Critical Plastic Strain
Moderator: bernd
Forum rules
and Helpful information for the FEM forum
and Helpful information for the FEM forum
Critical Plastic Strain
The issue of what to do with stress concentrations in FEA came up in several posts:
https://forum.freecadweb.org/viewtopic. ... 21#p215672
https://forum.freecadweb.org/viewtopic. ... 31#p220591
https://forum.freecadweb.org/viewtopic. ... 97#p266484
The paradox is that we appear to get punished in “FEM-assisted-design” for more accurate prediction of stress concentrations.
As explained in the above posts, the solution is to take account of plastic strains in the analysis and thereby redistribute peak stresses to lower loaded regions, as will happen in reality.
Then the design question becomes “what is an acceptable plastic strain?” or put differently “will the heavily loaded region crack before the ultimate limit load of the construction detail is reached?”
In my previous posts I recommended to limit the equivalent plastic strain (PEEQ in CCX and ABAQUS terms) to well below 0.05 or 5%.
Now we have fcFEM I can experiment with a more refined check for ductile fracture.
The specification of a critical plastic strain is the topic of active research (see https://www.vtt.fi/inf/julkaisut/muut/2 ... 177-17.pdf and https://www.vtt.fi/inf/julkaisut/muut/2 ... 741-16.pdf) and for the moment design codes make very conservative assumptions; typically eps_cr = 5%.
A better approach (that is both practical and widely accepted) is use of the Stress Modified Critical Strain (SMCS) criterion (see the above reports). It links critical plastic strain (eps_cr) to stress triaxiality (T):
eps_cr = alpha * exp(-beta * T)
where alpha is a material (ductility) parameter, beta=1.5 and T = pressure / sig_von_Mises.
This shows that steel under high isotropic tension (pressure>>0) is much more brittle than steel in pure shear (pressure=0). Alpha factors quoted in literature range for construction steel from 1-5, with the lower values applicable for higher strength steels.
I implemented the SMCS criterion in fcFEM and would like to demonstrate its application for the case of a plate with hole of previous posts.
The design question is: “will the material crack before the plastic limit load of the detail is reached?”. To answer this question I conservatively assume ductility at the lower end of the range (i.e. alpha=1.0) and then increase the load on the detail until the limit load is reached:
The acceptability of the induced plastic strain can now be reviewed by plotting the ratio of equivalent plastic strain to critical plastic strain in the last load step:
If the plastic strain ratio is low, so is the risk of ductile fracture. As can be seen from the plot, the maximum plastic strain ratio is of the order 0.02, which is far below the critical value of 1.0.
https://forum.freecadweb.org/viewtopic. ... 21#p215672
https://forum.freecadweb.org/viewtopic. ... 31#p220591
https://forum.freecadweb.org/viewtopic. ... 97#p266484
The paradox is that we appear to get punished in “FEM-assisted-design” for more accurate prediction of stress concentrations.
As explained in the above posts, the solution is to take account of plastic strains in the analysis and thereby redistribute peak stresses to lower loaded regions, as will happen in reality.
Then the design question becomes “what is an acceptable plastic strain?” or put differently “will the heavily loaded region crack before the ultimate limit load of the construction detail is reached?”
In my previous posts I recommended to limit the equivalent plastic strain (PEEQ in CCX and ABAQUS terms) to well below 0.05 or 5%.
Now we have fcFEM I can experiment with a more refined check for ductile fracture.
The specification of a critical plastic strain is the topic of active research (see https://www.vtt.fi/inf/julkaisut/muut/2 ... 177-17.pdf and https://www.vtt.fi/inf/julkaisut/muut/2 ... 741-16.pdf) and for the moment design codes make very conservative assumptions; typically eps_cr = 5%.
A better approach (that is both practical and widely accepted) is use of the Stress Modified Critical Strain (SMCS) criterion (see the above reports). It links critical plastic strain (eps_cr) to stress triaxiality (T):
eps_cr = alpha * exp(-beta * T)
where alpha is a material (ductility) parameter, beta=1.5 and T = pressure / sig_von_Mises.
