[h0rst]

Hello everybody,

is it possible in fluent (as it is in Ansys Classic: kxx, kyy ,kzz) to make the thermal conductivity direction-dependent?

I want to simulate the heating of a rotating part and I want to simulate as if the rotation is infinit.


Best regards
h0rst

[LuckyTran]

Yes. When you define the materials, use the anisotropic option. It will pop up a menu where you enter the matrix coefficients.

[Jiricbeng]

Yes, but you have to have pressure based solver, not density based. It does not work with density based solver.

[h0rst]

Thank you very much!

Fortunately, I am working with the pressure-based solver :-)

[h0rst]

I just tried to implement it but the problem is, that I have a cylindrical workpiece where the central axis is the Z-axis. So, I want infinite thermal conductivity in tangential direction around the z-axis (therefore, I need to use cylindrical coordinates).

How can I implement that?



Best regards
h0rst

[LuckyTran]

I must say that is a very exotic conductivity. If your physics is 2D, then use the 2D solver. Do you actually need infinite tangential conductivity?

You will run into other issues with infinite conductivity (an upwind scheme will not be appropriate, you would need to switch to a central scheme but only in that direction).

Finally,Fluent is an x,y,z solver. You will need a dedicated r,th,z solver.

I think you are trying to implement an infinite tangential conductivity as a workaround for a different problem. Maybe you can describe the actual problem and we can find an actual solution to the real problem.

[h0rst]

Hello LuckyTran,

attached is a picture of the actual situation.

I am pushing a current with a high amplitude and frequency through the copper coil which creates a magnetic field and heats up the workpiece in the middle by induction.

For getting a homogenous temperature at the surface, the workpiece rotates very fast. Since I want to neglect the influence of rotational speed, I want to set the thermal conductivity of the workpiece in tangential coordinates to a very high value which is like infinite.

I cannot do this simulation in 2D because I also want to consider the temperature in the corners of the coil.

I am calculating the W/m³ in Ansys classic and export them by udf to fluent. If I calculate also the thermal model in Ansys Classic (and neglecting fulid mechanics), I can easily switch to cylindrical coordinates and then set the conductivity to a very high value.

Now I am searching for a similar solution in Fluent.


Best regards
h0rst

[h0rst]

Hello again,

I tried to set orthotropic conductivity as cylindrical orthotropic and have set in tangential coordinates a very high value which actually creates a high conductivity in tangential direction. The problem is now, if I set this value very high, then the model does not converge and the results are bad. If I set it not that high, then the conductance in tangential coordinates is not enough to have a homogenous surface temperature in tangential direction.

Does someone have an idea how to solve this problem?


Best regards
h0rst

[Kontestator]

Hi h0rst,
Currently I'am dealing with isotropic model too. What I noticed is that when you have tetrahedral mesh the anisotripic model tends to 'explode'. By explosion I mean temperatures reaching infinity. So result obtained this way are useless. Moreover, the mesh quality doesn't matter. I tried basic geometry with very good tetra mesh and improving quality doesn't solve problem at all. On the other hand hex structural mesh works in the same case perfectly.
To sum up, if you used tetra mesh, try structural mesh instead. Probably there are fundamental reasons explaining that, but I figured it out by trying and failing because I haven't found materials describing this problem.

Regards

[h0rst]

Hello Kontestator,

I changeed the mesh to a structured mesh and tested with ortotophic model and very high tangential conductivity (10e6) and now it works!

Thank you so much!

[nhattan121]

Hi h0rst,

I have a same problem, but opposite - problem.

In my simulation, if i set thermal conductivity in radial direction too small (~0.05), it divergence. And else, if i set ~5, it converge very good.

Im using hecxa mesh. Should i change to tetra mesh?