我的检查表清单0

Pointwise

网格导出流程

[ ] Select Solver : OpenFOAM 3D
[x] Set BC types : make sure “all boundaries” are set or you may encounter --> FOAM FATAL ERROR: Continuity error cannot be removed by adjusting the outflow. Please check the velocity boundary conditions and/or run potentialFoam to initialise the outflow.
[x] Select blocks
[ ] Export CAE to some “$CASE/constant/polyMesh”
[x] Rescale to meter : transformPoints -scale ’(0.001 0.001 0.001)’
[ ] checkMesh [注：这里的skewness感觉是有量纲的(1/L^3)，从mm变到m之后，skewness从O(1e-9)变到O(1)]
[ ] serial run to check

配置OpenFOAM周期条件

语境
Pointwise里面网格为domain，OpenFOAM里面网格为patch

曾经天真的以为按照pointwise里面BC设定时选用cyclic，在网格文件生成完成后在constant/polyMesh/boundary里加上neighbourPatch就好，至少我在18.2R1这个版本不行。按照Maddalenna的提示。行得通的流程如下：

pointwise中要生成完全一样的domain，复制平移都不够（不够是指精度，重要的是点对点的对应关系），要达到这样的标准：create + periodic 这样生成的domain就是原先的twin，在domain list里面也可以看到domain之间的对应关系。这里就有了neighbourPatch的基础，没有这一步，极有可能会遇到face 1 area does not match neighbour *** by ***% -- possible face ordering problem.
按照pointwise基本流程导出网格文件，但在设置BC的时候设置成patch而不是cyclic
设置createPatchDict来完成patch到cyclic的转换. 默认createPatch 将生成新的网格文件，-overwrite可以改写原先网格文件，副产物还有一系列*.obj文件. 正确的Dict配置如下：

//  File system/createPatchDict
//  姑且在这个语境中用“面”代替patch

    {
        // Name of new patch
        name front_cyclic;     // 操作完成后会是cyclic类的面1的name

        // Type of new patch
        patchInfo
        {
            type            cyclic;      // 新面1，类型
            matchTolerance  0.001;
            neighbourPatch  back_cyclic; // 对应的新面2
        }

        // How to construct: either from patches or set
        constructFrom patches;

        // If constructFrom = patches : names of patches. Wildcards allowed.
        patches ( front );    // 旧面1
    }

    {
        name back_cyclic;      // 新生成的会是cyclic类的面2

        patchInfo
        {
            type            cyclic;
            matchTolerance  0.001;
            neighbourPatch  front_cyclic;
        }

        constructFrom patches;

        patches ( back );     // 旧面2
    }

这里需要解释一下：新面1,2是由旧1,2生成，生成的条件有“类型，matchTolerance,neighbourPatch”，当新2还没有生成的时候怎么将新1与新2对应呢？当然，这里如果把第一个大括号当成了新1 patch的constructor，它将找不到新2的定义。不过回想一下，其实旧12和新12都互为twin的关系，互相依赖，这样写并无道理，只是…程序具体怎么实现的就不知道了.
注1：为了保证无误，新旧1和新旧2的名字没有取一样；想改成新旧一样？走完这个流程，最后把constant/polyMesh/boundary里面改过来就好
注2：createPatch在这里是由原先pointwise的twin domains/patches由类型patch变成了类型cyclic，据utility的功能介绍还可以将patches变成一个patch，或者将faceSet变一个patch

