Torsional Spring - SPRING2?


has anyone an idea how to generate correctly a spring with only torsional stiffness (and no other stiffness like axial or bending) between two incident nodes of two rigid bodies?

*Rigid body, Nset=n_k1g, Ref node=1537, Rot node=1538
*Rigid body, Nset=n_k2g, Ref node=1539, Rot node=1540

This is not working, because the “Rot node” of a *Rigid body is only a dummy node and should not contain any element with respect to the documentation.

Is it possible to connect all nodes from one node set with their pilot node with beams to use all 6dofs at the pilot node and use after this SPRING2 with all 6 dofs?

Kindly regards

That’s interesting, I’ve never thought about such a limitation. Intermediate elements could help as a workaround but maybe it’s enough to just replace rigid body constraint with coupling for example.

Hi MArkussS , Calc_em,

I have tested appling a tangential stiffness per unit area to a rotating disc by means of the elastic support option and it behavesperfectly linear as far as I have gone (3Dstatic). Normal Stiffness =0 to not interfere with the other dimensiones. One load on each corner for the test.
Pictures shows we could go further with nonlinear too.


1 Like

I am trying to figure out how the Spring(1, 2 and A) elements work in CalculiX and as I understand the documentation, Spring elements only connect degrees of freedom from 1 to 3. That is not written directly in the documentation and is a little confusing. So the question is, is it possible to use rotational degrees of freedom 4, 5 and 6 in the Spring elements? Any ideas?

I think that the spring should be connected to the rotational node and apply the stiffness to the corresponding dof (1,2, or 3) for the rotation.

Could you try:


Right, it seems that rotational springs can’t be defined independently. I tried to solve this basic example:

1, 0, 0, 0
2, 1, 0, 0
1, 1, 2
4, 4
N1, 4, 4
N2, 4, 1

I obtained correct results in Abaqus but all zeros in CalculiX.

Thus, some workaround and attachment to the rotational node are needed, as you said. The question is how to create such a node. As noted by the OP, rigid body constraint uses a dummy rotational node so it won’t work. Then is it necessary to attach the spring to a beam, for example ?

hi All,

CalculiX only have translational springs, to modeling rotational spring some possibilities are shown in figure below. required eccentric two spring element (Kt) in the model and one additional nodes (red dot) connected by infinite stiff element or rigid body (gray line).




Ok, thank you for the confirmation. And definitely, the workaround you propose is something that can be done.

I would recommend that some note might be added to the CalculiX documentation that spring elements only support degrees of freedom 1, 2 and 3. Is this possible?

1 Like

actually i doubt about my understanding (hope i could be wrong), but several times i read the documentation there’s no words or equation regarding to rotational springs. also for now, i’m interested only at SPRINGA element due to it’s simple defined and nonlinear capabilities.

1 Like

Right, but personally I also think that it would be good if the documentation included a note about rotational springs (saying that they aren’t normally supported and workarounds are needed). That would help other users avoid confusion. Especially that CalculiX’s springs correspond to the ones available in Abaqus where rotational DOFs are supported.



¿Which kind of problems are solved with torsional springs?
¿Are you looking for something like it is shown in the vid.?

Sometimes torsional springs are used in analyses of simple mechanical systems. Here’s an example:
from this article:

Torsional springs can also be useful when modeling some real-life mechanisms such as door latches, precision mechanisms, levers, ratchets and car components.

Do you mean to couple the force P with the rotation of the base by means of user defined Spring Constant?. ¿Like a cheap kitchen scale?. I will try.


NOTE: I have test the *RIGID BODY card on my windows 10 machine (calculix ver 2.18) and it doesn’t work for shell elements on any of its options (ELSET or NSET).
If I extrude the shell elements to solids it works.
¿Is this a limitation of Calculix?. I don’t see it referenced in the manual.

Or a mouse trap :wink:

Strange, it always worked for me with shells but maybe it’s a matter of preprocessor. Can you say more about this issue ? Do you get any error messages ? Can you share the file ?

Here’s an exemplary shell model solved with rigid body constraint (force is applied to the top edge of the shell this way) using ccx 2.18:

Something like this?

NOTE: I have confirmation that there is some issue with shell elements and rigid body in the preprocessor. With solids it is possible, no problem.

WeTransfer - Send Large Files & Share Photos Online - Up to 2GB Free

Yeah, looks great :smiley: How did you model it ?

Sorry Calc_em

I posted the file and short explanation in the Mecway Forum. The inp files that the software generate do not directly work with ccx and it would be hard and large to explain. You won’t belive it works . :astonished: :grin:

spring element are common in FE, let me add some example application of rotational spring element simplification. is a foundation pile required to resist ~3000kN ultimate loads in column for normal force only, or smaller value when moment being existed.

this could be simplified as rotational spring and translation spring at column base supports, the value’s about 15000kN/m (one pile). many structural analysis application has feature rigid link to connect between each of individual spring element. the spring can be nonlinear based on force displacement of pile loading test results.

even these models are simple enough and fast, still could be more accurate rather than using solid element models cause of complexity in the interface behavior (cohesive zone) and soil inhomogeneity, compaction driving, saturated, etc.

(an example taken from this report)

another how is useful these element are in analysis of steel portal frames, pinned (rotational released) or rigid connection only method of analysis simplification and could lead to far enough from actually. the behavior can be predicted better by using spring element, known as semirigid connection or partially restrained.

sound like more civil/structural engineering ways rather than mechanical or aeronautical. but FE itself is a general purpose, even for a bone analysis.