Temperature result for shell 1

[Irwin]

I made a very simple analysis. I created 1 shell element and I applied on the face 1 (top surface) a temperature and a konvektion and an another temperature/konvection pair to the bottom face (face 2). I got a temperature value for the element. The question is: what is the meaning of it?
(I made a control analysis with a solid element. The result for this element is different.)

Irwin

 

[corus]

For shell elements you generally obtain the temperatures at the surfaces or at the mid-point depending on what you've asked for or what the default is.

corus

 

[Irwin]

-Is it possible to use it for something? I mean I would like to make a simple pipe model (with big diameter and small wall thickness) with this elements. Pressure and temperature will be apply on it! Can I use shell structure? Any experience?
-Can I use any option to write temperature on top and bottom surface at the same time?

Irwin

 

[prex]

Why not? They are there just for representing thin wall structures.
As far as the temperature is concerned, it depends on the options you have available in your code. If it allows to enter separate top and bottom temperatures, then you are calculating the stresses due to thermal gradient through thickness.

prex

http://www.xcalcs.com

Online tools for structural design

 

[Irwin]

Can somebody send me a NASTRAN (FEMAP) example about this? My problem is: I tried to compare the results with the solids, but maybe I made a mistake! I have just one temperature on each node and this will be transfer to the structural analysis, therfore no effect from the temperature difference of the top and bottom surface! During the pos-processing the FEMAP shows 2 temperature values too, which are existed outside, but this is not plot able! So again the question:
How can I calculate the temperature on the top and bottom of a shell element? How can I transfer this to the structural analysis?

Irwin

 

[jte]

Irwin-

Have you considered a hand-calc to determine this? I believe what you'll find is that you have a 2 degree temperature difference from the ID to the OD of the pipe. This will result in about zero impact on a three dimensional yield criteria such as Von Mises or Tresca.

I'm not familiar with FEMAP/NASTRAN but sounds to me like you are applying the temperature directly to the nodes. That would typically not be a correct way to apply the temp for a convection model. What you need is the convection coefficient with the fluid temperature applied to one face and another convection coefficient and fluid temperature pair applied to the other face.

The same would apply to your solid element model: If you are applying temperatures directly to your solid element nodes you are effectively forcing that surface to the applied temperature. Now step back a minute and ponder how much heat will transfer if your surface is the same temperature as the fluid... What's your delta-T?

jt

 

[corus]

I'm not sure where jte gets their figures from as I see no indication in previous posts on how to calculate the temperatures. Irwin, I believe, has applied a heat transfer coefficient with an ambient temperature so their results will be valid.
I, too, haven't used Nastran, however most codes are similar. In ANSYS it used to be the case that temperatures were input as TTOP and TBOT. In Abaqus you can have several temperatures specified through the thickness. These are identified as NT11, NT12 etc. Perhaps Nastran also identifies the calculated temperatures as separate variables which you can then plot. Input to the stress model will be a simple matter of specifying these variables. Note that I recall in ANSYS that if you msitakenly left one variable out then you effectively had a temperature gradient through the thickness of TTOP instead of TTOP-TBOT.

corus

 

[Irwin]

I applied the temperature and the convektion too on the shell element top and bottom. After the temperature analysis in the next step, I transfered the temperature results to the structural analysis. It seams for me, only node temperature is able to transfered to the structural model! This is my problem one side! On the other side I could not find any option for the output of the temperature fields on top and bottom!
Additional question according to the other code: Can any code calculate structural results from the effect of the temperature difference of the top and bottom surface of the shell elements?

Irwin

 

[ThomasH]

Hi

What type of Nastran are you using?

Since you say Nastran/Femap it might be MSC.Nastran for Windows and as far as I know it can't do temperature gradient. Femap writes a uniform temperatur (expansion) card and you can't change the bulk data in N4W. But Nastran (NEi, MSC and probably NX) can do this, the "problem" is in Femap.

Look in the manual for the TEMP commands in the bulk data section.

