I am currently working on the following scenario - a cantilever beam (rectangular section) meshed with solid elements subjected to a concentrated force at the free end. Bending occurs in the elasto-plastic regime (elastic perfectly-plastic material model). My goal is to obtain the deflection as close to the analytical one as possible using solid elements. Here are the current outcomes:
analytical solution: 23,625 mm
beam elements in Abaqus (40 x B22): 23,69 mm
solid elements in Abaqus (7000 x C3D8R): 23,36 mm
beam elements in CalculiX (100 x B32): 68,3 mm !!!
beam elements in CalculiX (100 x B32R): 22,6 mm
solid elements in CalculiX (7000 x C3D8R): 23,27 mm
solid elements in CalculiX (26451 x C3D10): 23 mm
As you can see, the result obtained with B32R elements in CalculiX is not so good and with B32 elements (full integration) I get completely wrong value. That’s probably because of shear locking.
Solid elements provide significantly better results (especially C3D8R) but they could be a bit more accurate.
Anyway, what I would like to ask you is whether there are some additional element types that could be better for this type of application and how far I should go with mesh refinement.
Also, does it matter if I use rigid body constraint or coupling to transfer the concentrated force to the front surface of the beam ?
you can try Incompatible mode brick elements.
here is a good resources of examples:
with these example:
I thought we had the same issue before, but i don’t find any the topic.
I had the same problem, and the solution was to change to these kind of elements!?
Please let me know, if you find a solution according to you hand calc…
Can you post your analytical solution? These would be very helpful for me.
(tip: I would always use a displacement for these king of calc. first and
check the force with the boundary reaction)
As you can see, the closest I managed to get to the analytical solution (23.625 mm) in both programs is with C3D8R elements and surface traction. Much to my surprise, neither second-order nor incompatible mode hexahedrons helped in this case. Perhaps the analytical solution is simplified in some way or solid elements can’t reach that level of accuracy in this case.
Anyway, I will share the analytical solution soon since I plan to publish a YouTube tutorial for this analysis. But I’m not sure if this solution will be useful for you since it’s just a single already derived formula taken from a quite old Polish book.
thank you for the vey helpfull manuel.
There is no possibility to use your formular with common or min. double symetric cross-section?
To inlcude moment of inertia in common?
Can you post the formular for a cantilever beam and self-weight?
These would be the same system like single spawn girder with hinged boundary,
so i can test the deflection with *rigid body and so on.
I am also interested in formulas for the deflection of beams with arbitrary cross-section, support and load type. Unfortunately, the Polish book I used for analytical solution in that video (as well as other books I checked) describes calculations just for the cantilever beam with a rectangular cross-section and concentrated force applied at the free end. The generalization to other types of beams is only briefly mentioned in the literature. “Mechanics of materials” book by Timoshenko and Gere features one of the best descriptons in this topic I’ve seen so far. You can find this fragment attached to one of the posts in researchgate discussion that you shared before.
thnx for your reply.
i have the book “Mechanics of materials”. I have checked to find a solution for the cantilever beam,
but i don’t make a sense of it. Maybe i’ll try again. I’m not so good in abstract or theoretical work.
If it helps you, i can provide some pages of interests for you as pdf.
wbr
I have done hand calculation with Imperfection for elastic and plastic calc. and Th.II.O
and i get the value like in the example with 6000,0 kN:
So i created a model with ccx with elastic and plastic material and imperfection:
For the elastic calc. i get 600,0 kN, but for the proof with plasticity it always about 5500,0 kN!?
If you#re interested i can provide the example and files and formulars.
So it’s a nonlinear column buckling problem with plasticity and imperfections ? Sounds interesting, especially if you have analytical solution for that. Please share it if it’s not a problem. CalculiX files would also be useful, especially that it seem that you solved this with solid elements, not beams.
By the way, the document that you attached to this post is currently unavailable. Can you repost it ?
Note most theoretical presentations of deformations of beam like members ignore the deflections due to shear deformations since it is usually, but not always, small in comparison to deflections due to bending. FEM with solid elements normally does not ignore this additional deflection, though the accuracy of the correction depends on the nature of the elements used.
beam & shell element are expanding to solid element in CalculiX during calculation. bellow are an explanation i extracted from official documents, may apply to beam element also.
Shell element S4 expanded to solid C3D8I: cannot be used in *DYNAMIC calculations, has controlled hourglassing, (ed. still questionable for one layers only)
Shell element S4R expanded to solid C3D8R: small elements are required to capture a stress concentration at the boundary of a structure,. massive hourglassing, displacements are completely wrong, but stress field is still correct.
Shell element S8 expanded to solid C3D20, badly for isochoric material behavior, i.e. for high values of Poisson’s coefficient or plastic behavior. too stiff in bending
Shell element S8R expanded to solid C3D20R: high stress concentrations at the surface of a structure might not be captured if the mesh is too coarse. problems in node-to-face contact calculations
if the user manually define layer by duplicated mesh with offset options, it will generate knot for every nodes and deformations result may lead to be too stiff
since beam element B32 expanded to C3D20 so the performances are probably bad for plasticit behavior as mention above…
Great, thank you very much for sharing this. It’s an interesting example to study non-linear buckling problems. I will let you know if I find anything else interesting on the topic of elastic-plastic bending. I’m still interested in cases like simply-supported beam with a rectangular section, subjected to UDL and possibly with hardening included.
For my PrePoMax tutorial case with plasticity (in which I verified only the deflection), I get the following equivalent plastic strain values from integration points of a critical element:
I think the point I’m checking now requires larger peeq values (>1). Your example looks very accurate anyway. Nice vid.
It has recently emerged a curious effect that makes Plastic models behave like if they had some strain rate dependency.
We are looking at that. Maybe you can join the discussion.
I have computed Prof Kraska example tensile test of a wire which reach a PEEQ of 2.
Apling the displacement with a different Strain rate (Let’s say a sinus function) the final PEEQ ends up at 1.7. (Exactly the same mesh, same material ,properties and same time step.
That is a 16% less equivalent plastic strain and I don’t really know how to read that result yet or which is the right one.
Is there an explanation for this?.
Someone has suggest there is some imperfection needed to properly initiate the necking but this can’t be done on a real model as one doesn’t know where the plastic behaviour will start.