OpenFOAM

Simulation 完整流程

环境变量
a) purge modules
b) set Foam environment : alias of301_intel
网格
a) transformPoints -scale '(0.001 0.001 0.001)'
b) checkMesh [need a time dir (empty dir is OK)]
c) 推荐使用格式上mesh变成binary，无论计算时的读写还是paraview读入都会更快 : foamFormatConvert -constant/-noZero [OF-2.3.1和OF-3.0.1在binary上不兼容，得通过ascii转换]
if needed, compile new Boundary Condition (which is a "*.so") for this simulation
初始条件+边界条件
a) IC (mapFields/topoSet)[OF-2.3.1 的 mapFields 就是个bug，推荐OF-4.x]
b) BC (changeDictionary) [推荐此处IC,BC均用ascii，便于查错和纠正]
system/controlDict :
a) check startTime 对不对, 保证startTime和endTime不相同 [如果相同OpenFOAM不会报错，log的末尾仍旧是”Finalising parallel run”]
b) 如果有自己编译的模块，加入libs ("*.so");
serial run check
if 5 is correct, prepare for parallel run :
a) decomposeParDict 指定MPI并行进程数
b) 清除startTime目录里面’uniform’
c) decomposePar -time 'startTime' : double check流场是否正确地被decompose. 首先写入硬盘的是constant/polyMesh的划分，后field transfer是流场的划分
d) BC : double check 一下BC有没有被正确写入processor*[value可能被改写，但原则上member一定要都在，在BC编写时write(Ostream&)写对了就没有问题]
e) if any warning : 要警惕，问题应当就出在当前步
如果测试节点足够，可考虑interactive parallel test；如不够，配置slurm file:
a) #SBATCH --job-name : sqeue 只能显示前8个字符
b) 队列, 节点数#SBATCH --nodes，每个节点task数#SBATCH --ntasks-per-node，总task数需要在srun或者mpirun那一行用到（可以小于节点数*单个节点task数）
c) 预估计算长#SBATCH --time
d) 允许含有 bash variable
e) 默认定向输出：标准输出#SBATCH --output；error输出#SBATCH --error
f) [仅occigen] slurm执行任务时的计算环境初始化配置 : 为避免module相关输出到error(竟然module purge也会输出到error我也是醉了，而我python monitor目前只扫描error文件里面有没有输出，认为没有输出才是正常运行状态)，这里slurm file 就不再加入任何的环境配置，通过第一个步骤即步骤0里面实现slurm任务提交时正确的环境配置[登陆之后第一个load的module为默认slurm提交环境，如果想换个环境，得logout然后重新登陆]
g) 注意 --exclusive 是否必要
h) 注意 --mem 是否足够
i) 主要任务执行行：即srun或mpirun那一行. 注意切忌行末加&幻想后台运行[例如后面一行还有其他executable的情况，如果当下行能后台运行，其后的command会被继续执行也许会有便利…但这样做的结果是&之后就没有然后了，而且还可能error message都没有，得不偿失]
j) 还在主要任务执行行 : 通常将标准输出改到 > logFile : 注意最好把所有的log都留下，也就是每一个任务换一个文件名 [改到：因为前面谈到#SBATCH --output，用这个选项会由slurm在机群上的任务提交顺序来命名，可读性不强，通常改写]
[optional] submit job chain via python :
a) [仅occigen] 因为$SCRATCH文件数目限制 : check-list python laundary
b) check-list python auto submit
paraview : 有条件的话（因为通常processor文件数目很多）优先读decomposed case (因为internalField没有影响，但经测试reconstruct可能boundaryField的value会被篡改)

注：IC 指初始条件；BC 指边界条件

preProcessing

mapFields

此为大坑，尤其是OF-2.x的版本，存在一些bug(不是fatal，但会让mapFields运行得无比慢，比fatal还可恶。按照帖子改了还是不行)，但用同样的mapFieldsDict试一试OpenFOAM/4.0-foss-2016b或者OpenFOAM-5.x不仅速度快而且不会有莫名其妙的报错

#!/bin/bash
source=/some/case/to/be/mapped
#taget 这里target就是"."

mapFields $sourcedir -case . -noFunctionObjects -fields '(U p T)' -sourceTime '8' -targetRegion region0 > log.mapFields_8 2>&1

回避
a) $source里empty的BC（有试过，会有报错）
b) 如果$source里面constant/polyMesh/boundary里面有mappedPatch，且如果$target里面没有相应的BC配置，可能会在mapFields最后写入数据的时候报错后果是例如U文件的写入遇到错误而被跳过].在$source有mappedPatch的情况下，$target里面constant/polyMesh/boundary也得改成相应BC
如果不是consistent，目标case里面要编辑好文件mapFieldsDict
确认$source里面startTime，它会是mapFields完成后的时间目录，输出格式改为ascii
检查在controlDict里面libs (...)是否在当下环境中配置
mapFields (等待时间可能很长)
手动检查mapFields是否无误地完成：检查目标case里面是否有-nan
把映射后的场的BC由calculated改成相应的物理BC，这样才可以续算，这个步骤可以通过changeDictionary来完成
串行试运行

# 一个长度为5D的圆管映射到一个长度为10D的圆管，inlet*完全对应
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      mapFieldsDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

patchMap        ( inlet0 inlet0         // Source 和 Target 都有的 patch
                  inlet1 inlet1         // 且一一对应
                  inlet2 inlet2
                  inlet3 inlet3
                  inlet4 inlet4 );

cuttingPatches  ( wall                  // 剩下 wall patch 和 outlet*
                  outlet0               // 此处为空->(U p)在 wall 和 oulet* 会出现异常大数甚至nan!!
                  outlet1               // 只填 wall， wall上面插值没有异常大数出现
                  outlet2               // 填上 wall patch 和 outlet*, outlet*都乖乖地保持了“最简单状态” (虽然U在 
                  outlet3               // outlet*上面不应该是 uniform (0 0 0)，但毕竟是 type calculated
                  outlet4 );

// ************************************************************************* //

# 两个T型圆管，几何完全一样，但网格不同
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      mapFieldsDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

patchMap        ( Port1 Port1        
                  Port2 Port2
				  Port3 Port3
				  wall  wall  );

cuttingPatches
();
// ************************************************************************* //

旋转data然后mapFields

想要rotate data，transformPoints声称可以rotate polyMesh里面的points(也就是网格)，也可以rotate vector field.试过了，确实可以，paraview上就看出来转了90度，但是将rotate过后的再mapFields就不成功了，经过反复测试始终还是rotate之前的data被map过去了的感觉

postProcessing

管理postProcessing

rsync.py将远程的postProcessing同步到本地目录，并通过json将相关数据存入一个文本文件database.txt:

sourceDir:远程目录
targetDir:本地目录
name2plot:画图的时候用到的legend
还有alias，即一个对case简单描述的string

