I performed a three point bending test in prepromax, however I couldn’t really find an option to obtain a stress strain or force displacement curve for a particular node. There is an option of getting stress and strain from history output by selecting multiple nodes. But these are stress values for a single time interval for each nodes. I need to obtain a continuous stress and strain for a particular node for different time steps like we do in the abaqus software. Is there any options for this which I might’ve missed? Also even for the stress values for different nodes from the history outputs the values are shown column wise which is not so convenient for copying and post processing analysis in excel.
There are two ways:
- Request history output of stress and strain for a selected element (you will get the results from each of the element’s integration points then) or reaction force and displacement for a selected node before running an analysis
- Use Results → History Output → Create → From Field Output. Then you will be able to get the stress and strain as extrapolated/averaged quantities from the nodes. However, to combine them into a stress-strain curve, you would have to export the results to Excel or other software where you can plot data. Same with force-displacement curve.
History output will be created for each frame of the results if you run a nonlinear (or transient) analysis with multiple frames. When you request it from a single node or integration point, you have just one column to copy to Excel.
Here’s an example of a force-displacement curve: https://youtu.be/Jq2mKRZmIsQ?si=sHmJPLPREg5iwZLB
Thank you for your response, I could get the results in different time steps now when I turned the non linear geometry on. However why so do you know? I performed similar setup in the abaqus software with nlgeom turned off and it still works the way I expect. I am doing a three point bending test, my interest is only in the elastic region so I defined the youngs modulus and the poissons ratio only.
You need one of the following 3 forms of nonlinearities to trigger the nonlinear solution procedure and get multiple frames of results:
- contact
- nonlinear material model (usually plasticity, sometimes hyperelasticity)
- Nlgeom
There is a workaround in CalculiX with a dummy plastic material. It’s discussed in detail here: Bending Moment + Rotation Simulation
Thank you
I followed one of your videos ((2) PrePoMax (CalculiX FEA) - Tutorial 11 - Four-point bending of a sandwich composite beam - YouTube) for four point bending for my three point bending setup, however in the results stress contour (for misses, s22 etc) the stress concentration or the peak stress is always occuring on the bottom support where I defined a roller support with u1,u2,u3 as zero and other three rotational dof unconstrained. Can you please tell me what could be the possible reasons. I created a similar section of surface in the bottom two support regions like you did in your video for the loading section, I also tried switching the support to the corner section but the problem persists. The images contains the details of the problem. The peak stress is supposed to occur at the bottom tension region, I can also provide you the file if you need to do a quick check
In practice, supports in 3- or 4-point bending tests are typically modeled as rigid parts in contact with the beam to avoid such issues:
If you want to use direct boundary conditions, avoid applying them to edges unless it’s necessary. Sometimes they are applied to outer side edges to simulate simply supported conditions, but it’s usually better to use small surface segments.
Also, keep in mind that it’s recommended to utilize symmetry whenever possible. This not only reduces the size of the model, but also makes it easier to avoid its underconstraint.
hey I used a shell type rigid roller type contact for suppport and loading, however there are lots of issues. is the shell part selection the right way to do? we typically model the roller support for three point bending as shell discrete rigid element in abaqus,where we don’t even need to assign a material to the supports, However here in prepromax I see even though I import the rollers as shell element I have to define a material property , so I chosen a stiff property with very high modulus. Also should I create a separate step for the loading? How the contact between the upper face, lower face and the roller should be modeled? as thCere is a convergence issue occuring for hard contact. It would be great if you could make a video on three point bending with roller supports as it seems there is lot to look here, there are tons of videos and tutorials related to 3pb done in other paid version softwares but those procedure doesn’t really seem to be working in prepromax. Thank you for your patience
It might be better to avoid shells in this case, since there’s a known limitation of CalculiX. In short words, shells + Nlgeom + rigid body = non-convergence. So, unless you disable geometric nonlinearity, you may want to use simplified solid supports instead. But at least you can use rigid body constraint instead of workarounds with very stiff materials (those are necessary pretty much only in explicit dynamics with CalculiX). Just make sure to constrain all DOFs of their reference points.
I would strongly advise making use of symmetry if possible here:
This will make it much easier to avoid rigid body motions. Relying on contact to eliminate them rarely works. Of course, you may still need some additional BCs, but most RBMs will be taken care of.
Here you can find some similar examples (including 3- and 4-point bending including supports/punch) in the form of CalculiX input files: GitHub - calculix/CalculiX-Examples: CalculiX examples by Prof. Martin Kraska from Brandenburg University of Applied Sciences. Excellent starting point to master parametric modelling with CGX and CCX.