Hi,
I want to configure a steel with Bilinear Isotropic Hardening, like in Ansys, because I want to compare results. But I’m unsure how to do it. I’ve used the following configuration:
*Plastic
250, 0.0 ← Yield Stress, Plastic Strain
1450, 0.2 ← Hardened Stress, Plastic Strain (Tangent) (the same configuration as Ansys)
But I’m not sure if this is correct
If I calculate with this configuration, and compare the results with Ansys, the Von Mises strees is higher
Thanks
Ansys uses tangent modulus E_T which is the slope of a line tangent to the stress-strain curve at a given point (stiffness like Young’s modulus in the elastic range). For CalculiX inputs, you need true stress vs true (logarithmic) plastic strain data points.
Hi FEAnalyst , and as always, thank you very much for your reply
I have also configured the material, following the instructions of Andreas Baer Engineering (https://www.youtube.com/watch?v=Uh_YFvLzWOw), and in fact, I used their sheet for 275JR steel.
I understand this is a Multilinear Isotropic configuration, ok ?
I have some question s:
Strain 0 is not the Yield Strees, it’s O k?
Should Strain 0 coincide with the Yield Strees?
With this configuration, can the results be compared with Ansys? I mean, are the configurations equivalent? (assuming they are different sol ver)
Should I configure it (Ramberg-Osgood; True Stress - Strain) with 250 instead of 275, so I can compare with A nsys?
With this Multilinear configuration, the results for Strees Von Mises are closer
Thanks
Yes, that’s right.
The first entered point should always be the yield stress and corresponding 0 plastic strain. Further points define the plastic curve via stress vs increasing plastic strain. CalculiX accepts even non-zero plastic strain for the first data point (Abaqus throws an error), but you still have to make sure your inputs match the expected quantities (subtract elastic strain if needed: Converting Engineering Stress-strain to True Stress-strain in Abaqus).
If you want to use the same bilinear model as in Ansys, you should specify something like this:
true stress — true plastic strain
yield strength — 0
UTS — strain at UTS
where the strain at UTS can be calculated as mentioned above.
For S275JR, the yield strength should be 275 MPa. But if you just want to compare both results without changing the inputs in Ansys, then you can use 250 MPa instead.
Isn’t it possible to define a bilinear model in Ansys without a tangent modulus (using just two points from the stress-strain curve) ? It would be easier that way.
I don’t think there is a good way to fit a bilinear Isotropic hardening curve with Ramberg-Osgood.
Curves can’t be comparable everywhere. It can be seen if you draw them both.
Hi Anys,
Thanks for your reply. Thanks to FEAnalyst too, and sorry if I ask basic questions, but,
It is correct to use the Ramberg-Osgood values?
I should only use them starting from the Yield Strees?
FEAnalyst, I don’t understand what you mean. This was supposed to have been taken into account in the Ramberg-Osgood transformation, right?
Ok, I understand that they are not comparable but are they valid ?
And another question, how could I graphically display the equivalent elastic strain at prepomax? .
It’s possible to show graphically the equivalent plastic strain, too?
Because I understand that TOSTRAIN is the total Strain (plastic + elastic)
Thanks
Yes starting from the yield stress, but with 0 plastic strain there. Since yielding starts only from the (initial) yield stress, plastic strain there is still 0. If your strain is non-zero there then it’s total strain with non-zero elastic part and you don’t enter that (CalculiX expects only the plastic part).
I mean that regardless of the way you obtain the plasticity data, you have to make sure it matches the format used by CalculiX so true stress vs true plastic strain. Entering non-zero strain in the first row is incorrect and Abaqus wouldn’t allow it (CalculiX only allows this because of worse input error handling).
Yes, TOSTRAIN (E) is the total Eulerian strain. MESTRAIN (ME) is the mechanical strain (total - thermal). PEEQ (PE) is the equivalent plastic strain. So there’s no output variable for elastic strain.
Check this article, it covers all the needed steps to get the plasticity data from Ramberg-Osgood equation in the format expected by Abaqus/CalculiX (especially note step 5): Stress-Strain Curve Approximation: Ramberg-Osgood Relationship - LearnFEA
It depends on what you mean by “valid”.
If you just want to compare ccx with ANSYS it is not right because there is no match between curves. You are using different material properties.
If you want to perform a real analysis, ideally one wants to use a curve that is endorsed by design standards. The Ramberg Osgood curve is perfectly valid for certain types of analysis. You can even get accepted parameters documented in some codes.
Bi-linear curves are also valid although it is mostly restricted for buckling problems.
A good starting point to get the picture I suggest you read:
DNV-RP-C208, Ju ne 2013
4.7.5 Stress-strain curves for ultimate capacity analyses
Long made short.
Apart from that check what the regulatory codes in your area say about the different curves usage.
Actually, you could even use the Ramberg-Osgood plasticity model in Abaqus. It’s not supported in PrePoMax and thus needs custom keywords, but can be easily entered via Keyword Editor:
*DEFORMATION PLASTICITY
E, v, sigma_0, n, alpha
where: E - Young’s modulus, v - Poisson’s ratio, sigma_0 - yield stress, n - exponent, alpha - yield offset.
Hi,
Thank you both so much for your help