画图的时候，在配置文件parameters_*.py里面有：读database.txt，通过alias来索引database[alias]['targetDir']和database[alias]['name2plot']

一旦按照以上操作“1.获取数据”并“2.抓取数据画图”，只需要确认有一致的alias就可以确认“画的数据是自己想要的”，具体的数据信息也可以通过database.txt来最终索引，只要这个索引不出错，就不会错

uv : reynoldsStress

# toolchain for uv_mean @12
userAverageVector U -time '6:12' # U_mean
userReyTensor_plusAvg U 12 -noIntermediateWrite -time '6:12' # reyTensor_mean, 不输出中间的reyTensor速度还是比较快的
userRMSuvw_fromReyTensor_mean -time '12' # uv_mean
sample -dict $sampleDicts/sets/set4uv -time '12' > log.set4uv 2>&1  # 需要sampleDict : set4uv

# 需要注意的在这里
# 以上最后一步输出有128个sample的结果，但只用其中64个来算uv，因为上下壁面会相互抵消(uv的定义相对于壁面，v的定义在两个壁面是反的)
# 这就是[parameters_](https://github.com/snow-stone/python/blob/master/userSetUV/parameters_t_r-2a_1_gradP0p703125.py)里面`'raw_sample_size':64`的原因

userProbeByLabel_noMean

or userProbeByLabelVector_noMean its version for vectors. $sliceStore is where you put your slice+number file (class labelList). userProbeByLabel_noMean don’t work on slices but on labelGroup which is itself a labelList containing all cell id of probes of interest (its defaut location is $sliceStore.

check-list userFindClosestInLabelList
userProbeByLabel_noMean T $sliceStore -time ‘0:xxxx’

userFindClosestInLabelList

前提是在input argument里面sliceStore处已经有sliceNumberList和refVectors，这个程序找的是遍历在sliceNumberList里面所有的slices找到离refVectors（注：这里仅有一个vector，但仍旧用vectors，为得是日后可以拓展）最近的cell，并将每个slice上面最近的cellID记下来写入到一个文件labelGroup.这个程序应当在一个OpenFOAM case中执行，其实就是提取网格信息，因此对于相同网格下的算例仅仅需要运行一次，于是就有了最后一个步骤将labelGroup移动到对应同一个网格的公共的目录下共享，详细check-list如下:

为了最终写出的labelList人类可读:system/controlDikt change format to ascii
userFindClosestInLabelList xx xx
cd constant
mv file to a shared place (for all cases with the same mesh structure)

reconstructPar

在reconstructPar -fields '(U p)'之后，reconstructPar -fields '(phi)'会将phi添加到对应的时间目录里面.

sample

基本流程

#!/bin/bash
sampleDict=system/sampleDict

sample -dict $sampleDict/sets/Dai_lines_5cutsBetween2and3_typeFace_cell -time '8:10' > log.sample-Dai_lines_5cutsBetween2and3_typeFace_cell 2>&1

编辑sampleDict：可能需要用python脚本来写入一系列sets的描述，例如160条线就不能全部手写
a) 检查fields，如果写得不对，OpenFOAM并不会报错
b) 检查是否有header（没有header会有报错），object填sampleDict
c) sets或者surfaces的输出文件名都可以个性化编辑
重命名sampleDict，是sets放目录$sampleDict/sets，是surfaces放目录$sampleDict/surfaces
sample

注：检查不出sample是否有结果？rm -rf postProcessing ; sample 这样会比较明确

用python写sampleDict

# file writeSampleDict_2Diagonals.py

import numpy as np
import os

def writeStartEnd(whichLineGroup,f,z,nPoints):
    if whichLineGroup == 0:
        f.write("\t\t"+ "type\t"  + "uniform;" +"\r\n")
        f.write("\t\t"+ "axis\t"  + "distance;" +"\r\n")
        f.write("\t\t"+ "start\t" + "("+z+ " 0.004 0.004);" +"\r\n")
        f.write("\t\t"+ "end\t" + "("+z+ " -0.004 -0.004);" +"\r\n")
        f.write("\t\t"+ "nPoints\t" + str(nPoints) + ";" +"\r\n")
    elif whichLineGroup == 1:
        f.write("\t\t"+ "type\t"  + "uniform;" +"\r\n")
        f.write("\t\t"+ "axis\t"  + "distance;" +"\r\n")
        f.write("\t\t"+ "start\t" + "("+z+ " -0.004 0.004);" +"\r\n")
        f.write("\t\t"+ "end\t" + "("+z+ " 0.004 -0.004);" +"\r\n")
        f.write("\t\t"+ "nPoints\t" + str(nPoints) + ";" +"\r\n")
    else:
        print "big problem"

