Very large temperature as a result of the application of voltage

[DenPopov]

I have an aluminum wire (diameter 1 mm, length 100 mm).  Wire connected to the battery (2.5 V), as a result wire is heated. Wire located inside pipe with water (flow rate 100 mm / s, temperature 20 C), the water cools the wire. As a result of analyzing the temperature reaches 950 C. This is not a normal result. I attached pictures of my actions. What am I doing wrong?

My steps:

1) Assign materials. 

2) Assign the boundary conditions

3) Run Solver 

4) Result

[Jon.Wilde]

Hi DenPopov,

As an initial suggestion, I would say it is worth having a suppressed 'cap' on each end of the wire. Not likely to affect results but it is always good to avoid internal Boundary Conditions as you have here.

You also need a really excellent and uniform mesh along the wire - could you share an image to demonstrate how the mesh is set presently?

I think you may need to run with Advection Scheme 5 also.

You could try the SST turbulence model, which may help capture the heat transfer to the water a little more accurately.

Also, bear in mind that the flow will be fairly poorly developed as there is no upstream region allowing it to become fully devloped, which may affect the results.

Kind regards,

Jon

[DenPopov]

Picture showing a mesh model:

You gave me advice that will help improve the accuracy of the calculation. I think that these recommendations will not help. Error hiding in the other.

Experiments do only with wire without environment. The same wire - diameter of 1 mm, length 100 mm, aluminum material.

Experiment No. 1

1) I applied a material to object.

2) I applied boundary conditions. On one end of a wire temperature 10 C, and on other end 100 C.

3) I started a solver.

4) Results. Everything left well.

 

Experiment No. 2

1) I applied a material to object. (All just as in experiment No. 1)

2) I applied boundary conditions. On one end of a wire voltage 0 V, and on other end voltage 2.5 V.

3) I started a solver. (All just as in experiment No. 1)

4) Results. Temperature didn't appear. If I change the voltage from 2.5 V to 2500 V, the temperature is still not change. What could be wrong?

Experiment No. 3

1) I applied a material to object. (All just as in experiment No. 1)

2) I applied boundary conditions. On one end of a wire voltage 0 V, and on other end voltage 2.5 V. I apply temperature 1 C to one of the wire ends.

3) I started a solver. (All just as in experiment No. 1)

4) Results. Very large temperature!

[Jon.Wilde]

Would you mind sharing the CFZ file please?

Kind regards

Jon

[AstroJohnPE]

For experiment 2, it could be that heat transfer was disabled because either no thermal boundary conditions were found or the applied conditions are insufficient. At least, that's what it says in the message window on the second line after the ANALYSIS STARTED line!

For experiment 3, it could be

• the non-fatal warnings that occurred in the analysis. I do not see anything labeled as a warning in the message window.
• It could be poor convergence.
• If you are doing a steady state analysis and only remove the heat from one end (with the 1 C boundary condition), how hot should the rod get with X amount of power applied by the 2.5 V difference? I probably have a wrong formula or material property because I calculate 231 MW (231E6 W) of power being created. That would certainly cause the rod to get hot.

[DenPopov]

Wildej, I attached the file to the message. 

AstroJohnPE, I also think that the problem is that I didn't set the temperature in the boundary conditions. But I don't understand why there is big temperature. How you received 231 MW? I will lay out my calculations.

[Jon.Wilde]

Hi,

My suggestions still stand and I did not really understand your reply.

Advection Scheme 5

SST turbulence model (when running with water)

More mesh - this is a cross section of your wire, which should still look cylindrical when meshed - this usually has a huge impact on accuracy.

Kind regards,

Jon

[AstroJohnPE]

Thanks for the correct power calculation, but even 1818 W seems like a lot of power in a tiny space to me. How hot does a 40W light bulb get? The glass is certainly quite hot (hotter than 65 C is my guess). Since that has a lot of cooling (radiation and convection), the filament temperature must be much hotter.

Referring to experiment 3, you can calculate what temperature gradient is necessary to remove 1818 W from the end of the rod:

Q = (k*A/L)*dT = (k*A)*(dT/L)

1818 W = (204 W/mC)(pi/4)(0.001 m)^2 *(dT/L)

dT/L = 11.3E6 C/m = 11300 C/mm

That's a large temperature gradient!

I didn't want to go through the proper integration of the heat generation along the length versus the temperature gradient (as much fun as that would be), but a quick "back of the envelope" calculation where you assume the 1818 W is generated entirely at the middle of the wire gives this result:

1818 W = (204 W/mC)(pi/4)(0.001 m)^2/(0.05 m) *dT

dT = 567341 C.

It looks like CFD is calculating 567220 C. Not bad for a "back of the envelope" calculation!!!

So it seems plausible that your first calculation with the water cooling could be on the order of 900 C. I'm guessing that you did not include such effects as the water boiling, the material properties of the wire changing with temperature, and so forth.

[DenPopov]

I congratulate all on past holidays!

I had problems with message addition. Probably you received notices of the answer, but new messages weren't. Support service of Autodesk solved this problem, thanks!

I looked for the solution of the problem and received some results. I will describe the static analysis in Simulation CFD which is approximately equal to the analytical decision in Mathcad. It is good. But the dynamic analysis glitches. And I don't understand in what a mistake.

