The model only converges when NL geom is activated if I remove the translational constraint along U2.
My issue is that I want to solve this case without applying any boundary conditions on the point pForce except for DR3, because I know there will be a rotation due to having only one screw. However, Iâm wondering if, using this approach, the beam will still account for shear.
Do you need Nlgeom ? I think it could be skipped at this stage. It often causes issues in CalculiX, especially with shells and rigid body constraints (hence the error in ccx 2.23 we talked about). Itâs better to avoid having to many nonlinearities in the model and in CalculiX even rigid body constraints and shell expansion introduce it.
strange, connecting rotational nodes of rigid body should transferring moment and generate shear also but results shown not.
result in case Fy only,
In my case due to large sliding the modele donât converge if NL geom is not activated.
Ok, I understood it in an opposite way - that with Nlgeom it only converges if you remove the U2 constraint.
1 Like
I found an interesting trick some years ago that works well if you use beam as connector.
It can be difficult to get in prepomax because there are not beams available right now.
The idea is that your beam element is of type circular or tube and it extends beyond the hole .
Both extremes of the beam have bigger diameter than the main body so they become the nut and head. The interesting part is that those wider part of the beam (under ânutâ and âheadâ) is a selectable surface that can be used to establish a tied contact with the plat e.
No rigid bodies involved. Nonlinear and preload is supported. It can sustain tension, bending , shear or whatever you ne ed.
1 Like
Sometimes shells are added to 1D beam models in a similar way, even in Abaqus:
(Modeling Bolted Connections in Abaqus FEA)
FreeCAD FEM has beams, but mixed element meshes are not yet supported so indeed keyword edits are necessary to add beam to such models. In fact, it might be easier to export the input deck and add the necessary keywords using a text editor before submitting the analysis in CalculiX.
However, to be honest, I still think that highly simplified solid bolt models are the best way to approach such problems in CalculiX (especially involving shear loading). Even when there are more bolts, itâs quite easy to define them while avoiding several issues with 1D elements and coupling/rigid body constraints.
indeed, even clamping at bol head and nut generate bending still bearing plate hole and shear transfer mechanism does not represent well. Probably, an automatic bolt mesh generated internally in PrePoMax can be useful since working as part assembly.
in case of shell model with large number of bolts, spring element seems to be more convenient, and bolt nonlinear response in axial and shear can considering in analysis also.
FreeCAD has add-on Fasteners workbench, making it easy to add standard solid bolts to CAD geometries. Their heads and nuts are detailed, but could be simplified. Or one could prepare simple parametric cylinder-based bolt geometries and add them to models when needed. Another option would be to prepare a hex meshed bolt and scale, then move/pattern it in PrePoMax. IMO simplified solid bolt models will always be superior, especially when the software doesnât have such robust 1D elements for this purpose.
Thank you all for taking the time to answer my question. Is there any way to merge or constrain the REF and ROT nodes together? I understand that modeling the bolt in full 3D is the best option, but I need to use an RBE to simplify one of my models. I want the RBE bolt to become an option for now and for future calculations. Thatâs why Iâm open to any possible solutions.
In the case I want my bolt to work only in compression, can I follow this method by modeling only the beam REF node?
REF and ROT nodes use the same DOF numbers (1-3), but in a different way (as translations for REF node and rotations for ROT node). Basically, translational DOFs of ROT node are interpreted as the rotations about the REF node. Thus, the ROT node coordinates are irrelevant. I wouldnât try to merge or further constraint them, especially since rigid body constraints are internally treated as nonlinear MPCs and any additional constraints can easily cause overconstraint in the model.
Perhaps you should try coupling constraints instead (they are the closest equivalents of Nastranâs RBEs). They are covered in detail here: Different coupling constraints and their limitations - CalculiX (official versions are on www.calculix.de, the official GitHub repository is at https://github.com/Dhondtguido/CalculiX).