Good Luck

Thomas

 

[jte]

corus-

Where do I get my figures? Simple: SWAG. But I'd be curious to see just how much delta T there is between the ID and OD of the pipe with Irwin's process fluid on the inside and uninsulated convection on the other... I'll bet my 2 degree number is within 5 degrees of the result. The SWAG is based on the several times I've run this (Mathcad) calc myself for steel pipes/vessels in refinery service.

Irwin-

I'm still not clear on whether you applied your temperature as a bulk fluid temperature for the convection (good) or as a nodal temperature (not good). Once you've run the thermal analysis you'd read in the calculated nodal temperatures into the structural model for the thermal stress evaluation. I don't think the programs I'm familiar with would handle through thickness delta-T loadings with their shell elements. I'd have to go with axisymmetric or solids.

Can you be specific and post the actual numbers you are using for temperature and convection and conduction and pipe diameter and thickness? Just out of curiosity...

jt

 

[Irwin]

I am using NX/NASTRAN. (This is same with an older MSC/NASTRAN.)

Again from the begining. ;-)
Just one shell element! I can apply on the top and on the bottom different temperatures and convections. It looks the NASTRAN calculate something. The results are nodal and/or elemental temperatures, but there is a remark/information in the output selection window that the highest and the lowest value is something, which are not plottable! My problem with this temperature is that the temperature result is not understandable for me.
For further analysis I can use a nodal temperature field from a result file, therfore I can not use this type of result.
I would like to know is it possible to make a similar analysis with shell elements as I did with solids? (Or this is a dream.)

Irwin

 

[prex]

With shell elements you can only have a linear temperature gradient across the thickness, provided your code allows you to enter it (don't know Nastran, but would be surprised it doesn't, as this loading condition is quite common with shells).
Of course you can also have different temperatures in different regions of your model, but only one linear gradient at each location (element or node).
So, if in your solid model you had a non linear temperature distribution across the thickness (wonder why you could be interested to that, but that's not my problem), then you can't do exactly the same with shells, you can only derive an equivalent linear gradient to use with shell elements.

prex

http://www.xcalcs.com

Online tools for structural design

 

[torpen]

Hello,

Yes it is possible to perform thermal analysis with shell elements. The outputs are the inner face temperature, the outer face temperature and the mid-plane temperature in case of a one layer shell element. For example you can define a composite material with multi-layer shell elements.

If you have x elements in the thickness of your solid model you can define x layers in your shell elements.
And you obtain the temperature at each layer and at the inner and outer sides of the shell.


Regards,

Torpen.

 

[Irwin]

It songs good! Have you got any example about this?

Regards,

Irwin

 

[torpen]

Hello,

I suppose you can find examples in the thermal analysis manual of your code.
You can keep your example by replacing convection on one side by constant temperature. Like that you have half of the answer.

Much of what you need has already been written in this thread.

Firstable you must be sure if conduction through-plane is considered by your shell thermal element. That is to say : is your thermal element a shell element or a plate element? One possible answer can be given by the number of dofs of your thermal model. Thermal shell elements have at least 2 temperature degrees of freedom (top and bottom surfaces) at each node (8 dofs for a quadrangle element). The thermal plate element has just one dof per node and do not support conduction through the thickness.

If you need to map the temperature field (top and bottom temperatures) on structural shells to perform a thermal-stress analysis, you have to move two data :
- the top (or bottom) temperature (easy)
- and the thru-thickness temperature variation (feature available in your code?)
into a shell structural model.


Regards,

Torpen.

 

[Irwin]

I think the NASTRAN can not do that. I could not find any example or information about this. :-(

Irwin

 

[bond077]

On which platform u made this analysis,
Based on the energy and continum the elemental surface will be associated with a definite temperature at the steady state. So u got that temperature value of the element. Obvoiusly solid will give different result , since here the flow of thermal energy will takes place through different pattern due to the core of the material.

 

[Irwin]

Windows 2000