def writeLines(f,z_value_List,N,Nb_lineGroup,resolution,dictName):
    for i in range(Nb_lineGroup*N):
        whichLineGroup = i // N  # quotient  0, 1 ,2... Nb_lineGroup
        j = i % N                # remainder 0, 1, 2... Ns
        
        f.write("\t"+dictName+'-'+str(i)+"\r\n")
        f.write("\t{\r\n")
        writeStartEnd(whichLineGroup,f,z_value_List[j],resolution)
        f.write("\t}\r\n")
        f.write("\r\n")        
    
def write_LineSet(f,z_value_List,Nb_slices_along_z,Nb_lineGroup,resolution,dictName):
    f.write("sets\r\n")
    f.write("(\r\n")
    writeLines(f,z_value_List,Nb_slices_along_z,Nb_lineGroup,resolution,dictName)
    f.write(");\r\n")

def write_headerSetting_sampleLines(f,fieldName,interpolationScheme):
    f.write("setFormat raw;\r\n")
    f.write("\r\n")
    f.write("interpolationScheme "+interpolationScheme+";\r\n")
    f.write("\r\n")
    f.write("fields\r\n")
    f.write("(\r\n")
    f.write("\t"+fieldName+"\r\n")
    f.write(");\r\n")

def write_sampleLines(dictName,fieldName,interpolationScheme,z_value_List,Nb_lineDisplacement,Nb_lineGroup,resolution):
    f= open(dictName,"w")
    write_headerSetting_sampleLines(f,fieldName,interpolationScheme)
    write_LineSet(f,z_value_List,Nb_lineDisplacement,Nb_lineGroup,resolution,dictName)
    f.close()
    
def NLines2Dict(Nb_lineDisplacement):
    l = np.linspace(-0.08,-0.04,num=Nb_lineDisplacement)
    listStr = [str(x) for x in l]
    print "A list of all line displacements :\n"
    print listStr
    
    dictName="lineOn2Diagonals"
    fieldName="U_mean"
    interpolationScheme="cell"
    write_sampleLines(dictName,fieldName,interpolationScheme,listStr,Nb_lineDisplacement,2,resolution=200)
    
    os.system('dos2unix '+dictName)
    print "\n"
    print "sampleDict written. Think to add a file header!"

NLines2Dict(64)

configure python script for sampleDict : dictName, fieldName, interpolationScheme… Sampled data will be named as `postProcessing/sets/time/dictName-n_fieldName. “dictName” may also includes information like “interpolationScheme”.
run python script
add header to sampleDict
run sample utility
verify generated files in postProcessing
begin plotting using python
edit plot parameters : a spatial statistic will require “time”, “number of samples” etc. This file is the footprint of the statistics.
configure plot script : ajust “dataShape” or likewise. In other word, not all data are eligable because not all data are of the same shape. We can interpolate but I d rather not.
run plot script
ajust plot and save fig to figure
write plot data (x,y) to txt file in foler data for reporducing use or later ajustement

python

laundary

为了防止occigen $SCRATCH关于文件数量的quota溢出，用python在后台nohup长时间地监控，对userDefinedLog里面removedTimes与dataWritingHistory的补集的时间步做reconstructPar和rm -rf processor*/timeStep

拷贝laundary.py和reconstruct_occigen-OF301.sh
保证userDefinedLog/removedTimes存在
设置python脚本的时间参数（预估simu时长，留出laundary余量）和processor个数的参数
检查上一个laundary是否结束:ls -l log.clean_*看时间
判断reconstructPar的进程:ls processor0 | xargs ls -l > log.ls；如果有的目录没有顺利reconstructPar会有内容(非std output)输出到终端，至于目录对应上了但场是否完全(比如U p nu phi) reconstructPar 只能看log.ls
a) reconstructPar有很多时间步积压，手动完成laundary，然后进行b)
b) reconstructPar运行顺利，没有太多时间步积压在processor*里，那么准备续算：rm userDefinedLog/dataWritingHistory并清空userDefinedLog/removedTimes里面的内容
nohup python laundary.py OF301 > log.clean_*
记录是在哪个登陆节点，需在对应的节点用ps -eaf | grep $USER才能找到nohup的任务

cluster

occigen

算例提交

openfoam env : 一句话如果用python来做slurm多个连续任务提交，必须在提交前做好这一步(即check-list第0步)，具体来说如果忘记了提交slurm会在第一个job报错，然后你发现slurm找不到mpirun，这时候补上环境变量再重新提交，新的提交第一个job能通过，但第二个job仍然会报错找不到 mpirun；似乎slurm的默认环境是你登陆某login节点后第一次提交任务的环境，也就是说：login之后得首先做这个事情再提交任何算例(虽然直接使用sbatch **倒是不影响，但对通过python来提交的job chain会被迫终断）
nohup python submit.py > log.submit : 提交job，通过squeue的返回值离散地监控job状态，通过返回值来检验一个算例完成后(这里还有个bug)修改system/controlDict里面startTime和endTime用于自动提交下一个算例(限制：simuLog不停地被改写，应该把每个job的log都留下来才好)；log.submit取好名字以方便查看
nohup python watchDog.py > log.watchDog : 设置一个运行最大时长，在这个时间内用reconstructPar来保留计算输出数据，删除processor*里面已经reconstructPar完成地时间步大幅度削减文件个数，保证不超过scratch的限额；log取好名字以方便查看
G3. 笔记本上面记录下来是哪个login，什么算例，连续提交多少个job，每个job预计计算的物理的间隔是多少(用于更新startTime和endTime)：因为ps -eaf | grep $USER只能找出相应登陆节点上面的job
检查log.submit，查看jobs的情况

数据同步

千万千万要注意para0，在dir里面并没有用到，一定要double check !!!!

