## You are here

# Nodal Stresses

Hi all

I want to know how to find nodal stresses. For example say, in a plane stress analysis knowing displacement's dof, we can get stresses. But these stresses are those at the Gaussian points. We can extrapolate these stresses at Gaussian points to nodal values. My question is, for every node we will get four stresse values (extrapolated from stresses at Gaussian points) using these how I can get single value at the node? What averaging techniques I should follow and how ? And after finding a single stress at a node, how we can get stress for the element?

Thanks in advance

Sreenu

- SivaSrinivasKolukula's blog
- Log in or register to post comments
- 15284 reads

## Comments

## That's right,

That's right, SivaSrinivasKolukula, the problem is simple enough that none may want to mention it on his resume---but, I do so, anyway.

In case you have missed it during your reading of the book by Cook et al. on FEM, go back to it; it's mentioned in it, too; look for the phrase "stress recovery." Also, in many online notes, e.g., those by Prof. Carlos Felippa.

(The reason I mention it in my detailed resume is in an obviously (though only partially) useless attempt to deflect another line of sarcasm from many others (esp. the Western ones): "So, you say you wrote solver code, huh?" ... Adding the clarification helps me do that---thwart the usual sort of sarcasms (usually) leveled against me. (Incidentally (and somewhat surprisingly) none gets sarcastic with my "first in 75, (102,) 187, 200+ years" line, though! (Funny, isn't it? (Yes, I, too, can get sarcastic. (But, as a rule, only in reciprocation (and, *after* much provocation (from the (obvious) incompetents)))))))

--Ajit

- - - - -

[E&OE]

## Dear sir

Dear sir

Yes I have refered Cook 'stress recovery' and Nodal avaraging techniques, patch recovery..etc..... I am writing code in MATLAB and checking the values with a standard FEM software. The stress values at Gaussian points are matching but not at the nodes..

Sreenu

## Re. Nodal stresses

Dear Sreenu,

A few questions:

What standard software do you use for benchmarking? What is the element like---its type, number of nodes, order, number of Gauss points, etc.? And, what is the order of the stress extrapolation expression? Can the benchmarked software somehow be made to report on the extrapolated values at each node---n number of values for the n elements which share that particular node? How is the extrapolation carried out in your code, and in the referred software? How is the averaging carried out in each?

Stress extrapolation and recovery is a bit of grey area. Perhaps the extrapolation part of it is not so grey (esp. if the element is isoparametric), but there could possibly be some options in the averaging part of it---it might have been implemented with some (ad-hoc) weighting schemes. Look into such possibilities, too.

And, finally, a few simpler questions that you might want to check on first, before going over the above: Does your code produce values that are reasonable to your engineering judgment? Or, can there be bug(s) in it? Have you compared the nearest Gauss point values and the recovered nodal values? Have you graphically plotted the recovered values and the raw values (with discontinuities/banding intact)? Do they make sense---as patterns, and in terms of absolute values, as compared to some experimental values? Ditto, for the benchmarked software. What is the %age difference between the two? How does each software behave for (i) structured mesh, (ii) irregular mesh, (iii) structured and irregular meshes with some (or all) elements having aspect ratios that are deliberately kept somewhat bad for the problem at hand?

Best,

--Ajit

- - - - -

[E&OE]

## Inspiration and genius--one

Inspiration and genius--one and the same.

-----------------

Siva Srinivas Kolukula

Senior Research Fellow

## Dear Sir

Dear Sir

I am using Isoparametric Q4 elements for the analysis. The

problem is a plane stress problem. The standard FEM software I am using for

comparison is CASTEM. The stress values at the Gaussian points are in absolute

perfect match. There is no error between both the codes for the stress at

sampling points. CASTEM has the option to get stresses at nodal points as well.

CASTEM has two options to extrapolate the values from Gaussian points to

node's: (1) Extrapolate the values using the shape functions (2) Least square

fit of the values (Patch recovery Technique). And after getting the nodal

values they are either averaged dependng on the nodal sharing or simply a sum

of the nodal stresses.

I have followed both the techniques. Below are the

results. I have shown maximum and minimum values for the stress.

1.

From standard FEM software:

sum = [4.63364E+05 1.34811E+05 50234

-1.21302E+05

-78506 -50234];

average

= [1.94435E+05 67405 50234.

-85170

-39253 -50234.];

2.

