Hello evrybody

i am simulating molten steel flow inside a rectangular vessal using k-epsilon model i got a small problem .After around 1500 iteration i am getting the problem like "Temparature is limited to 1.000e06 in certain cell in zone 2 in domain"

can any body help me please

very much thanx in advance

bye

Hello

I'm just guessing here put are you using a heat flow. If you have put a positive heatflow in to the model, heat coming in, you can have this kind of problem. I mistakenly put the wrong sign to my heat flows in my calculation (+ in place of -) and got a reposrt like this.

Tuomas

hi Thanx for ur response

But in my problem molten steel at high temparature of about 1873 is coming with a velocity of (-0.3875m/s) so i think i have given evry thing fine .i am very much pleased if u have any other solution

bye

Sorry, that is all I have, but it certainly seems that from somewhere there is coming extra heat to your system and temperature rises to high for fluent in some cells.

If I may ask why is your incoming velocity negative?

Tuomas

i got similar problem. I'ven't added any heat or whatsoever to beside the problem setup, which doesn't include any heatflow. I even have fuel injection. P1-model and energy eqn also failed after 100 iterations. what's going on. is there anyway where I can limit this temp values?

I think without this limitation your residuals would have diverged.

So, Re-initialize your temperature field, and decrease the under-relaxation factor for the energy equation~0.1-0.5(depends on the problem).

Start your calculation (witout flow better)...

then after few iterations or time steps, if you do not have the same message, increase slowly the the under-relaxation factor to increase convergence speed...

I hope this will solve the problem

Hi,

What Cp values are you using?

i got similar problem. I'ven't added any heat or whatsoever to beside the problem setup, which doesn't include any heatflow. I even have fuel injection. P1-model and energy eqn also failed after 100 iterations. what's going on. is there anyway where I can limit this temp values?

the Cp values are not constant. all for species are piece-wise polynomial. hey, Kharicha I'll reduce it to .1 since I already done that for 0.2. The problem is few iteration say first 100 are alright, and then diverges afterwards. so I'm wondering if increasing it will make a diffference since P1-model and energy eqn blow off.

If Cp is strongly varying with temperature between t1 and t2, you should verify that you have enough meshed the area of your domain where the range t1-t2 is likely to occur.

Do the same for the other parameters wich depend on the temperature field as thermal conductivity and density.

Sorry that i keep asking. I do not know the backgroud case setup for your work. I guess you are running simulation for a reacting flow. What combustion model are you using? Is your flow laminar or turbulent? If you are running a turbulent flow and you are using the finite rate chemistry model, then this could be the source of the reason why your temperature is diverging. The finite rate chemistry model doesn't seem to work for turbulent reacting flows. The model is unable to predict the turbulent burning velocity and it in fact over-predicts it by a factor of about 5-6. Also, if your flow is turbulent, then Da<1 and chemistry is slow. However, the temperature sensitivity of the rate of reaction of the finite rate chemistry model makes the rate very sentitive to small temperature changes.

James

well, it's turbulent and NOT using finite rate chem but rather EDC. is not only temp that blow up but also the dissipation rate. however, the temp starts first. all these occur after 100th iteration. before that every thing seems alright and the radiation-model(P1) looks okay. but just after the 100th iteration, it turns to blow up. okay, I'll try injecting the fuel within longer iteration and see what happens.

thanks a lot by the way to all you guys!!!

hi Toumas Hirsi

velocity is negetive sign because steel is coming in negetive Z direction

Hi Srinivas

The problem is due to meshing. At a particular cell zone, the temperature is increasing. You can see the same, using clip range in the contour plot of temperature and identify which region is having bad mesh, try to refine the mesh in that area and you can remove this error.

hi Gopal

Can u tell me how to refine the mesh?

one more thing is that i am getting the converged solution for the same mesh when there is no bouyancy effects. Thanx alot in advanse

Hi srinivas

It is clear that your solution will converge. Only culprit is your cel 19879, where due to some uncertainities with neighbouring cel, the temperature value will go high. This will reflected in your results only. where you will get a wide range of max and min values. If you clip to the range, then ur result will seem to be okk.

For refining that, better try to find the above cel giving problem..using grid zones panel and refine the mesh in that area alone...

PS: while iteration you should not get this msg: Temparature is limited to 1.00000 in 19879 cel in the FLUENT window

Hi Gopal

Many Thx for your valuble suggestions.And i may be bothering u by keep on asking questions.Do you think it will works better if i again model the geometry with more number of cell elements? or could you plz tell me how to find which cell is giving problems?is it purly by observation? or is there any simple thumb rule?

And what aill happen if i got this problem Temparature is limited to 1.00000 in 19879 cel in the FLUENT window

Thanx alot

Um... that's not Cell #19879... that says that the temperature is limited to 1 in 19,879 cells. There are almost 20 thousand cells that have hit the temperature limit.

There are a lot of things that can cause this. The most common one is poor mesh. Bad boundary conditions are also a common cause.

As far as looking at the problem, you can plot the temperature contours. Turn off nodal values, choose "default_interior" under the surfaces command, and then limit the range you're plotting on. If it's being limited to 1K, then plot the range of 1 to 100K (molten steel should be MUCH hotter). You'll probably want to turn on your grid as you're looking at the results in order to get a reference frame. Once you know the problem region, you can start trying to figure out what's causing the problem.

Good luck, Jason

Hi...

You can go through tha jason reply...he has clearly described the way to identify the cell giving problem.

Remodelling is not required. If you have one or two zones(this you can find from the fluent window while iteration) giving this problem, you can refine mesh in thar region along.

If the zones are too many, like 20000 than it is good to go for remeshing instead of remodelling.

As i found boundary conditions has little to do with this problem. You can verify it by cliping the range in the contours to the expected value of the results...you will get the results you expected....

have a nice day

HI Gopal And Jason

i am very much thankful for your valuble suggestions.Really it's wonderful experiance to get in touch with u.

Thx alot bye