#!/bin/bash

para0=inlet_0p3
para1=a_0p08
para2=setT_St_1
log=sync_log.$para1
dir=/store/lmfa/fct/hluo/occigen/caseByGeometry/T/shape_square/2a_3_T/BirdCarreau/inlet_0p3/$para1rsync -av occigen:/scratch/cnt0028/mfa0464/hluo/caseByGeometry/T/shape_square/2a_3_T/BirdCarreau/$para0/$para1/$para2/* DATA --exclude processor* &&
echo "DATA sync BirdCarreau : $para0 $para1 $para2 ended with success" >> $dir/$log

newton

No #SBATCH --exclusive (if not necessary)
Naming of the file with exactly 8 chars with -2 indicates for example 2nd run. Ex : p10D_gP5-2
consider remove #SBATCH --mem-per-cpu=4000 because there are nodes which bigger memory available

error

error while loading shared libraries: libpsm_infinipath.so.1: cannot open shared object file: No such file or directory : check #SBATCH --mem, this is an error saying you are maybe asking for more memory than the machine can offer
slurmstepd: error: Detected 1 oom-kill event(s) in step... : check #SBATCH –mem`, this is an errory saying that the memory you are asking for is not enough for the program

old note

#!/bin/bash
# FILE : p10D_gP5-2

#BATCH --job-name=MeshConvergence                    # Is this even useful ? SABTCH no?
#SBATCH --output=job.%j.out
#SBATCH --error=job.%j.err 
#SBATCH --mail-user=haining.luo@doctorant.ec-lyon.fr
#SBATCH --mail-type=ALL
#
#SBATCH --partition=mononode
#SBATCH --mem-per-cpu=4000
#SBATCH --nodes=1
#SBATCH --ntasks-per-node=16
#SBATCH --cpus-per-task=1
#SBATCH -t 1-00:00:00

# number of simulation
nos=2
logFile=logSimulation$nos

# 在newton上module purge load部分可以保留
module purge
# Opt/Debug mode on
module load OpenMPI/1.6.5-GCC-4.8.3 ; \
. /home/lmfa/hluo/LocalSoftware/OpenFOAM/OpenFOAM-2.3.x/etc/bashrc.Opt

echo "NodeName = " $SLURMD_NODENAME >> $logFile
echo "JobID = " $SLURM_JOB_ID >> $logFile

mpirun -np 16 pimpleFoam -parallel >> $logFile

run mapFields need a big memory. There’s now a template for big-memory job. Especially, don’t put & at the end of commands or mapFields will only last for 2s and there’s no error message returned so could be confusing.

#!/bin/bash
#
##SBATCH --job-name=T-1b_mirrorMerge_mapped
#SBATCH --output=job.%j.out
#SBATCH --error=job.%j.err 
#SBATCH --mail-user=haining.luo@doctorant.ec-lyon.fr
#SBATCH --mail-type=ALL
#
#SBATCH --partition=test
#SBATCH --mem=32000                  # asking for 32000Mb ~ 30Gb of memory 
#SBATCH --nodes=1                    # 1 node
#SBATCH --ntasks-per-node=1          # one task for one node
##SBATCH --cpus-per-task=1           # one cpu per task
##SBATCH -t 1:00:00

# number of simulation
nos=1
logFile=logSimulation$nos

module purge
# debug mode on
module load OpenMPI/1.6.5-GCC-4.8.3 ; \
. /home/lmfa/hluo/LocalSoftware/OpenFOAM/OpenFOAM-2.3.x/etc/bashrc.Opt

# run solver 
#decomposePar  # Do this manually

echo "NodeName = " $SLURMD_NODENAME >> $logFile
echo "JobID = " $SLURM_JOB_ID >> $logFile

#mpirun -np 64 icoFoam -parallel >> $logFile

sourcedir=/home/lmfa/hluo/LocalSoftware/OpenFOAM/hluo-2.3.x/run/1b_mirrorMerge_mapped_NearestFace
mapFields $sourcedir -case . -noFunctionObjects -fields '(U p)' -sourceTime '6.01' -targetRegion region0 > logMapFields_new 2>&1  # No "&" here

Here maybe a reason that zaurak well perform likely 2 times better than cpus on newton when the constraint on memory is not there.