Task №1

There is a square pipe, the cross section of a pipe of 5х5 mm, length of a pipe doesn't matter. Water flows with a speed of 100 mm/s, water temperature on an entrance to a pipe 20 C. In a pipe the aluminum wire, radius of a wire of 2 mm, length of a wire of 50 mm is placed. What power (W) is necessary for a wire that water temperature increased on 50 C?

Analytical solution

I solved a problem analytically. I took properties of materials from Simulation CFD library.

Calculation showed that the power of 522 W is necessary for a wire.

Verification of the decision in Simulation CFD

Pictures of creation of settlement model in Simulation CFD:

Result of calculation in Simulation CFD:

From results it is visible that water temperature on the average increased on 50-55 C. Temperature of the top sheets of water is equal 90 C, in the center 70 C, in the bottom layers 50 C. If I made a pipe longer, temperature of all sheets of water would become identical. It seems to me that the analysis was successful. The analysis confirmed analytical calculation. If there are remarks, please tell.

Task №2

I want to make the dynamic analysis. Power of a wire changes in time. In drawings I will show, what changes I made to the previous analysis.

During calculation there was error! How to correct it? In what there can be a mistake?

[OmkarJ]

You have run 200 inner iterations but the timestep is 1 sec. Generally, it is recommended to reduce the timestep and use lesser no. of inner iterations, than running larger timesteps and running larger number of inner iterations so that you have adequate temporal resolution. Your timestep is same as the time for increase of heat geneartion. How about running say 0.5s and 100 inner iterations, or 0.25s and 50 inner iterations etc? Also, reducing the underrelaxation factors for T and other parameters may help too. Alternatively, you can have Intelligent solution control turned on. But this will mean the convergence will be very slow since timestep chosent will be very conservative. In transient analysis, more often than not, you can only be sure of the "optimum" timestep by observing how it progresses. You would want the global parameters to "flatten" just at the end of the inner iterations for each timestep. 

Also, regarding the steady state analysis, you would also want to check if you have used adequate fine mesh to capture the lengthscales and gradients of temperature. Hope you have done mesh sensitivity study.

[DenPopov]

Intelligent solution control was always enabled. I reduced the «time step size» and left a large «inner iterations» (time step size = 0,05; inner iterations = 200), but in this case there was an error solver. I increased the «Advanced Solution Control» (picture settings below), but this time the error solver.

What could be wrong? Mesh is fine enough, included «boundary mesh enhancement».

What do you mean decrease under relaxation factors for T and other parameters? Where can I make these changes?

How to make a mesh sensitivity study?

[OmkarJ]

You can not possibly know if the mesh is fine just by looking at it 🙂

Using very coarse meshes will introduce artificial diffusion and you may lose some transient and turbulent effects due to this, making it quasi-steady simulation  It may not be a a cause of divergence, rather, this will make your solution more stable, but more inaccurate. It is advisable to do mesh sensitivity analysis, wherein you have a converged result on mesh, refine it at critical areas to create second mesh and have a converged result on that as well. If these two meshes do not have significant difference in the results you are interested in, then you have a reason to say, it is "fine enough" and any further refinement will not give significantly different results.  AT the same time, if you keep refining the mesh beyond this point, it will capture very small unsteady turbulent scales and thigns start to become unstable. 

If you have  turned Intelligent Solution Control on, then Solver will ignore your timestep and calculate its own timestep (which is very small generally) depending on local CFL numbers. You do not need 200 inner iterations then . Have you tried reducing them? Will just acceelerate the solution, but it is likely not a cause of divergence.

The underrelaxation factors are given in "Solution Control" dialogue box, under manual control. (The fields which say 0.5 etc). In some cases you can improve the stability by reducing them.

Also, can you post image of your plots? 

[DenPopov]

Just wanted to write you that I've been experimenting with the settings window "Solution Control", which set the parameters from 0.5 to 0.1. Analysis was held without a mistake! Below is a picture of calculation settings.

But why the calculation is not complete? Calculation ended on time 4.42351. As seen in the previous figure, "stop time" = 10.

[OmkarJ]

You still haven't postedd the plots. You can find it under "Convergence plot" tab at the bottom.

You have entered the time steps to run as 100. Since you have enabled ICS, Solver has chosen smaller timestep than you specified. Hence 100 timesteps finished earlier. Specify a large number there,  like 1000000 so even with small timestep of Solver, you finsih upto required stop time. Also, in the "Advanced Solution Control" dialogue, deselect the "Automatic Convergence Assessment". Often that is a cause of premature stopping of iterations, at leasst in steady state. I never ever turn it on, and always judge the convergence manually.  

Few thoughts:

1) Analysis completed doesn't mean it is accurate. IT just "calculated something". You would need adequate time and mesh resolution along with proper boundary conditions for accuracy. While timestep seems to be taken care of by ICS automatically, your meshcount is too small (112k). I wouldnt trust any result for such a coarse mesh. You would wnat to do mesh sensitivity for a steady state as I mentioned before.

2) You don't want all factors to be 0.1, as this will slow things down. Try slowling them down gradually, adn stop when things start working. You want their values as large as possible, without divergence.

[Jon.Wilde]

The other issue here is that you are running transiently with Intelligent Solution Control on, which can (likely will) stop the analysis early. Turn this off and the analysis should run for the full time you desire.

You also have a Stop Time and Timesteps To Run set. CFD uses one or the other, set one to -1 so that it is ignored.