various temperature in shell element 1

[mehrafarid]

Why the temperature are same in heat transfer analysis for depth of shell element? The integration point in slab was defined 5, Then I should have 5 different temperature.

 

[corus]

It would depend on whether you had heat flow from the surface. No heat flow - no temperature gradient.

Tata but not yet tara

 

[mehrafarid]

I think that I did find it.
I have slab with fire in below level (not top). Then I defined heat flux in load from below surface.
with steady state I got no temperature variation but when I changed to transient it gave me different temperature.

But now question is I defined 20C for predefined in initial step. my steps is until 4860 second. In middle depth of slab I see temperature changes from 20C in 0 sec. and decreases to 18C and after that goes up. I think that the temperature should not be decreases !!!
I defined concrete with 2400 kg/m3 , specific heat: 900 and conv. 1.6 in SI

 

[corus]

I don't think a shell element is the right kind of element for carrying out a transient thermal analysis, especially on what must be a relatively thick piece of concrete. Use 2D or 3D elements that would model the thickness.

Tata but not yet tara

 

[mehrafarid]

Thank you for your time.
1. I do not know, for 4 hours fire that temperature is varied by time, should I use STEADY STATE or TRANSIENT?

2. When I use STEADY STATE, the temperature in depth of concrete (250mm) is the same for all integration nodes (NT11,NT12,NT13,NT14,NT15)

3. Can I use shell element for 250mm concrete slab? I think YES

 

[corus]

The reason why you get strange temperatures is because you don't have enough nodes through the thickness and the results are unstable.

It's always wise to verify your answers by other means. Try a 1D model with lots of nodes through the thickness and compare the results with your shell model. Personally I wouldn't believe results of a transient thermal analysis from a shell model, but that's up to you.

Tata but not yet tara

 

[mehrafarid]

Thank you for your time.
I think I should use steady state. Then why I have the same temperature in depth of shell element.
I defined 5 integration point in 250mm slab with shell element.I use surface heat flux in bottom surface of slab as a load.
In bindary condition I use a table with temperature variation from 20C to 1200C during 4860 sec. and NT11 is realease for temperature.

 

[corus]

If you use steady state then why use temperatures that vary with time? If you're defining a heat flux on a surface together with fixed temperatures (albeit varying with time) then only the fixed temperatures will be used. You can't have both. Make sure that you define surface conditions on the positive and negative sides of the element, otherwise you're defining adiabatic conditions for one surface, and hence no heat flow across the shell (in steady state).

Tata but not yet tara

 

[mehrafarid]

Thank you again

My temperature must be varied with time from 20C to 1200C between 0 sec to 4860 sec.
--------------------------------------
As I understand in your email: I must have transient (not steady state) because temperature is vary. OK?
--------------------------------------
Temperature is from below of slab.
for heat flux (in load):
I put magnitude: 1 and amplitude: the default Instan... correct?
should I use bottom surface or top & bot.?
---------------------------------------

 

[corus]

If you apply varying temperatures to the bottom then you can only apply the flux to the top surface. It'll be instantaneous if it acts instantaneously.

Tata but not yet tara

 

[mehrafarid]

I apply varying temperature from below (By Degrees of freedom: 11), the temperature is varied with time.
Heat flux is from top surface (Magnitude:1 Amplitude: Instantaneous)

But I see for NT14 and NT15 the temperature goes down and after goes up. NT11 shows correctly but NT14, NT15 not.


I attached my file (SLAB-HEAT TRANSFER model)
Thank you in advance

 

[corus]

The model you provided is a static, general model which doesn't calculate temperatures. On top of that you have no thermal properties, other than specific heat defined for one material. I think you've also defined two materials for the same regions, ie. concrete and steel.

Tata but not yet tara

 

[mehrafarid]

No... the file that I sent it has 2 model.
The second model is for heat transfer (not first model)
My problem is for heat transfer model (second one).After it will be solved, I think the static model will be OK.

Please see the second model with name of SLAB-HEAT TRANSFER model.

Thanks again

 

[corus]

Ok, found it. As I said before, with a transient you will need more nodes through the thickness, or with a shell model, more section points. As it's essentially a 1D problem (thermally) I'd check your results with a 1D or 2D solid thermal model that reprsents temperatures through the thickness.

Tata but not yet tara

 

[mehrafarid]

Thank you Mr. corus
I changed 11 integration point instead of 5 points and now it is correct.
I checked the temperature output with hand calculation and SAFIR software and it is approximately OK.

Thanks again

 

[Hipp53]

Mehrafarid,
I am trying to model something very similar to your discussion on various temp. in shell element for a research project. I looked at your slab model and I have a question regarding the rebar. As you know, you can not use rebar in heat transfer analysis. I see that you neglected it in this part of the model. However, you used it for the structural part. I am not sure how the model understands the degradation of the steel due to heat. Also, when I try to run the structural part of your model, I come up with an error that reads:

The number of temperature points 10 for beam or shell section found on the output database is larger than in the current model. This number must match between models.

Can you explain this error and how to avoid it?
Thank you so much for your help!