hluo@zaurak $ cat /proc/cpuinfo | grep model
#...
model name	: Intel(R) Xeon(R) CPU E5-1620 v4 @ 3.50GHz

hluo@compil-haswell $ cat /proc/cpuinfo | grep model
#...
model name	: Intel(R) Xeon(R) CPU E5-2660 v3 @ 2.60GHz

hluo@visu $ cat /proc/cpuinfo | grep model
#...
model name	: Intel(R) Xeon(R) CPU E5-2640 v4 @ 2.40GHz

Inkscape

导出

[ ] draw sketch
[x] Edit-> Resize page to selection
[ ] Export PNG image -> Export as -> Export

在最后一步如果遇到”the chosen area to be exported is invalid”,可以在Export PNG Image标签页里面四个标签Page,Drawing,Selection,Custom（默认是最后一个），选成比如说Drawing再点Export.

clip

import image
F4 (select “rectangular tool”) draw a rectangular (marked by red)
F1 (select “select tool”), ctrl+A select all
Object -> clip -> set

gimp

这个软件可以得到图片里面的坐标

paraview

显示几何外形

如果想要显示一下外形，但又不想要网格视角:
Clean to grid -> Extract surface -> change opacity

scripting

load state

load state也可以被载入到script里面(no legend)

I. 用paraview生成*.psvm

paraview -> start trace -> open *.foam -> …
saveFig (very possible I will do this. otherwise its nonsense.)
save state
stop trace

II. 拿出上一步得到的script，把关键行(例如)

LoadState('/store/T_c/1j/D2-NN-1j_test_from0p3_forcingSinus_St3p2_A_eq_0p05/hluo15_T_c_vorticity_z_300.pvsm', LoadStateDataFileOptions='Use File Names From State',
    DataDirectory='/store/T_c/1j/D2-NN-1j_test_from0p3_forcingSinus_St3p2_A_eq_0p05',
    OnlyUseFilesInDataDirectory=0,
    D2NN1k_syn_forcingfoamFileName='/store/T_c/1j/D2-NN-1j_test_from0p3_forcingSinus_St3p2_A_eq_0p05/D2-NN-1k_syn_forcing.foam')

转换为

SaveScreenshot(dirName+'/'+'hluo15_T_c_vorticity_z_300.png', renderView1, ImageResolution=[2754, 1838],
    FontScaling='Scale fonts proportionally',
    OverrideColorPalette='',
    StereoMode='No change',
    TransparentBackground=0, 
    # PNG options
    CompressionLevel='5')

尾巴上再加入

import os
print "Finalizing "+ os.path.basename(__file__) +" " + "@ dir : " + dirName 
import datetime
print datetime.datetime.now().strftime("%Y-%m-%d %H:%M")
print "==============================="

III. 对不同目录（不同case）批量操作:

拷贝*.psvm到相应目录（如果pvpython找不到*.psvm也会出图，白板）
修改*.psvm里面带有关键字.foam的行，对应当下目录
来到run.sh，用绝对路径作为参数开始批量运行

出图程序里面修改变量的range

LUT.RGBPoints和PWF.Points里面上下界都得改，PWF.RescaleTransferFunction也要改，当然LUT.UseLogScale也要改：


# get color transfer function/color map for 'k_mean_nonD'
# ...
k_mean_nonDLUT.RGBPoints = [1e-6, 0.231373, 0.298039, 0.752941, 0.00014459355054441403, 0.865003, 0.865003, 0.865003, 1, 0.705882, 0.0156863, 0.14902]

# get opacity transfer function/opacity map for 'k_mean_nonD'
# ...
k_mean_nonDPWF.Points = [1e-06, 0.0, 0.5, 0.0, 1, 1.0, 0.5, 0.0]

# Rescale transfer function
k_mean_nonDPWF.RescaleTransferFunction(1e-06, 1)

# Properties modified on k_mean_nonDLUT
k_mean_nonDLUT.UseLogScale = 0

纯粹读数据，摸索数据结构

似乎是默认读最后一个时间步，为免出错，每个case就一个时间步

#### import the simple module from the paraview
from paraview.simple import *
#### disable automatic camera reset on 'Show'
paraview.simple._DisableFirstRenderCameraReset()

# create a new 'OpenFOAMReader'
cavityfoam = OpenFOAMReader(FileName='/home/hluo/OpenFOAM/hluo-2.3.1/run/tutorials/incompressible/icoFoam/cavity_org/cavity.foam')

print type(cavityfoam)
print cavityfoam.CellArrays
print type(cavityfoam.CellArrays)
print "GetAvailable()"
print cavityfoam.CellArrays.GetAvailable()
print "GetData()"
print cavityfoam.CellArrays.GetData()

data=servermanager.Fetch(cavityfoam)
print type(data)
print "GetNumberOfBlocks() : " , data.GetNumberOfBlocks()
#print "getBlock() : " , data.GetBlock(1)
obj = data.GetBlock(0)
print obj.GetNumberOfCells()

cellData = obj.GetCellData()
N = obj.GetNumberOfCells()
#print cellData
obj_p = cellData.GetArray('p')
print type(obj_p)
print "obj_p.GetDataTypeValueMin() : ", obj_p.GetDataTypeValueMin() # 这里得出的最大最小有问题
print "obj_p.GetDataTypeValueMax() : ", obj_p.GetDataTypeValueMax()

