Elastoplastic Analysis of an Offshore Component
Elastoplastic Analysis of an Offshore Component
(OP)
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!
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!





RE: Elastoplastic Analysis of an Offshore Component
RE: Elastoplastic Analysis of an Offshore Component
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!
RE: Elastoplastic Analysis of an Offshore Component
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.
RE: Elastoplastic Analysis of an Offshore Component
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.
RE: Elastoplastic Analysis of an Offshore Component
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.
RE: Elastoplastic Analysis of an Offshore Component
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.
RE: Elastoplastic Analysis of an Offshore Component
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.
RE: Elastoplastic Analysis of an Offshore Component
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.
RE: Elastoplastic Analysis of an Offshore Component
Thank you again!
RE: Elastoplastic Analysis of an Offshore Component
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
RE: Elastoplastic Analysis of an Offshore Component
RE: Elastoplastic Analysis of an Offshore Component
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
RE: Elastoplastic Analysis of an Offshore Component
Increase your element order, increase your mesh density. That should solve this problem.
RE: Elastoplastic Analysis of an Offshore Component
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.
RE: Elastoplastic Analysis of an Offshore Component
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.
RE: Elastoplastic Analysis of an Offshore Component
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.
RE: Elastoplastic Analysis of an Offshore Component