Elastoplastic Analysis of an Offshore Component

[wnmascare]

Hi Everyone!

I performed a simple elastoplastic analysis on an offshore component on Abaqus. Then, when I plotted the equivalent plastic strain (PEEQ), I observed that the maximum PEEQ took place in a region different from the maximum von Mises stress. How is it possible? Have you faced a similar situation before?

Thanks in advance!

 

[SWComposites]

Probably because von Mises stress is a criteria for the prediction of the onset of yielding; it is meaningless in the plastic range. Refer to a strength of materials text.

 

[wnmascare]

SWComposites, thank you very much for your prompt response.

I believe that Abaqus calculates platicity by means of the operator split method. In this case, at each load increment, Abaqus verifies the yield function, which is based on the von Mises stress/criterion. Thus, plastic strains will take place as long as the von Mises stress exceeds the yield stress of the material. That is why I believe that higher plastic strains always take place at high von Mises stress region. Is that right?

Thank you very much!

 

[wnmascare]

Hi everyone!

Again, I performed an elastoplastic analysis on Abaqus and I got a von Mises stress higher than the yield stress of the material, but no plastic strain has been calculated. I modeled my component with C3D8 element and I provided the right stress x plastic strain curve on the input file under the *PLASTIC command. Have you guys faced such a situation before?

Thanks in advance.

 

[burningDiesel]

It is probably an interpolation issue, i.e. the Mises stress in all integration points is below the yield stress, so no plastic strains are calculated on the integration points.
If the mises stress you see on the interpolated contour plot is much higher than the one at the integration points, it just means that you have a bad or too coarse mesh.

 

[wnmascare]

SDEBOCK, thank you very much for your prompt reply. Bsed on your answer, I see that I have problems on contour plot interpretation on Abaqus. I confess that I am not totally sure what kind of contour I must plot to analyze my jobs. If someone else here can help me on that, I would appreciate.

First of all, I don't use Abaqus/CAE to pre-process my model. I use Hypermesh. I just create the mesh and, following, the input file. Then, I open this file and I type the Abaqus commands to create materials (*MATERIALS), section properties (*SHELL SECTION, *SOLID SECTION, *MEMBRANE SECTION, etc.), loading and boundary condition (*CLOAD, *DLOAD, *DSLOAD, *BOUNDARY, etc.), type of analysis (*STATIC or *DYNAMIC) and output variables (*NODE OUTPUT, *ELEMENT OUTPUT, etc.). Finally, as soon as the analysis is complete and the ODB file is available, then I open it on Abaqus/CAE for post-processing.

For the output variables, I type the following:

*OUTPUT, FIELD
*NODE OUTPUT
U
*ELEMENT OUTPUT, POSITION = NODES
S,EE,LE,PE,PEEQ,

You can see that I require the results interpolated to the nodes. On Abaqus/CAE, I usually just plot stresses and strains with Banded countour plot (Options => Contour) and no averaging (Results => Options). This is what I did in my analysis, in which I got von Mises stress higher than the material yield stress and no plastic strain took place.

Should I keep on requiring output variable to be interpolated to nodes?
Is my contour plot strategy right? If not, what would be the best way to visualize contour plots on Abaqus/CAE?
What do you guys suggest me?

I will appreciate any help.

Thanks in advance.

 

[burningDiesel]

You can't really plot contours of integration points in CAE (as far as I know). The quilted option instead of banded interpolates to surfaces instead of nodes, which is already closer to the real integration point value.
You can request the value at the integration point using *ELEMENT OUTPUT,POSITION=INTEGRATION POINTS (also the default).

Just look where your highest value is, and check the integration point values of that element. In a sufficiently refined mesh, distance between integration points and nodes should be small enough so the difference (even before interpolation) is small and negligible. If needed you can do a membrane overlay at the surface of the structure to get integration points at the surface.

 

[wnmascare]

SDEBOCK, thank you again for your reply.

Does anyone here know what kind of situations Banded and Quilt contour plots are more appropriate? Because there are two contour plot options, then there must be some situation in which one of them is more appropriate.