print obj_p.GetValue(10)

print "GetRange() : ", obj_p.GetRange() # 这里貌似是正确的
for i in range(N):
    obj_p.SetValue(i, obj_p.GetValue(i)/10)

print obj_p.GetValue(10)

export screen shot

export 有什么好说的？嗯……如果要对一系列算例做同样的图一般会选用load state来加载*.pvsm，似乎注意改一下*.foam对应的path就好，但是如果要让export screen shot输出同样像素的图的话，记得一定要全屏之后再export！！

do not skip time 0

paraview data.foam
uncheck all “Cell Array” ; remain defaut “Skip Zero Time” then apply : geometry will be visualized but no “Cell Array” (field data) is there. Make sense.
uncheck “Skip Zero Time” -> apply : cell array will then appear ; select field of interest.

color map

如果是对成的数据[-a,a]，用红白蓝diverging挺好，能分辨出0对应白
如果是[0,a]，用黑白灰最好，但paraview好像默认可以从Edit Color Map选项卡中带桃心的小按钮Choose Preset里面有X-ray和GrayScale，选择后apply（默认就会变到RGB color Space）；如果想要恢复diverging，最下面有个恢复默认按钮；如果想要自定义，参见RBG自定义

用load state来复现camera视角

target 目标视角：想要复制的视角，对应的case叫目标case
working 工作视角：想要在工作case下复现目标视角

目标视角的存储通过目标case(Visu)里save state来实现(默认读取了一个绝对路径的但其实为空白的target.foam文件)，得到target.pvsm
复制目标case下的target.pvsm到工作case(Visu)里，编辑查找关键字target.foam并替换成工作路径/working.foam
工作路径下创建working.foam
工作路径下打开paraview
load state 选择编辑后的target.pvsm-> “Load State Data File Options” 选Use File Names From State
等待复现

注意：

还涉及一个working case里面时间步是不是和state里面一致的事情，我的测试刚好target和working case有相对应的同一时刻的data
在paraview-5.4.1测试成功

根据x坐标截取一个cell slice的label

cell slice : 这里的网格是正交的六面体，所以严格意义上一个x坐标对应“一层网格”，通过在paraview里面find Data中选取xcoord between xx and xx就可以选定这一系列cell
label : 一系列的cell的label合起来就是个labelList，而且是全局的，因此可以取出U中例如U[labelList_slice0]子集进行操作

下为流程：

paraview 可视化 case
calculator : xcoord (defaut : point data)
Filters -> Point data to cell data 这里我们只想对xcoord操作但注意这一步会将U(如果有的话)也插值一遍，值会跟先前有略微差别
Edit -> fidn Data -> (cells) (Pointdatatocelldata) (criteria : xcoord between [xmin, xmax] -> run selection
close “find Data” (selection is still effective)
split horozontal (very smalll icon on the right above render view) -> spread sheet -> show only selected elements -> attribute : cells 注意一定要选cells要不然得到的spread sheet行数不是cell number -> check 行数是否等于画网格时定下的个数
Toggle cell visibility (eliminate other colons : left with only labelIDs) -> export spread sheet *.csv -> optional depending on paraview version (filter colons by visibility)
modify *.csv : add OpenFOAM header (shown below), add ( and ) for list
use OpenFOAM to read modified file via class IOList<label>

// example of OpenFOAM header for file named "slice16"
$ head -10 slice16
FoamFile
{
    version     2.0;
    format      ascii;
    class       labelList; // IMPORTANT
    object      slice0;    // not important
}

16900
(
/*
 ...
*/
)

scripting

Base

利用Tools->Start Trace选上all properties Fully Trace Supplemental Proxies Show incremental Trace

Open -> some *.foam file (no need for the real file when running script afterwards, but necessary here for GUI use, to generate the script to run)
clip… slice…
export as
Tools -> End trace
pvpython script.py

Note

值得注意的是legend，利用以上python trace的结果不加改动的情况下，会默认变得巨大，所以得加上
加上auto-rescale是个必须得有的好习惯
以上1和2的改动放在renderView1之前，经测试是有效的

"""
some operations : read some certain array
"""
# Properties modified on t_meanLUTColorBar    调整legend nu_mean** 需要根据实际object名字替换
nu_meanLUTColorBar.TitleFontSize = 4
nu_meanLUTColorBar.LabelFontSize = 4
nu_meanLUTColorBar.ScalarBarThickness = 5
nu_meanLUTColorBar.ScalarBarLength = 0.5

# rescale color and/or opacity maps used to exactly fit the current data range  等同于auto-rescale
slice1Display.RescaleTransferFunctionToDataRange(False, True)

# current camera placement for renderView1    
renderView1.CameraPosition = [0.013999999035149813, -0.08839503035519257, 0.0]
renderView1.CameraFocalPoint = [0.013999999035149813, -0.0020000000949949026, 0.0]
renderView1.CameraViewUp = [0.0, 0.0, 1.0]
renderView1.CameraParallelScale = 0.022360679233547745

