Thermal Set

[ULBsha]

Hello,

I was wondering if there is a difference between the two following load cases:

1) Only a mechanical set (without any thermal set) for which the temperature for material properties is set to 295 K.

2) The same mechanical set (295 K for material properties) PLUS a uniform thermal set of 295 K everywhere.


Actually, I realized that I get 2 different results when optimizing these 2 studies but I do not understand why. Do you have any explanation for that ?


Thanks a lot.
Regards

[Christian W.]

The temperature will extra stresses in the structure. Typically, in a thermal analysis you apply not T but dT.

[James]

Christian W. is right, the extra thermal load will cause thermal stresses proportional to (alpha * delta T).

The reference temperature, defined for each load set on the project setup form/load sets tab, defines the reference temperature for the material properties. This is not a load, so there is no additional element forces calculated based on the thermal case.

If you create the model and apply a thermal case applied, there will be additional loads calculated based on the thermal expansion coefficient (alpha). For composites, HyperSizer handles the calculation of residual ply strains locally by computing the difference in the free thermal growth of the entire laminate vs. the thermal growth of the local plies.
See: http://hypersizer.com/download.php?type=analysis&file=HyperSizer_Stiffness_Method_-_Thermoelastic_In-Plane_Stiffness_Formulation.HME.pdf, section 4.

You should also be aware that HyperSizer will use different factors for a thermal set vs. a mechanical set. The thermal help/hurt factors, applied on the design-to loads tab, will factor up/down the thermally-induced loads based on if the thermal load increases or decreases the margins of safety. As a best practice, we recommend separating thermal and mechanical loads into unique FEA subcases, and creating the load case combinations inside HyperSizer.

To understand the thermal help/hurt factors, see: http://hypersizer.com/help/#Loads/load-factors.php

I hope this is helpful

-James


 

[ULBsha]

Thanks Christian and James.

Indeed, I understand that thermal stresses are proportional to (alhpa*delta T).
But, do you mean that if we only have a mechanical load set with a reference temperature of 295 K, using Ti-6Al-4V let say, HyperSizer doesn't consider the thermal expansion of this material, which is alpha=8.82 at 295 K ?

If it doesn't consider it at all when we only have a reference temperature, I understand the thing (in this case I could ask what would be the usefulness of mentioning/setting a reference temperature then?);
But if it does, why should there be a difference between
- no thermal load, but only reference temperature of 295K, and
- uniform thermal load of 295K everywhere ?
I mean, in this particular case where the reference temperature and the thermal load have the same magnitude, the "delta T" is the same in both cases, isn't it ?


I am asking this because my optimized structure weights almost 50 tons under only a mechanical load set (and 295K reference temperature), but I get 800 tons (!!!) if I add a uniform temperature load set of 295 K (the whole structure is made of Ti-6Al-4V) !? Note also that if I remove the mechanical subcase and I only impose my uniform thermal load of 295 K, the structure weight drops to 3 tons (which seems logical since there is almost no stress in the structure).


Kind regards.

[James]

If you specify a reference temperature on the loads sets tab, HyperSizer does not calculate thermal strains. Since an initial temperature is not specified there is no way to calculate a delta T. You must define a thermal load set for HyperSizer to include the thermal stresses.

The usefulness of defining a reference temperature for mechanical cases on the load sets tab is to set the reference temperature for the material properties. So when HyperSizer calculates strength and buckling margins for the mechanical load set it uses the appropriate material properties.

If a thermal set is paired with a mechanical set, HyperSizer will compute the material reference temperature for each component based on the average element temperature.

-James

[ULBsha]

Thanks James.

I realized that I hadn't specified either the initial temperature, nor a reference temperature (in my MAT1 card). By adding them it solved my problem.

However, I have another question concerning the way HyperSizer calculates the material properties beside the indicated temperature range; How the material properties are calculated if the properties are given up to 700K for instance, but the applied load goes up to 750K ? It doesn't seem to be a simple extrapolation since my structure gets much much more heavier if the maximum applied temperature exceeds only "slightly" the material limit...

Thanks.

[James]

HyperSizer will not extrapolate outside the stored temperatures to determine material properties. If a reference temperature is greater than the temperature assigned to the properties, then the properties from the highest reference temperature are used.

I'm not sure why your structure gets much much more heavier if the maximum applied temperature exceeds only "slightly" the material limit. Do you have material correction factors defined as a function of reference temperature?

-James

[ULBsha]

Dear James,

It is very interesting to know that HyperSizer doesn't extrapolate outside the stored temperatures. So, does it mean that if the highest assigned temperature is 500K, there will be no difference between the case with a uniform temp load of 500K and the one of 700k ?

Regarding the material correction factors, I use isotropic materials (Ti-6AI-4V KMAT1%301). Therefore, if I am understanding well, the factors are already imposed by HyperSizer materials database and I am not allowed to change them.

Finally, I really do not understand what could cause this huge increase of mass if the applied temperature is higher than the assigned temperature... 

[James]

If the maximum stored temperature is 500F then the HyperSizer analysis will not change if you increase the reference temperature to 700F. The same stiffness and allowable properties are used as if your reference temperature were set to 500F.

Check to see if the FEA solution is returning different loads. Compare the magnitude of the FEA loads for the thermal cases between the two sets of results.

-James

[ULBsha]

Dear James,

I'm back to you regarding this issue again. Let me summarise the problem by describing a simplified case:

I'm trying to analyse an aircraft on which both mechanical and thermal loads are applied.
Let assume that the mechanical load is just a uniform pressure load over the structure, while the thermal load is a time-dependent function, as shown in the figure (see attachment):
1) 300K during the first 1500seconds;
2) An increase of temperature to 750K, performed in a period of 1500seconds;
3) 750K is maintained during the rest of the experiment (let say 9000seconds).