This shows that steel under high isotropic tension (pressure>>0) is much more brittle than steel in pure shear (pressure=0). Alpha factors quoted in literature range for construction steel from 1-5, with the lower values applicable for higher strength steels.
I implemented the SMCS criterion in fcFEM and would like to demonstrate its application for the case of a plate with hole of previous posts.
The design question is: “will the material crack before the plastic limit load of the detail is reached?”. To answer this question I conservatively assume ductility at the lower end of the range (i.e. alpha=1.0) and then increase the load on the detail until the limit load is reached:
The acceptability of the induced plastic strain can now be reviewed by plotting the ratio of equivalent plastic strain to critical plastic strain in the last load step:
If the plastic strain ratio is low, so is the risk of ductile fracture. As can be seen from the plot, the maximum plastic strain ratio is of the order 0.02, which is far below the critical value of 1.0.
Re: Critical Plastic Strain
I added the critical plastic strain ratio as a post-processing step for CCX results. This is available from the VTK pipeline and for export to ParaView:
However, the 3 additional material parameters still need to be added to the material input objects
However, the 3 additional material parameters still need to be added to the material input objects
-
- Veteran
- Posts: 3129
- Joined: Sat May 20, 2017 12:06 pm
- Location: Germany
Re: Critical Plastic Strain
No, I mean alpha, beta and sig_y to compute the critical strain (see model at beginning of the post). I guess it is only 2, because sig_y is implied in the stress-strain curve.
Re: Critical Plastic Strain
PS: you give yield stress first and strain second in your list. I thought it was the other way around?
-
- Veteran
- Posts: 3129
- Joined: Sat May 20, 2017 12:06 pm
- Location: Germany
Re: Critical Plastic Strain
yield-stress first, than strain (and maybe temperature)
See ccx manual 2.20 page 533:
See ccx manual 2.20 page 533:
Re: Critical Plastic Strain
CCX predicts a critical strain ratio of 0.2 at full load (1.0 signifies rupture), but cannot push beyond that due to breakdown of the solver at collapse.
fcFEM happily continues at collapse and at the end of the following load-deflection curve computes a critica strain ratio of 0.56 ... getting closer to rupture.
Re: Critical Plastic Strain
I have now integrated the critical strain ratio calculation in FC such that no additional material parameters need to be entered.
Starting from the definition:
critical strain ratio = PEEQ / (alpha * exp(-beta * T)),
where:
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)
So this is how I have now implemented the Critical Plastic Strain calculation in FC. It takes all required parameters from the user input.
I will give an example of how this works and then start to prepare a pull request.
Starting from the definition:
critical strain ratio = PEEQ / (alpha * exp(-beta * T)),
where:
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)
So this is how I have now implemented the Critical Plastic Strain calculation in FC. It takes all required parameters from the user input.
I will give an example of how this works and then start to prepare a pull request.
Re: Critical Plastic Strain
sweet!
Alone you go faster. Together we go farther
Please mark thread [Solved]
Want to contribute back to FC? Checkout:
'good first issues' | Open TODOs and FIXMEs | How to Help FreeCAD | How to report Bugs
Please mark thread [Solved]
Want to contribute back to FC? Checkout:
'good first issues' | Open TODOs and FIXMEs | How to Help FreeCAD | How to report Bugs
-
- Veteran
- Posts: 3129
- Joined: Sat May 20, 2017 12:06 pm
- Location: Germany
Re: Critical Plastic Strain
For testing:
DNV-RP-C208 manual, example B.1.2 page 44, cantilever beam with notch
https://rules.dnv.com/docs/pdf/DNVPM/co ... P-C208.pdf
zip contains FC-file, SMath-file, force definition pdf
Bonus file:
Frame buckling, example B2 page 46:
DNV-RP-C208 manual, example B.1.2 page 44, cantilever beam with notch
https://rules.dnv.com/docs/pdf/DNVPM/co ... P-C208.pdf
zip contains FC-file, SMath-file, force definition pdf
Bonus file:
Frame buckling, example B2 page 46: