy as np
import scipy as sp
from scipy.sparse import coo_matrix,tril,triu,diags
from scipy.linalg import norm 

data=np.load('pEqn.npz')
nCells=data["nCells"][0]
nFaces=data["nFaces"][0]
AA=data['AA']
JR=data['JR']
JC=data['JC']

A=coo_matrix((AA,(JR,JC)),shape=(nCells,nCells))

L=tril(A,-1)
U=triu(A,1)
D=diags(AA[0:nCells],0)
Dinv=diags(1.0/AA[0:nCells],0)

delta= L.dot(Dinv).dot(U)

print "norm of error of LU-SGS: norm(L*Dinv*U)=", norm(delta.toarray())/norm(A.toarray())
    
# a Laplacian operator
# proof of diagonally dominance
print abs(np.abs((L+U).toarray()).sum(1)/np.abs(D.toarray()).sum(1)-1).max() 
# proof of symmetry
print abs(L-U.T).sum() 


## reference: Jisheng Kou, Yitian Li, A uniparametric LU-SGS method for systems of nonlinear equations, In Applied Mathematics and Computation, Volume 189, Issue 1, 2007, Pages 235-240, ISSN 0096-3003, 
f=lambda w:norm(((1-w)*(L+U)-w*w*L.dot(Dinv).dot(U)).toarray())/norm(A.toarray())
for w in np.linspace(0,1,100):
	print f(w)

最后结果：

>>>
>>> print "norm of error of LU-SGS: norm(L*Dinv*U)=", norm(delta.toarray())/norm(A.toarray())
relative norm of error of LU-SGS: norm(L*Dinv*U)= 0.141875980931
>>>
... # a Laplacian operator
... # proof of diagonally dominance
... print abs(np.abs((L+U).toarray()).sum(1)/np.abs(D.toarray()).sum(1)-1).max()
0.5
>>> # proof of symmetry
... print abs(L-U.T).sum()
0.0

CFD中文网

在Docker里把OF里的完整矩阵抓出来了。

use OpenFOAM in docker

Install docker for windows

test

download OpenFOAM image

run OpenFOAM

modify OpenFOAM solver

replication

modification