Might be better to ask about that there (on the CalculiX forum) since coupling constraints also arenât available in PrePoMax yet and require keyword edits. Combined with beam elements, you may end up exporting the input file from PrePoMax and editing it outside of it.
Thatâs a nonlinear behaviour. You can get it with my proposal defining the contact as Unilateral.
My proposal is not a mixed element mesh as ABAQUS. The bolt, nut and head are beams.
When talking about bolts I have the feeling we usually end up at the same point.
No matter the answer or proposal, there is always some complain mainly because it is an idealization and itâs not assumed there is a sacrifice behind.
We search for a âsimplified bolt connectionâ. Simplified in which sense?.
1-Simple to set up?
2-Simplified because we are only interested to keep the parts toghether?
3-Simplified because I just want to use a couple of elements?
4-Are you interested in the bolt response, the hole area, both?
5-Symplified aproach comparable in results with some other software?.
6-Simplified because Iâm only interested to meassure forces, or moments,âŚ
First think is to warranty the convergence. No matter how âsimpleâ it is a proposal, if it doesnât converge, itâs useless. Once it works we can start talking about the range of validity.
Which are the relevant DOFâs?
So just regular (nonlinear) contact (hard or sotfened) instead of tie constraints (to clarify if someone is looking for corresponding CalculiX features).
But the parts being connected are not beams.
Yeah, it all depends on the goals/requirements of the OP. In Abaqus or other similar software, the choice is usually easier - couplings + beams/connectors are sufficient in most cases. Sometimes (less frequently, at least for larger assemblies which are the most common models) simplified solid models are used. However, in CalculiX, there are many limitations and multiple workarounds exist. Their choice depends mostly on what behaviors are to be captured, what outputs are needed and what modeling effort is required.
itâs a beam i guess, using tied contact at end. This is undocumented, i found this can be work when first discussed with Victor at CalculiX forum about beam contact with shell face.
I mean the OPâs model and the standard models with beams where the joined structures have to be modeled with shell or solid elements.
tâs largening diameter of additional beam for bolt head and nut, then use tied contact connected to solid face probably.
My point is just that FreeCAD FEM currently allows only one element dimensionality (beam, solid or shell) in the same analysis. PrePoMax doesnât have this limitation, but doesnât support beams. So one could e.g. create beams in FreeCAD FEM and copy their definitions to an input deck exported from PrePoMax. Individual beams can be easily defined by hand, but their more complex combinations could warrant such an approach.
Thank you for the detailed questions. I will try to clarify my objective point by point.
1 â Simple to set up?
Yes, partly. I am looking for a solution that is reasonably simple to implement and easy to modify in the model.
2 â Simplified because we are only interested in keeping the parts together?
Yes. One of the main objectives is to ensure that the bolt keeps the connected parts together.
3 â Simplified because I just want to use a couple of elements?
Yes. I would like to keep the model lightweight, so using only a small number of elements (beam elements) is preferred.
4 â Are you interested in the bolt response, the hole area, or both?
My main interest is that the beam behaves as a real bolt would. In other words, it should generate both axial (tension/compression) and shear reactions so that I can observe the resulting stresses in the structure.
Additionally, I would like to recover the forces in the beam in order to size the bolt separately.
5 â Simplified approach comparable with other software?
Not necessarily for comparison purposes, but the results should of course remain physically consistent.
6 â Simplified because Iâm only interested in measuring forces or moments?
Yes, mainly. My goal is to measure the forces transmitted through the bolt so that they can be used for bolt sizing.
Regarding the relevant DOFs, my understanding is that the most important ones are the three translational DOFs (UX, UY, UZ), since they control the transfer of axial and shear forces between the connected parts. Rotational DOFs may also play a role depending on how the beam is connected to the surrounding structure.
Another important point for me is not to over-constrain the model. I would like to avoid introducing artificial boundary conditions (for example blocking certain displacements) that could make the model numerically stable but physically unrealistic for some of the load cases I intend to study.