# save screenshot

customize range, logscale, use another color mapping 它们之间按照以下顺序排列是有效的

# Rescale transfer function
nu_meanPWF.RescaleTransferFunction(2e-06, 0.0003)

# convert to log space
nu_meanLUT.MapControlPointsToLogSpace()

# Properties modified on nu_meanLUT
nu_meanLUT.UseLogScale = 1

# Apply a preset using its name. Note this may not work as expected when presets have duplicate names.
nu_meanLUT.ApplyPreset('Yellow - Gray - Blue', True)

如果有多个不同位置的slice，那么一定要记得加上下面这一行(在save screenshot前就行)以保证图”有效部分”的大小不会改变

# reset view to fit data
renderView1.ResetCamera()

# save screenshot

possible bug

1 2	raise ValueError("%s is not a valid value for attribute %s." % (value, name)) ValueError: is not a valid value for attribute ScaleArrayComponent.

可能是最初没有读入后面要用到的数组，也有可能后面取slice什么的超出了计算域，感觉报的是个找不到目标数据的错

blender

一句话：通过paraivew做初期可视化，包括color map，导出后可通过blender调整camera和lamp. Paraview里面也有这个功能，但相对鸡肋.

blender version : 2.8 beta compatibility issue : glibc too old in CentOS

paraview -> visu -> File -> save Data -> *.ply (check coloring; check alpha : even if you dont have any transparency in paraview setting. This is important for blender/ or shall we say bug)
blencer -> File -> import -> *.ply
(optional but often needed) s0.01（导入的data通常会显得很大，需要缩小）: scale by 0.01;s90x以x为轴旋转90度；blender里面朝上通常为z
Now we have a render vie for data. Care now for coloring. -> choose blender render or cycles render
Add -> input -> attribut (the color attribute) : (i) name = Col ; (ii) connect “color” to “base color” of BSDF
如果import的数据是contour，可能会有尖角出现，光滑一下：select mesh->object->shade smooth (need to be in object mode : normally by defaut)
接下来就是调整camera和lamp了，最终blender出图是camera的视角，lamp可选太阳光什么的

Note : Gratitude to Juan Ignacio Polanco

svn

branching

video reference createBranch,workWithBranches,resolvingConflicts,svn_resolve_tree_conflict_in_merge

# Note a good pratice : make sure trunk is updated to the lastest version
# create branch by copying trunk. 
$ svn copy https://subversion.renater.fr/jnnf/trunk https://subversion.renater.fr/jnnf/branches/haining -m 'create branch haining'

# confirm existance of branch/haining in svn server
$ svn list https://subversion.renater.fr/jnnf/branches/ 

# get branch data from svn server
[branches] $ svn update # better than : svn checkout https://subversion.renater.fr/jnnf/branches/haining. This will give problems when doing svn delete at the end of checkList

# make changes on branch/haining, running tests
# if new file added : svn add
[haining] $ svn commit -m 'information on modification'

# make sure branch itself is updated 
[haining] $ svn update 

# now we are going to push changes to trunk. BUT
# firstly we have to merge from trunk to this branch (necessary step):
# possibly we may get some conflicts for THIS merge.
[haining] $ svn merge ^/trunk

# verify merge by running tests
# commit merge
[haining] $ svn commit -m 'merge from trunk to branch/haining is sucessful. ready to reintegrate into trunk'

# go to trunk
[trunk] $ svn update

# now re-integrate from branch/haining to trunk then managing possible conflicts (usually choose postpone and vim)
[trunk] $ svn merge --reintegrate ^/branches/haining

# verify again changes by running tests
# If all is well, we commit
[trunk] $ svn commit -m 'merged trunk from branches/haining'

# branches/haining is now useless
# thus remove them from version control meaning on the svn server. 
[branches] $ svn rm haining 
[branches] $ svn commit 'removing branches/haining'

# wont be able to see 'haining' anymore
$ svn list https://subversion.renater.fr/jnnf/branches/ 

# checking status :
[branches] $ svn status
?       haining        # ? means no longer in version control

resolving conflict

!M : svn rm file --force (if it is rm * not by svn remove)

out of date : svn update; svn resolved fileName (one by one) ; svn commit -m 'fix out of date'

svn和git之间相互转换

一定要非常注意！

如果是我的thesis，先make clean
cp -r拷贝整个文件夹（最好不要是根目录，因为包含.svn或者.git）到目的地文件夹
如果是根目录继续往下看
如果是svn拷贝到git，一定要删掉.svn ; 如果反之，一定记得删掉 .git (.gitignore倒是无所谓啦)
然后才开始进行其他操作

ubuntu in win10

Terminal默认不能输入中文，vim打开也会乱码，需如此配置:

Terminal上端right-click->properties->font，改为NSimSun : 这样在终端就可以敲出中文
vim 打开含中文字符的文本，:set encoding?如果不是utf-8`se:set encoding=utf-8`: 这样vim里面的中文字符就会正确解码
将以上设为默认right-click->defaut;.vimrc