08-23-2018 09:59 AM - edited 08-27-2018 02:49 AM
Hello experts,
I'm looking for the calculation formula of strain energy density in NX NASTRAN (used by SimCenter NX 10).
I can see in post processing the strain energy density as single value for each element. I assume that deriving algorithm uses the following formula with principal stress and strain values.
EDIT 2018-08-24: I guess it's an description error in the next picture. It must be named as strain energy density. The text where I've got that formula named it density in previous chapters, too.
_______________________________
_______________________________
But in my example the values given by NX NASTRAN and the derived value from formula are not the same. Difference isn't huge but visible. see excel export from post processing>>>
<<<
Hint: I also did derive the strain energy density by means of stress components but the result is the same as from principal values (0.01114584).
I wasn't able to find the algorithm for calculation for strain energy density in NASTRAN help.
So where is the mistake? Who can help? Every suggestion is welcome. Best wishes, Michael
| Production: NX10; Development: VB, TCL/TK, FORTRAN; Testing: NX12 | engelke engineering art GmbH, Germany | 2019-07-08
| Kudos for good posts! And if my post answers your question, please mark it as an "Accepted Solution".
Solved! Go to Solution.
08-24-2018 02:35 AM
the QRG gives a differnt formula - see attached
in QRG , ignoring thermal load, for a linear element ESE = 1/2 * uT *Ke * u
08-24-2018 03:58 AM - edited 08-24-2018 05:23 AM
Hi selex_ct,
thank you for answering. The online help you mentioned is the following:
Unfortunately, the formula given by you is for element strain energy not for strain energy density. Strain energy is the integration over volume of strain energy density. But we need strain energy density. And online documentation of QRG has no information about that.
The Theoretical Manual for NX NASTRAN (pdf) says at several places:
>>>
<<<
but my studies were far away in the distant past so I don't know what the L-parenthesis means. Nevertheless, I'm not able to interpret it for different elements (CHEXAi, CTETRAi).
But as I see it, the strain energy density is not necessarily constant in an element. By using of elements with midside-nodes there are gradients of stress and strain in one element and the question is:
What is the method to compute that averaged elemental strain energy density (only one value per element)?
If I use not averaged elemental stress and strain values (only one set per element each) strain energy density should vary. So I assume there is another formula for calculating of strain energy density than the the calculation from elemental stress/strains given by post processor.
Hint: I assume that my given formula in former post is for strain energy density and not for strain energy as designated. I think it's an description error (see my modification in former post).
>>>
<<<
Who can help? Best wishes, Michael
08-24-2018 04:46 AM - edited 08-24-2018 08:44 AM
the L-parenthesis refer to a type of matrix - Might be a row matrix (and where {} is a colum matrix).
08-27-2018 06:34 AM
Hi,
I wonder what integration scheme you are using in your element formulation.
Can you calculate the strain energy density in all Gauss points and compare those results with the single result from the postprocessor?
Best regards.
Martin from Siemens PLM
08-27-2018 09:01 AM
Hi Martin,
I tried to analyze elemental results in stress and strains AND elemental strain energy density from post processing.
At the moment I'm not able to get component results at Gauss points because I don't know how to extract it. Additionally, I have no "access" to the shape functions of elements to derive the averaged strain energy density by means of numerical integration at Gauss points by myself.
My assumption was that elemental stress and strain represent all information which are necessary to compute elemental strain energy density. Now I see that stress and strain gradients in elements volume have another influence on ESE and density than I did expect (mention of bending influence is exactly the point, therefore, the results cant' be identical).
Can you help me in getting the Gauss point results and correct weighting factors for numerical integration of a standard CHEXA20? - My property settings are the following (NX10, Solution 101):
$* PROPERTY CARDS $* $* NX Property: SOLID_001 PSOLID 1 1 0 SMECH
That means IN, STRESS and ISOP are blank.
I'm not sure what happens if I set "Stress Output Location" to "GAUSS". Does it influence Post processing results or only results of Print/PUNCH?
Can you ore someone else help? Best wishes, Michael
08-30-2018 10:37 AM - edited 08-30-2018 10:40 AM
Hi, here is a short addition:
after changing the element type to CHEXA8 (linear) and setting in property the stress output location to GAUSS (only meaningful for linear solid elements in SOL101) the stress tensor values are stored at the database position of element nodal stress tensor values.
Therefore, I could extract it from post processor with excel.
According to the information that integration scheme is 2x2x2 and GAUSS-point weighting factors in this special case are 1.000 I could derive componental strain energy density(SED.ii) for ii=XX, YY, ZZ, XY, ... at every integration point, respectively with
GAUSS-SED.ii = (STRESS.ii * STRAIN.ii)/2
Then I derived:
- the arithmetic averaged values for components SED.ii over all integration points, and,
- after summation over all components
I've got the same value for averaged elemental strain energy density like NX.
I did assume that
Integral of d(Strain.ii) = strain.ii
Problem:
Getting GAUSS integration points values stored at nodal data base position seems to work only for linear elements (in SOL101). That's it. Is it correct?
Best wishes, Michael
08-31-2018 06:08 AM
Finally,
I could see that by deriving the strain energy density at all GAUSS integration points at first (Row sum) and afterwards averaging it over all integration points (columns) yields the same result. I believe that's the way NX is solving it.
>>>
<<<
That's all.