I didn´t open the file, but are you sure that the surfaces were you have applied the loads are in the middle? Because even Abaqus is telling that is not simmetric your model/bc
2 Likes
the shell model using linear element type (S4 & S3) it expanded to C3D8I and C3D6 element in CalculiX. The behavior of linear shell element in bending are known not so good, specifically for S3.
probably, quadratic element type (S8R & S6) with layering could be better. The advantages of CalculiX approach is in nonlinear plasticity and contact. Actually, it’s a truly solid element not a shell.
1 Like
Its OK, the Abaqus agrees with Nastran…thats all thats needed…perfect symmetry is not what the issue is…its that Calculix approach gives bad answers for large shells…
propably linear triangular shell element cause of locking, since the location is in high stress zone (supported column). It can give insight when the mesh model is converted to quadratic.
Just by changing the legend you get the below displacement plot, which is similar to Abaqus and Nastran.
Considering the span is 100 inches, the displacement difference between the two solvers is roughly 0.16%.
Your mesh is not enough fine to capture the real deformation of the structure, even NASTRAN and Abaqus are showing bad results due to the poor mesh. Refine by two at lest the mesh of the plate and reinforcement, and change to second order elements in both softwares (CCX and Nastran), and not only the results will be more closer between them (displacement about 0.7in), but also the deformation will be more simetric as it should be.
A convergence analysis is a god practice to make sure of the results.
3 Likes
I played with your model, and the first thing you need to change is the element order. In Caclulix, a linear shell element is expanded to a linear solid element, which is not accurate for bending loads. That is why the plate under the load does not bend as it should.
The second thing you must do is make a mesh convergence study. Not all codes are equally precise, so if you want to compare the results of different codes and check if they work, first make a convergence study in all of them and compare the converged results. That way you will be comparing the “right” result obtained by the selected code. Especially in this case where one code expands the shell elements into solids.
3 Likes
Agreed, the OP should refine the mesh. There are some high aspect ratio elements that are creating dissimilar contact patterns between the legs and the table top and obviously resulting in the asymmetric displacement plot.
The von Mises stress plot clearly shows this.
1 Like
The source of the error could be the single layer of elements under out-of plane shear load close to the supports. As an alterntive or additionally o second order elements you could try a composite shell with more than one layer, this is expanded into multiple layers of solid elements. Yet I didn’t see where to specify that in PrePoMax.
1 Like
Looks like you are comparing who is less bad. Result is not symmetric and that is not acceptable. You just need to work a little more on your mesh and all software’s will find at the end. Another result with calculix+Mecway just improving the upper mesh.
Result is .61 inch
NOTE: Large spams are very sensible to the BC at the suporting areas. It happens the same with cantilever beams. Small changes at the supoorting area can make a big difference on the tip deflection.
2 Likes
I understand that you may feel disappointed by calculix, but to say that it is a “trap” is a bit of a stretch. Also, in case you did not read the disclaimer in the calculix site:
Copyright (C) 1998 Guido Dhondt and Klaus WittigThis program is free software; you can redistribute it and/or modify it under the terms of the GNU General Public License as published by the Free Software Foundation; either version 2 of the License, or (at your option) any later version.
This program is distributed in the hope that it will be useful, but WITHOUT ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or FITNESS FOR A PARTICULAR PURPOSE. See the GNU General Public License for more details.
You should have received a copy of the GNU General Public License along with this program; if not, write to the Free Software Foundation, Inc., 675 Mass Ave, Cambridge, MA 02139, USA.
The burden is on the user to do the proper tests and make sure the software works for their application. If not, you can also modify the code yourself and fix whatever you need to fix.
This is also true for paid software like nastran or abaqus… most experienced guys here probably submit bug reports to those paid packages all the time.
1 Like
That was my first thought…
Im benchmarking Calculix vs Nastran … Solver benchmarks are done using the same mesh order of elements…So Im comparing 1st order linear elements of Calculix vs the ones in Nastran using same mesh
What are the details on how this is done?
The problem with Calculix is the benchmarks in the documentation show that its accurate, but when you run 1st order elements the results are total garbage. I feel that the authors are not being honest about its capabilities. 2nd order elements give good results, but had to figure that out the hard way
To change the legend, double-click on it and switch the Min/max limit type from Automatic to Manual. Then set the Min value and Max value as you wish.
Well, Abaqus may also give totally useless results with too coarse meshes or incorrectly selected element types (their choice depends on a given problem). Here it may just be more pronounced because of the expansion to solids.
I hope you realize that you are using a free software. In order to use free software you must usually do a little more investigation into how it works and performs. And it will not always perform as well as commercial tools but it is free and the choice is yours.
Even the result you got on the first try is about 20 % away from Abaqus’s result so I would not call it total garbage.
4 Likes
Yeah, CalculiX may have some bugs but it’s incredibly powerful and user-friendly (which is not common in FEA) for a free software and usually gives results as good as those you can get from commercial software (there have been many comparisons). It may just require some additional considerations and getting used to its characteristics but it’s definitely worth it. We’ve seen here examples of large shell models solved with success. If you want to get accurate results, mesh convergence studies are always a must, regardless of the software. We do them in Abaqus too and often find huge differences for meshes that are too coarse and/or use wrong element type (and in Abaqus the choice is way harder since you have many special types of elements).
2 Likes
I think @pano is completely right and it would be counterproductive trying to convince anyone without enough skills to use CalculiX. I encourage you to keep using Nastran.
Those expensive tools are more prepared to digest input garbage up to a certain level.
6 Likes
Not Abaqus with its strict convergence criteria, overconstraint checks and so on. Unless you just run linear or explicit all the time and don’t check the results carefully. Then you don’t have to worry about convergence and pretty much anything can pass. CAD-embedded FEA modules are on another level though. They often make sure the user doesn’t have to worry about anything else than applying fixed constraint on one side and force on the other side. Even material and mesh definition is often done automatically and without bothering the user with the display of ugly coarse meshes 
2 Likes