Thank you for your patience and such great commitment in deciphering my text with errors.
1 Like
The author of the program probably also encountered this problem:
Did you apply opposite moments (one positive and one negative) and did you use the same simple supports ? I’ve tried it yesterday and I think it wasn’t so bad.
Where is this long quote from ? I can’t find it when I search for the exact strings.
I would say that symmetry, rigid body constraints, buckling or nonlinearities and shells indeed are problematic combinations, especially in CalculiX due to its significant limitations. It’s often better to avoid rigid bodies, sometimes even symmetry (particularly for buckling problems), but more importantly, it often makes sense to use solid elements (at least for part of the model, e.g. where rigid body constraint is applied).
Yes, it’s a major limitation of CalculiX. As I’ve mentioned, its dev decided to prevent the usage of rigid body constraints with shells even in linear analyses in the newest release of CalculiX (not yet provided with PrePoMax), but I asked him if he could allow it for linear cases.
Here’s a list of the most important known CalculiX limitations: Known CalculiX limitations
1 Like
I applied only one moment, at the end of the beam. Where it theoretically should be. At the point of symmetry, only BC.
What Poisson value are you using?
1 Like
Validation Poisson Ratio is 0.3 Your deviation is : 2.15%
With Solid Elements C3D8I, 0.3 Poisson and Moment applied directly as Moment to RIGID BODY REF node deviation is 0.14% (4334 KN*cm).
Quite different Stress Distribution.
1 Like
Thanks for your help.
I wanted to compare PrePoMax to a commercial program using shell elements. Just like in the PDF file.
The result is very good.
Submitting your initial model (the same input deck) in Abaqus (on which CalculiX is based, but Abaqus has true shell elements) yields the following results for the full model:
And for the model with symmetry:
Later, I can check how different types of elements (including solids) perform in this solver for that benchmark case.
Thank you for your involvement. I admire your perseverance in running this forum. In this case, you misunderstood me. I used data from a simple engineering program as a comparison. There are few companies that use ANSYS or ABAQUS. Even fewer people can handle them. In your results, I only see deformation. Probable for buckling mode 1. That’s also good. I can’t read the forces or critical moment. This type of problem is fundamental in the design of steel structures in construction and the verification of engineering programs. I’m sure there is a large group of people interested in these results. I apologize for the confusion, but I don’t always find the time to respond and try again.
I often share results from Abaqus mostly because CalculiX is directly based on it (it’s pretty much its open-source version). To the point that the keyword syntax is pretty much the same with small differences (Abaqus has more options). Of course, Abaqus has more robust algorithms and better element formulations. In this case, its main advantage is that shell elements equivalent to CalculiX ones are not internally expanded to solids. Also, you can often exclude solver error this way - CalculiX has some major limitations and bugs (also related to unusual shell formulation - the screenshots from Abaqus show e.g. that symmetry works equally well when there are no such issues).
The screenshots indeed show the deformed shape of the model (the displacement values are irrelevant), but more importantly - at the bottom of each screenshot there’s “eigenvalue” - this is the buckling factor you also get from PrePoMax. Here, it’s 1036. The model definition is the same as in CalculiX - the input file was used directly in Abaqus due to shared syntax.
1 Like
This is from a frequency step. Are you evaluating natural vibrations of this model now ?
The results are different 1036 vs 993.1227 ?
Yeah, eigenvalues are common for both linear buckling and natural vibration (eigenfrequency) calculations. But what I got, is a linear buckling eigenvalue = buckling factor. I obtained 1036 instead of around 993 by only changing the solver to Abaqus (btw. PrePoMax even can even serve directly as its preprocessor) and thus using true S4 shells instead of expanded ones (those in CalculiX become a single layer of C3D8I elements).
It’s a free LTBeamN software, right ? Mentioned on this blog: Zagadnienia związane z "Belka stalowa stężona i nie zabezpieczona przed zwichrzeniem w klasycznym podejściu normowym" (there’s an interesting statement about the practical usage of this software and classic formulas at the end of the article)
I wonder if it’s possible to refine the mesh in that software and see how this affects the results.
1 Like
Yes, I use it sometimes.
Distributing the load linearly across the whole section and not only the flanges. 4346 KN cm.
Pressure of 1*z/7.99898743560001 KPa (z units in mm)
Signed Von Misses for the Static Solution.
1 Like
What does the mesh look like?
Is this result from PrePoMax?
Was the load applied to the nodes as concentrated forces?