According to its help, Abaqus extrapolates results to the nodes, when plotting Banded countour. On the other hand, Quilt extrapolates results to the element faces on the surface of the model and then takes a weighted sum to produce a single value per face. it also says that since Quilt contour values are computed for each element face individually with no averaging across element boundaries, a Quilt contour plot is an effective means of displaying results on an element-by-element basis.

Can anyone here understand why it is more effective?

Thanks in advance.

 

[burningDiesel]

It's more effective showing results on 'element by element base', as you will only have 1 result per element (if there is only 1 face of the element on the surface).
Regarding which one is 'better', they are both 'wrong', as they are interpolated from integration points. The idea is that if your mesh is fine enough (or the problem simple enough), they are close to the real values.
E.g. imagine a beam under simple bending in the elastic range; the integration points in a hexahedral element are located at 1/sqrt(3) from the center. But, because the stress & strain are linear over the thickness of the beam, the finite element approximation will give exact values at the border because of it!
If you change to elastic-plastic material though, it can be that at the integration point you have stress below yield, but at the border higher than yield. Since everything is calculated at integration point, you will not have yield in your result, and the interpolation is completely wrong.

Long story short, only use integration point values for managing real results. If you want to make a pretty picture, use the contour plots.

 

[wnmascare]

This was exactly what I got in some of my previous analyses. Because I used to plot my results with Banded contour option, I got Mises stress higher than the yield point, but no plastic strains. This looked wierd, because I didn't understand why.

Thank you again!

 

[dlkk]

Hellow. Hellow . I need a little help if you can do this for me....
I am beginner in using abaqus and i have a problem in interpretation of results.
I have to understand the Equivalent Plastic Strain at integration Point PEEK.
I n the last incremement i have the value for this parameter 2.179e+00. what means this value?
My model in in meters.
How i can interpretate this value? I found in Abaqus help but i didn`t find any interpretation there...
Thnaks you very much

 

[wnmascare]

Since you are performin and alastoplastic analysis, you need to have any plastic strain criterion to confront your results. Depending on your application, you are allowed to have some degree of plastic strain. Abaqus help will not give you any indication about that.

 

[wnmascare]

Hi everyone!

I performed another elastoplastic analysis of an offshore component and the maximum von Mises stress was 284.3 MPa. In turn, the plasticity curve I used in the analysis is described below. Since 284.3 MPa is greater than 256.52 MPa, a small amount of plastic strain would suppose to take place. But, I got PEEQ = 0.0. Has anyone here been through to a similar situation? Do you guys understand why this happened?

Thank you all in advance.

*PLASTIC, HARDENING = ISOTROPIC
256.52, 0.00000
260.00, 0.00592
265.00, 0.01444
270.00, 0.02296
280.00, 0.03999
290.00, 0.05703
295.00, 0.06554
300.00, 0.07406
310.00, 0.09109
315.00, 0.09961
320.00, 0.10813
330.00, 0.12516
335.00, 0.13368
343.48, 0.14812

 

[TGS4]

Your maximum von Mises stress is likely at a node, which is extrapolated from the Gauss points. You elements only go "plastic" when the stress at the Gauss point exceeds the local yield stress.

Increase your element order, increase your mesh density. That should solve this problem.

 

[wnmascare]

TGS4, thank you very much for your prompt reply. It helped a lot.

I take this chance to ask another question. Abaqus Help says that the QUILT visualization mode is the most effective way of displaying element-based results.

In sum, in this visualization mode, the stress values calculated at the integration points are extrapolated to the element faces and, then, takes a weighted sum to produce a single value per face. So, can you guys understand QUILT mode is the most effective way of displaying results?

Thank you all in advance.

 

[burningDiesel]

the quilt averages to element faces (instead of nodes), and in most cases yes, this value is closer to the actual integration point values.
But as TGS4 mentioned, when your mesh is fine enough, everything (nodal (averaged or not), quilt or integration point values) should be close enough anyway.

 

[TGS4]

As sdebock said - if the quilt and averaged plots are giving you different answers, then your mesh is not adequately refined - and your problem therefore is a mesh discretization error problem.

Add more elements, increase the element order, and compare the averaged to unaveraged. Unless or until the averaged and unaveraged values match, you need to keep increasing your mesh density.

 

[wnmascare]

Thank you guys for your answers. I will keep those tips in mind for my next analyses.