some regulation recommended to limit the plastic strain about 4% at ultimate loads, looking the documentation itself is linearized not based on peak values. hope this missing feature will be available in the next future release. thx u
…it’s not about averaging and extrapolated nodes were are common in FE. i mean linearized along failure lines by curve fitting a straight line using the method of least squares. using Paraview it can be access trough PlotOverLine and PlotChartView.
instead of use averaging, there’s another straight forward in post-processing of strain result called Stress Modified Critical Strain or Critical Plastic Strain. but it seems have sensitivity in mesh refinement
strain based design (ductile fracture materials i.e steel) is in heavy intention research since it’s last crucial steps to review and predict the strength capacity and failure modes of a part
FreeCAD also implemented this features and it been discussed by developer in the forum.
Quasi plastic limit analysis is valid (and not excessively mesh dependant although mesh convergence does need to be checked) approach for this sort of analysis, if that is that is finding ultimate capacity. I would suggest reading up a little bit basically you set up properties so that the material transitions from elastic to very plastic at around material yield. As I have used it the load is applied by displacement and the capacity is based on the change of slope of the reaction vs displacement curve.
There are of course other models but this is robust compared to models where you delete elements based on strain. I used those while at Boeing and with a good bit of work they correlated nicely with test data but I wouldn’t use it without testing (and I don’t know if calculix can solve those problems)
referring to document reports: strain plot are based on extrapolate from Gauss Point, so dense mesh the more accurate results. Critical Plastic Strain reported at the peak and concentrated, but equivalent plastic strain need to averaging along the line of failure path. so make it less sensitive due to averaging not as peak.
right, i heard about it from another FE codes such as LS-Dyna/Radioss to approaching of loss in strength and stiffness at fracture.
however, i seen Stress Modified Critical Strain is different methods to predict the strength and modes of failures.
also, load displacement response in steel has classified as stability or serviceability limit states for slender part or members. in case of stable models, mainly govern by strain.
I have give a try to the example B.1.2 T-section cantilever beam with notch.
Previously I have made some tests on the material used to check everything was ok.
Results looks fine and curves agree with the manual . I’m pending the computation of the critical strain ratio according to the developer formula :
“PEEQ / (alpha * exp(-beta * T)),
PEEQ = equivalent plastic strain (produced by CCX),
T = stress triaxiality = pressure / sig_von_Mises (calculated by FC),
beta=1.5,
Alpha is a material (ductility) parameter, So alpha is the only unknown. However, this can be linked to the critical plastic strain in the stress-strain curve, for which the triaxiality T = 1/3.
With this it can be shown that alpha = 1.65 * eps_cr_uniaxial (the last strain entered by the user in the MaterialMechanicalNonlinear object)”
-¿What is pressure?
-I would say “eps_cr_uniaxial / the last strain entered by the user” is the True strain corresponding to the Ultimate σult [MPa]. ¿Am I right?
hi, firstly i’m only shown a proposed ideas of another methods in direct calculation of strain at limit loads. it can be good alternative instead of averaging i discussed before in YT
the developer of FreeCAD extend to define and approximates alpha values based on some assumption, this is not documented in references report. please ask in their forum directly.
according to original reference documents, the toughness parameter (alpha) could not a single values and it seems better to left the user input manually. even some default proposed value is available, still can give possibility to overrides.
Very interesting method. I agree Linearization tool or PlotPath could be useful.
I’m waiting for the FreeCad forum to send me the verification EMail. I would like to make some questions as ccx model match quite well with the DNV Example but my Critical Strain Ratio is slightly hight. I think the difference comes from me using True Stress Strain values while FreeCad user report shows Engineering values.
Regarding Alpha I would say 1.65 * eps_cr_uniaxial is an error. At some point he mentions Ratio =1 means failure.
Attached my provisional results.
i did not see into details, only lookup the table and figures.
the ratio of triaxiality plots shown below 1.0 so make the assumption is valid.
the values of critical strain ratios in pictures attached shown 0.67 not 0.847 as reported by FreeCAD developer, so it requires to investigated further.
critical strain ratio depending on material strength and triaxial stress, for below 1.0 of triaxiality the ranges between 25% and 100% in percentage or 0.25 and 1.0 with decimal values
linearized or averaging mostly depend on strain distribution along path defined, it can be inconsistent due to highly concentration or nearly uniform at the notch areas.
maximum plastic strain by linearized is depend on steel material strength, typically 4% in percentage or 0.04 in decimal values.
due to averaging, maximum plastic strain by linearized become less sensitive in mesh. not the case of critical strain ratio since it reported directly at the peaks.
Thanks for your comments. I’m still pending admission on the Freecad forum.
My value for the critical strain ratio is first 0.67 and later 1.11 after refinement. I need to clarify this.
I have a very good agreement at this point.
From my results Critical ratio seems highly sensitive to the mesh size.
Apart from that : I have seen various pictures in the DNV manual showing “(Avg 75%)” in the description of the Plastic Strain Max Principal SNEG. ¿Does someone know what is it? ¿Does prepomax average in the same way.?
even it had the same names, but the meaning may differs. equivalent plastic strain (PE) in CalculiX GraphiX is PEEQ in Abaqus Plot. initialize PE in Abaqus has different terms in definition of plastic strain at a tensor in direction of stress.
i’m not really sure regarding 75% reported, but it may have relation with averaging nodal values plotted using extrapolate based on integration point of individual element contributed.
thanks for pointing, this features given flexibility to the user and more advanced. work as user defined post processing results, so it can be capture large broad ranges of user interested in.
or the ability to export easily into Paraview… late to the conversation. How are things going with this? Last time I translated to paraview from frd I found that I lost some information along the way. Its not super ideal.
Creating an export to Paraview is not a primary task, and it is a question of whether it will be integrated in the future.
But the new PrePoMax v1.4.0 has the possibility to export the nodal coordinates while preparing a history output. That could help in exporting the results for later analysis since the nodal values can be sorted by the nodal coordinates in the data analysis software.
