I am trying to plot stress-strain curve for a simple solid block of 3*3*3 mm structural steel with load on top and bottom is constrained. Analyzing with step controls (20 substeps)with large deflection on. The solution is performing with plastic deformation showing on deform counters. While plotting SS curve it always comes linear. Why..any suggestion appreciated ..thanks
You are doing geometric non-linear analysis with E and poison ratio as input. Have you supplied stress -strain data for material non-linear analysis?
Chitaranjan Pany yes i am doing analysis E and PR...is it necessary to supply SS data ...and I am not getting point about non-linear analyses...as i am using structural steel as input material...
@ Charles Chinwuba Ike it is simple cubic solid structure of 3mm*3mm*3mm
The pre-defined structural steel is only a linear material. You will need a material model with non-linearity, i.e. for simple models you can adopt the bilinear model or multilinear.
If you would like to visualize some non-linear SS curve immediately, you can start by adding any self-defined tangent modulus you like to the structural steel. Of course, that is just your hypothetical material, you should obtain actual non-linear curves from experiments and fit them for bilinear or multilinear models (for simple models).
ok Xinwei Li thanks for your answer ..i will try this option...but if i am analyzing 3*3*3 block with some pores with same structural steel material and trying to plot SS curve with max principle stress and strain of whole block..but still it i coming liner..my point is.. in analysis the material is deforming but SS curve is linear in all the cases, even if I am taking some other material too ,like PLA TITANIUM CoCr etc
Nishant Singh Ok assuming your material model is right which contains non-linear portion already, you should NOT be analyzing the max principal stress and strain for the stress-strain curve of your deformed material.
Get the reaction force of the displacement and divide accordingly by area for stress. Strain corresponds to the timestep. Solution -> probe -> force reaction-> boundary condition:displacement -> note to choose directions correctly
However, piece of advice is that static-structural (since you mentioned "Analyzing with step controls (20 substeps)with large deflection on" ) can only get you to converge under low strains, for large strains (maybe > 20 %) you will actually need to use explicit dynamics.
Xinwei Li thank you for your valuable suggestions. I will try with these options. However, I also used explicit dynamics and compressing porous block (PLA) in between two rigid 3*3*1 structural steel material with BC >velocity 160 mm/sec and end time .0002 sec but failed to get large strains..as shown in fig below
based on the type of analysis, either Non linear or Linear, the curve acts....meanwhile material property also plays important role in predicting the curves.
Nishant Singh
Assuming things are right, you can try a higher end time, like 0.001s. 0.0002s may be too low to capture the phenomenon. Also note that the material model should be correct.
Attached is an example of what I'm doing also, compression of a porous solid. Note to add the contact force segment in solutions before you run it.
Thank you Xinwei Li for your valuable suggestions. I came up with the solutions with no-linear material properties i.e. bi-linear isotropic hardening and for stress-strain as suggested by you I put the displacement loading directly to the block and plotted force-displacement curve. Thankyou!
- Badges
- Science topic
- Similar topics
- Engineering
- Mechanical Engineering