[jpina]

Hello,

I’m reading the pag. 34 of this PhD Tesis*

And it says that “a constant heat transfer coefficient is used for the thermal boundary condition. The value of the coefficient was chosen so that simulated replications matched the experimental values using reverse engineering.”

As far as I know, when simulating a flow using a multiphase model, it is NOT possible to set the heat transfer coefficient constant between the wall and the fluid, because it is calculated at each time step.

I have contacted the author and he said me that he set the h value constant.

I use ANSYS Fluent and I really think that this is not possible, is it possible in CFX? As far as I know, it is not!

I will appreciate your help!

*https://www.google.es/url?url=https://www.sintef.no/globalassets/project/mpc/tofteberg_phd_2009_web.pdf&rct=j&frm=1&q=&esrc=s&s a=U&ved=0ahUKEwjPo_3XkOjLAhXBDxoKHVx4CjwQFggXMAE&u sg=AFQjCNFL-I9UFbQp3U0s1mZRAHeYmkWy-w

[ghorrocks]

This is possible in CFX and Fluent. This is a basic boundary condition which is commonly used.

You appear to be confused with interface boundary conditions where the heat transfer at the interface is calculated from the flow conditions, so the user does not specify a heat transfer coefficient (htc) value. But for external walls all CFD solvers I know of offer the option to set a htc.

[jpina]

Dear gorrhocks,

what the paper says to set constant, is the h between wall and internal fluid, not between wall and external fluid.

[ghorrocks]

You can set a heat transfer coefficient on a wall boundary on a fluid or a solid domain. You cannot set a HTC on an interface, as mentioned in my previous post:

You appear to be confused with interface boundary conditions where the heat transfer at the interface is calculated from the flow conditions, so the user does not specify a heat transfer coefficient (htc) value.

If I have misunderstood your question please explain it more clearly, preferably with an image showing what you mean.

[jpina]

Hi,

thanks for the interest.

We have the following geometry:



And in the paper the author says to set the heat transfer coefficient of flow-wall to a constant. I don’t think it is even possible, because this internal h coefficient is calculated. I know that I could set an external h with the environment, but what the author says to have done, is to set the internal h to a given value (5000W/m^2/K in his case).

[Opaque]

Please read the documentation section about

Chapter 4: Turbulence and Near-Wall Modeling | 4.2. Modeling Flow Near the Wall | 4.2.4.1. Heat Flux

You can override the internal calculation of the Wall Heat Transfer Coefficient. If the properties are constant, you may get away with it. For variable properties, there may be consistency issue between the hydrodynamic and thermal boundary layers that must be satisfied. Good luck

Hope the above helps,

[jpina]

Hello guys,

you put me in the good way and I've finally found how to do it with Fluent, I copy the documentation for the people of the future!

After a lot of research, I've finally found how to set a constant heat transfer coefficient. I copy what I've found and used:

5. Wall Heat Flux

The wall heat flux function ( DEFINE_HEAT_FLUX) can be used to modify
the way that the solver computes the heat flux between
a wall and the neighboring fluid cells. For example, you can customize
the heat transfer coefficient or the law-of-the-wall for
temperature. The UDF presented below uses an internal heat transfer
coefficient to specify the wall heat flux. It is another example
of a UDF that utilizes the ADJUST function to adjust a computed value,
and it is executed as a compiled UDF.

The diffusive heat flux coefficients ( cid) are specified in this UDF.
The diffusive heat flux ( qid) will then be computed by
FLUENT using the following equation:

qid = cid[0] + cid[1]*C_T(c0,t0) - cid[2]*F_T(f,t) -
cid[3]*pow(F_T(f,t),4)

/************************************************** *********************/
/* UDF for specifying the diffusive heat flux between a wall and
*/
/* neighboring cells
*/
/************************************************** *********************/

#include "udf.h"

static real h = 0.; /* heat transfer coefficient (W/m^2 C)
*/

DEFINE_ADJUST(htc_adjust, domain)
{
/* Define the heat transfer coefficient. */

h = 120;
}

DEFINE_HEAT_FLUX(heat_flux, f, t, c0, t0, cid, cir)
{
cid[0] = 0.;
cid[1] = h;
cid[2] = h;
cid[3] = 0.;
}

[Rashi]

Hi,


Sorry for the noob question. How do I input UDF to an interface?
Do I have to de-couple the interface to do so?


TIA


Cheers,
Rashi

Originally Posted by jpina

Hello guys,

you put me in the good way and I've finally found how to do it with Fluent, I copy the documentation for the people of the future!

After a lot of research, I've finally found how to set a constant heat transfer coefficient. I copy what I've found and used:

5. Wall Heat Flux

The wall heat flux function ( DEFINE_HEAT_FLUX) can be used to modify
the way that the solver computes the heat flux between
a wall and the neighboring fluid cells. For example, you can customize
the heat transfer coefficient or the law-of-the-wall for
temperature. The UDF presented below uses an internal heat transfer
coefficient to specify the wall heat flux. It is another example
of a UDF that utilizes the ADJUST function to adjust a computed value,
and it is executed as a compiled UDF.

The diffusive heat flux coefficients ( cid) are specified in this UDF.
The diffusive heat flux ( qid) will then be computed by
FLUENT using the following equation:

qid = cid[0] + cid[1]*C_T(c0,t0) - cid[2]*F_T(f,t) -
cid[3]*pow(F_T(f,t),4)

/************************************************** *********************/
/* UDF for specifying the diffusive heat flux between a wall and
*/
/* neighboring cells
*/
/************************************************** *********************/

#include "udf.h"

static real h = 0.; /* heat transfer coefficient (W/m^2 C)
*/

DEFINE_ADJUST(htc_adjust, domain)
{
/* Define the heat transfer coefficient. */

h = 120;
}

DEFINE_HEAT_FLUX(heat_flux, f, t, c0, t0, cid, cir)
{
cid[0] = 0.;
cid[1] = h;
cid[2] = h;
cid[3] = 0.;
}

[ghorrocks]

CFX does not use UDFs. They are a Fluent thing. If you are using Fluent then you should try the Fluent forum.

If you want to put a source term on a boundary interface that is easy, you can do that in the GUI. No user function is required (unless your function is too complex for CEL).