My MATLAB CODE:

Values

using Extrapolation:

average

= 1.0e+005 * [ 2.0792 0.4222 0.7579

-0.7903

-0.4344 -0.7579 ];

sum

= 1.0e+005 *[ 4.6424 0.8895 0.8968

-1.2760

-0.8688 -0.8968] ;

Values

using Patch Recovery:

Average

= 1.0e+005 *[ 2.0792 0.9085 0.9535

-0.7903

-0.3088 -0.7579];

sum

= 1.0e+005 *[ 4.8124 0.9260 0.9535

-0.7903 -0.6176 -1.1501] ;

How

the values are??? May be the standard software is using different orientation

of the coordinate axes. Whatever, I think the values at the Gaussian points are

most accurate and will be used for further calculation. As they are in perfect

match, I am happy.

Sir

I need one more clarification, for an element I have four Gaussian points and

for every point I got stress values. If I want to use one value, which one I

should pick? Shall I have to average or what???

Thanking

you

Sreenu

## Interpretation of numbers

Dear Sreenu,

[Tries to contain the laughter.]

What is the domain geometry? How is it meshed? What are the node and element numbers like? What are the material properties (values, units)? What are the displacement/force boundary conditions (values, units)? To which element do the result matrices refer? In what order do the physical quantities appear in those results-matrices?

In the absence of answers to these (and such) questions, all that I could figure out was that there was a symmetry between 0.50234 and -0.50234 in each of sum and average results for CASTEM, and a similar symmetry between 0.8968 & -0.8968 and between 0.7579 and -0.7579 in your results. Couldn't figure out anything more! (LOL!)

There always are chances that a given software might be reporting its results in an element-local coordinate system, and that you may have to transform these into the global coordinate system before comparisons can be made to the results produced by another software (and perhaps also that the global coordinate systems in the two models/softwares themselves might not have been identically positioned/aligned, anyway (LOL!!))

OK.

Why do you need only one value, presumably for each element, when you have already used four Gauss points? Here, I have forgotten, and so can't tell off-hand, whether the average of the values obtained at the four Gauss points for the gradient variable can be expected to come out to be the same as its value obtained using just one Gauss point, when the element is plane-stress/strain Q4---the "rs" product term included in the bilinear model "instinctively" makes one a bit doubtful, esp. when the element geomtry isn't rectangular and the loading+constraints isn't symmetrical.

Anyway, if you are happy, I am happy ;-)

--Ajit

- - - - -

[E&OE]

## Dear Sir

Dear Sir

Any ways....I need stress values at the Gaussian points for further analysis and castem values and my code values are perfect match.

Why do you need only one value, presumably for each element ?

I want to find geometric stiffness for a structure, then I need to have initial stress in hand.

KG = ∫∫N'[σ]N.t.dx.dy

where σ is the initial stress. To find it, for σ what value I should use?? For an element we have four Gauss points and which one should be picked, this the way my doubt rised..

Thanking you

Sreenu

## geometric stiffness

The answer is simple. Just perform numerical integration in KG. If you are using 4 Gauss points, then you have to compute KG using the Cauchy stress at those 4 Gauss points.

## Hi But Cauchy stress

Hi

But Cauchy stress gives stress at a point. Can you be more brief...?

Using stress values at four Gaussian points how to find the stree for the element.....

Sreenu

## Re: Hi But Cauchy stress

Well, I answered what you asked. You already said that you have 4 Gauss points. Therefore you should use each sigma at those 4 Gauss points to compute KG numerically. That is the way you should typically do in a FE code.

If you are using constant strain elements, the stress in the element is constant and therefore the stress will take on the same value at all the 4 Gauss points. Otherwise, the stress is not constant in the element and you cannot find a unique stress in it. You could interpolate inside the element to get a value at an arbitrary location x in the element. As Ajit said, why bother with this if you have already used the stress at the 4 Gauss points? Can't really see why you want to use just 1 value.

## Hi I apologize for

Hi

I apologize for late reply....For caluclating Geoemtric Stiffness Cauchy stress is not required..I got the values...Using Patch Recovery method the stress at four Gauss points is extrapolated to center of the element. This will be used in place of σ. The following is the value I got for first load...

FEM : 4.96219E+07

Timoshenko : 4.97643E+07

Thank you Ajith Sir and Alejandro for discussion and help....

Sreenu