Temperature result for shell
Temperature result for shell
(OP)
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
(I made a control analysis with a solid element. The result for this element is different.)
Irwin





RE: Temperature result for shell
corus
RE: Temperature result for shell
-Can I use any option to write temperature on top and bottom surface at the same time?
Irwin
RE: Temperature result for shell
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
RE: Temperature result for shell
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
RE: Temperature result for shell
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
RE: Temperature result for shell
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
RE: Temperature result for shell
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
RE: Temperature result for shell
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
RE: Temperature result for shell
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
RE: Temperature result for shell
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
RE: Temperature result for shell
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
RE: Temperature result for shell
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.
RE: Temperature result for shell
Regards,
Irwin
RE: Temperature result for shell
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.
RE: Temperature result for shell
Irwin
RE: Temperature result for shell
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.
RE: Temperature result for shell