I want to size the aircraft structure with respect to its cruise phase, i.e. when the temperature is at 750K (in other words, in segment 3).

I use the following ordinary commands to setup my input Nastran file:

SOL SESTATICS
CEND
TEMP(INIT) = 1

SUBCASE 100
TEMP(LOAD)=101
BEGIN BULK

Now, the question is how to define the thermal set, regarding the initial temperature TEMP(INIT) ?
Should I put:
TEMPD,1,300
TEMPD,101,750

or:
TEMPD,1,750
TEMPD,101,750

Indeed, I want to have the effect of thermal stresses, so I think that my initial temperature (TEMP(INIT)) should not be equal to 750K, which is my (final) thermal load (TEMP(LOAD)). However, since the increase of temperature is done over a long period, is it realistic to put the initial temperature at 300K ?

The strange thing is that when my TEMP(INIT) value is equal to 750K, the HyperFEA calculation gives me a realistic increase of weight compared to the case without any temperature load. I guess this increase is just due to the change of the material properties because of higher temperatures that are applied.
But if I set TEMP(INIT) value to 300K, the calculation diverges and the weight goes infinitely high (thousands of tonnes !!) without converging. Note also that this divergence doesn't happen if I decrease the cruise temperature (TEMP(LOAD)) from 750 to 600K and maintain the TEMP(INIT) at 300K. It seems that the very high thermal stresses induce this divergence, but I don't know why! The used material is Titanium.

Thanks a lot.
Regards

[James]

The initial temperature should represent the "stress free" temperature. The duration of the temperature shouldn't matter. The mechanical loads for your cruise condition are occurring at the same time as your 750K applied temperature so I think your delta T = 750-300 to determine the thermal stresses.

Your assessment of the mass increase due to increasing the material reference temperature makes sense to me.

So when you set Temp(init)=300, deltaT=350K and there is a huge mass increase. This sounds like a problem with the CTE properties (alpha) in the FEM. Can you double check the magnitude and that the units work out?
 

[ULBsha]

Thanks James.

No, the CTE seems to be fine (a variation between 8.5e-6 m/mK and 10e-6 m/mK). However, the Gii values are quite strange according to me: a huge increase when the delta T goes from: DeltaT=(600-300)  to  DeltaT=(800-300) !!!

Please find attached the 3 *.PM files for which a uniform temperature of 295K, 600K and 800K are applied as thermal load, with initial temperature of 295K for the three studies. For instance, on the component "200003 FuselageSkin_2", you will see this huge increase...  (you can also notice the huge increase of masse/unit area given in the PSHELL card).

Do you have any idea about this problem ?

Just one thing to be sure: I read the MSC Quick User Guide and it's mentioned that for the initial temperature, we have to use TEMP(INIT) and in this way we don't have to put any Tref in the MAT card.
However, in my initial material properties (my input bdf file for HyperSizer), I used the TEMP(INIT) command, but I also used this Tref as 295, which is the same than my TEMP(INIT) value... Could this cause any issue ? 

Thanks again

[James]

If both temp(init) and Tref are specified, then the Temp(init) will be used instead of Tref on the property cards. I have used the Temp(init) card before and I can confirm this behavior.

The increased Gij and NSM on the Mat cards is likely because the panels are sizing up in HyperSizer. HyperSizer will then export the ABD stiffness terms for the stiffened panel to the MAT2 cards that are referenced in the PSHELL card. See: http://hypersizer.com/help_7.0/#FE-Update/update-stiffened_panel_export.php%3FTocPath%3DFEM%2520Interface%7CUpdating%2520the%2520Model%7C_____3

Can you confirm the Gij values in the .pm1 file are the same ABD values represented in the sizing form > properties tab?

Can you look at the input loads from your cases where deltaT = 800-300. I think the thermal loads are probably really high which is causing the panels to size up in HyperSizer.

[ULBsha]

Dear James,

Thanks for your help.

Actually, the Gij values in the .pm1 file are the same ABD values represented in the sizing form. However, I noticed that some of my components show Invalid Geometry for the MOS (I have one single component in a group, to fully optimise the structure). I know what this means, but I don't understand why it happens when my deltaT goes from '600-300' to '800-300'...

Indeed, I am using the Object Model ability, so I have some scripts written in Matlab that update the variable bounds automatically after each set of X iterations between HyperSizer and Nastran (HyperFEA). So, the process is the same, but apparently it doesn't work correctly with high applied temperatures...
I also get this issue when I try to size the AP1 (given as tutorial) with a applied uniform thermal load of 1000K ! Please note that I get a vehicle mass of less than 5 tonnes if we apply a 750K load, with positive MOSs, but it increases to 32tonnes if it's 1000K, with some Invalid Geometries...

Regarding the input load, I don't really understand what you mean. If you mean the forces in different elements shown in my *_i.f06 file, it's quite difficult to compare the different cases... but when I compare element by element for both cases, it seems that the forces for the deltaT=800-300 are higher than those for deltaT=600-300... (some times 1 or 2 orders of magnitude higher)...

Do you have any solution... ?

Thanks again.

[James]

It sounds like your components are oversizing. Oversizing occurs when HyperSizer can't find a solution that fits within your sizing bounds so it returns the heaviest solution. The geometric checks are a pass/fail check. The "INVLD GEOM" is treated as a negative margin. What happens when you turn off the geometry checks and resize the  case with deltaT=800-300?

The element forces for the thermal case can be viewed in the HyperSizer graphics window. What is the magnitude of the element forces for the thermal case?