Hi, I am working on a simple shell buckling example (cylinder under compression) and have defined a reference point with both shell edges (bottom and top of cylinder) with Rigid Body Constraint.
Linear Buckle results are fine, however, in a static step analysis I want to get the displacement and forces from the reference points and it is somehow not available ? Is this feature not yet implemented ? Is there any other way to plot the load displacement data ?
Best Regards
Ronald
Thanks, for the answer, I know, I can defined it like shown in your picture but if the analysis is
finished, there are no results to choose from, see pic below
There should be a .dat file with those results in the working directory. Check if it’s there. Sometimes it’s not written or loaded properly (then there should be an error message when opening the results).
yes, if I try to open the file, I always get this message:
is there a way to fix it? under which keyword in the dat-file is it? or another way to plot the force-displacement curve?
If I run the analysis in compatibiltiy mode, I dont get the error widget anymore but History output is still not available
It’s possible that the .dat file is in the working directory (Temp folder mentioned in the error message), just written in such a way (e.g. with duplicated time increments) that PrePoMax can’t open it. It might be also a fault of the restricted access in this directory so maybe try changing it. Of course, you can access the data in this file manually (if it’s there) and plot it e.g. in Excel. It’s just a tabular output similar to Abaqus.
Ok I am step ahead, If I select per History Output only ONE Variable for a reference point (RF or U) then it works, I do not get the error message (that the dat cannot be opened) and can select the history output results. The results are as expected for U but for RF I get for all componentes basically zero (float E-13).
Looks like the sum of the nodal forces is not caluclated properly with respect to the reference point.
So in your case RF 1 has prescribed U3 displacement ? What if you request RF from RF 2 (fixed bottom) ? You don’t need the Totals=Yes setting here as those are individual ref points. But you could also try replacing rigid body constraint with directly applied BC and requesting history output for the nodes on the edge, this time with Totals=Yes. Especially since there are known convergence issues in CalculiX when rigid body constraints are used with shells and Nlgeom.
yes RF-1 has prescribed U3 disp. Reaction forces are zero (float E-13) at RP-1 and RP-2. I try with direct BC although it is MUCH less convinient. Problem is I want to add multiple loads later on in the model (2 Forces and 2 Moments) which are not so easy to add in a direct manner. I will update further findings.
If you share the model (not necessarily here, you can do it via private message but some hosting website would likely have to be used either way), I will take a look at it. I had a similar case in one of my tutorials: https://www.youtube.com/watch?v=Jq2mKRZmIsQ
Sharing the file would help determine what is wrong with the .dat file reader.
“Sorry, new users can not upload attachments.”
How long do I have to wait to be not a new user anymore?
I uploaded the inp to my Github
hnrwagner/PrePoMax (github.com)
Like I said History output works this way for me, but sum of reaction force RF3 is not properly calculated at reference point 1 and 2.
MNA_IW1_HO_OK.inp - no correct reaction forces at reference point 1 and 2
MNA_LC2_10percent-S4.inp - History Output not able to read & no correct reaction forces/moments at reference point 2
You should be able to upload attachments now.
It’s interesting that it can’t read the .dat file when both RF and U are included in one request.
It would be good if you could share the .pmx file or .inp with a coarser mesh - this one is too refined (and thus takes too long to solve) for debugging purposes.
here is it
Tower2024.pmx (5.7 MB)
Ok, so I fixed the problem with reading the .dat file in case of buckling analyses.
However, I detected an additional problem when running the buckling analysis: if material plasticity is defined, the analysis fails. I could add a warning to PrePoMax, but I think this could be a bug in CalculiX.
Additionally, using shells and rigid connections does not seem to work at all in this case. Neither using Pasitx or Pardiso solvers. Pardiso throws an error, while the Pastix gives some garbage results.
The fix will be available in the next developer version.
that would be great, I am working with the guys from Eurocode for shell buckling design and we want to write a new publication where we compare different opensource FEA codes and I want to present the results from PrePomax. Also I want to use PrePomax for teaching in Germany and upload some video on my youtube channel
Best Regards
Ronald
Hi hnrwagner,
I also like Buckling analysis.
I looked at this shell. Take into consideration that ccx expands shells into solids and that Fixed ends require a special treatment to assure there are no rotations in the BC area. Take a close look at your results , especially in the lip and you will notice how it is rotating even you have defined a Rigid Body BC.
Not sure how much difference it could make but if you will publish some comparison it’s work to take this into consideration.
Buckling load is almost the same but Buckling shape is quite different. Wavy patterns move away from the lip.
|7896| [ N ]|Result with Transform + Kinematic| (S8R)
|—|—|—|
||||
|7889| [ N ]|Result Rigid Body| (S8R)
hello, welcome to the forum. I enjoyed all advanced of video list, thank you for sharing and interesting in opensource also. Some video posted explains about continuum shell element in Abaqus, probably this nearest one to shell element in CalculiX, not a classical.
Abaqus need specific approach in meshing and modeling at intersection, but CalculiX does it automatically by the knot.
The new 2.1.4 version should be able to read the buckling output from the .dat file. Please give it a try.
