温度换热系数边界条件如何设置？

OpenFOAM
1

在ansys中计算温度时可以采用换热系数和环境温度的边界条件：
11111
在openfoam中如何实现这个边界 ？

2

看看这个能不能帮到你

externalWallHeatFluxTemperatureFvPatchScalarField Class Reference

3

看了下这个条件，如下设置，

 wall
    {
        type            externalWallHeatFluxTemperature;
        mode            coefficient;
        Ta              constant 300.0;
        h               uniform 10.0;
        kappaMethod     solidThermo;
	value           $internalField;
    }

提示如下错误：

Create time

Create mesh for time = 0


SIMPLE: No convergence criteria found

Reading field T

Reading transportProperties

Reading diffusivity DT

No finite volume options present

Calculating temperature distribution

Time = 0.005



--> FOAM FATAL ERROR:

    request for solidThermo thermophysicalProperties from objectRegistry region0 failed
    available objects of type solidThermo are
0()

    From function const Type& Foam::objectRegistry::lookupObject(const Foam::word&) const [with Type = Foam::solidThermo]
    in file /home/ubuntu/OpenFOAM/OpenFOAM-6/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 193.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::error::abort() at ??:?
#2  Foam::solidThermo const& Foam::objectRegistry::lookupObject<Foam::solidThermo>(Foam::word const&) const at ??:?
#3  Foam::temperatureCoupledBase::kappa(Foam::Field<double> const&) const at ??:?
#4  Foam::externalWallHeatFluxTemperatureFvPatchScalarField::updateCoeffs() at ??:?
#5  Foam::fvMatrix<double>::fvMatrix(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::dimensionSet const&) at ??:?
#6  ? at ??:?
#7  ? at ??:?
#8  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#9  ? at ??:?
"log.laplacianFoam" 64L, 2213C
4

For

SIMPLE: No convergence criteria found

Please check your system/fvSolution file having

SIMPLE
{
    nNonOrthogonalCorrectors 0;

    convergence          1e-4; // This is the convergence criteria
}

For

No finite volume options present

You need a constant/fvOptions file, please refer to file tutorials/heatTransfer/chtMultiRegionSimpleFoam/heatExchanger/constant/air/fvOptions

for

    request for solidThermo thermophysicalProperties from objectRegistry region0 failed

I guess you defined kappa to be computed in a wrong region. Check your regionProperties file.

Can you provide the following info,

  1. Which OpenFOAM version?
  2. What are the files thermophysicalProperties and regionProperties in your case?
5

问题描述：固体传热，一个圆柱，底部给定温度300，侧面和顶部给定换热系数和环境温度。因此其实只用到Ta和h就行了。openfoam版本是：openfoam6。如下设置
image
simple中也加了convergence参数：
image
提示错误如下：

image
image736×305 6.28 KB

1）fvSolution中simple的参数convergence好像不起作用
2） 只算固体传热，只用Ta和h，这个kappaMethod是干什么的？不用不行？如果加上KappaMethod，就会出现我第一个帖子中的问题，但是我这个case没有内热源等源项，不需要fvoptions。

这个是我的case文件，请帮忙看一下。
https://www.lanzous.com/i2ivdrg

6

你使用的求解器 laplacianFoam 只能计算简单的传热，对于这一个 case ，不能满足你的要求，也就是说 laplacianFoam 所包含的模型不能处理这一复杂的边界。

要做这样一个模拟，可以：

  1. 如果只是固体传热部分，可以根据 chtMultiRegionFoam 来修改。
  2. 如果用 chtMultiRegionFoam 来做 solid 传热，处理起来会比较复杂。