Extreme temperature and solver exited unexpectedly

[Anonymous]

Hi everyone,

For two days now, I am experiencing troubles with my CFD calculation:

• I try to assess a natural ventilation (solar chimney);
• I followed precisely these steps: https://knowledge.autodesk.com/support/cfd/learn-explore/caas/CloudHelp/cloudhelp/2014/ENU/SimCFD/fi...
• I can see within the materials the temperature rising a lot. Also, no air movement can be seen within the building (opened at the bottom and at the top as it is explained in the link above). And while the calculation is in process, I see the max temperature reaching incredible values (14000°C), then the solver stops unexpectedly.

I have a young experience w/ autodeskCFD, so for sure I am modelling something wrong. But could someone help me?

Best,

[frederic.gaillard.7]

Hello @Anonymous, 

For the rising temperature problem use a manual control in the solution control tab. 

1. Change the temperature slider bar to 0.5 (instead of 1.00)
2. clic on 0.001 (1e-3)

When i had unrealistic temperature in my model i change the relaxation factor. Usually it works but it takes more time to solve. Not sure if you have to change both of them, but this solution work for me.  
You should confirm with an autodesk expert to have a more accurate answer. 

here some link that might help you 

1. Autodesk Manual Convergence
2. Relaxation Factor

Hope it helps 
Fred

[bob.schlosser]

Hello,  it would be helpful if you attached the simulation file for others to take a look.  One red flag you mentioned is that there is no air movement.  Check that the air is set to 'variable'

[Anonymous]

Thanks a lot frederic.gaillard.7 and bob.schlosse,

I've started new calculation with your technic, Frederic. I'll send you back a file if needed. I keep you informed.

Again, thank you very much.

[Jon.Wilde]

Agree. We can alter the relaxation but should only really need to if we have solver instability.

I think there is something fundamentally wrong in the setup here. Can you share the file?

[Anonymous]

Dear frederic.gaillard.7,  bob.schlosser & Jon.Wilde,

 thank you very much for your answers.

 I've tried all day long to solve my problem but I still have an unbelievable rise of temperature, and air movement are strangely low. I changed my air material to Variable air material, as it is recommanded for convection assessment.

I am looking forward for reading your answers.

 Best,

[Jon.Wilde]

Happy to assist as I am sure the others are too 🙂

Could you share a CFZ file though please? We need only that one.

[Anonymous]

Excuse me for the late answer.

I think I arrived to something nice, but I had to use the relaxation factor reduction.

Let me know if you think it is OK.

Looking forward for reading your answer.

Best,

[Jon.Wilde]

There is quite a bit that needs to be different here. 

Could you alter the air volume so that the building is not flying? This would mean you need to draw it in CAD.

We cannot have any internal boundary conditions - all of those need to be removed.

The air volume should only have one P=0, at the far end and not at the sides.

You must leave Intelligent Solution Control on and I would not recommend lowering the relaxation parameters...

[Anonymous]

Thanks a lot!

Which air volume? Do you mean the internal one? Or the external box?

I test your solutions and answer as soon as possible.

Best,

Jean

[Jon.Wilde · Accepted solution]

The large air domain, the biggest one. Needs creating in CAD so that the building is on the floor. You might also need to model a ground thickness too then, so some of the heat from the sun can be absorbed here...

Also, there should only be boundary conditions attached to this and nothing else.

Inlet 

Flow

Temperature

Outlet 

P=0

Walls

Slip

[frederic.gaillard.7]

Hi John, 

Can you told us why it's not recommanded to lower the relaxation factor ? 

- does it affect the solution convergence ? 

- lowering the relaxation factor induce unrealistic result ? 
I have the same problem as jean had but in a transient solution mode. 

Thx 
Fred

[Jon.Wilde · Accepted solution]

You can lower it and should achieve identical results, it will just take longer 🙂

You might need to tighten (lower the value of) the convergence assessment as smaller changes would happen from one iteration to the next. This would ensure that CFD does not converge too soon.

Sometimes it is really necessary, but rarely. Personally, I try to avoid it as it takes more time.

One time I do often use it is if I have a fan material with a fan curve. CFD can produce a saw-tooth convergence plot as it hunts for the fan performance point, lowering the relaxation parameters can avoid this.

Does that help?

[frederic.gaillard.7]

Yes it help ! 
Specially in my case because it involves a material fan with fan curve. 
Thank You 

[Anonymous]

Thank you very much Jon Wilde, you've been very helpful!

I tried this morning & it worked very well.

Have a nice week.

[Jon.Wilde]

You are most welcome, thanks for letting us know.

Hope you enjoy CFD! 🙂

[Anonymous]

Yes, I enjoy CFD 😉

I would add one question before ending:

• I don't understand clearly the slip/symmetry boundary.

You've seen my model: I extracted this part and created two walls (+y and -Y) to model only a part even if the building is longer in these directions with the internal air volume opened on the rest of the building, on both side with the same chimney. This morning, once again I've tried to model it w/ boundaries slip/Symmetry instead of these walls (see below). Would be more accurate. The thing is that it can't work. I already had this dilemma and I tried to understand the logic of this "circular symmetry" as explained on the website. But honestly, I can't get why in my case it couldn't work.

Could you explain me?

Best,

[Jon.Wilde · Accepted solution]

For the sides of the domain, just use a velocity in the direction of the flow (switch to components rather than normal when assigning). That keeps the flow moving nicely.

We end up with radiation being mirrored all over the place if we have more than one slip/symmetry condition. Does that help?

(I can't explain it with regards to what is going on in the code but hope this is sufficient).

[Anonymous]

OK, I get it!

And to add this lateral boundary condition helps a lot.

Thank you very much.

Best,

[Anonymous]

Dear Jon Wilde,

I come back to this comment.

I don't understand why you do not recommend to use the boundary "film coefficient" in my case, over the roof for example. I've tried to understand, but I still don't get it. Could you shed light on this for me? What I understood is that you use it only if there is no external air volume, is this it?

Thks,