Torque + Force

[Roland]

Dear FEM forum,

Here is a beam with an eccentric force, F (black):
.

Beam_torqued-bent.png (16.39 KiB) Viewed 3884 times

.
Force F can be analyzed as a central force F' + a Torque T (both red).
I want to analyze the strength and displacement of the square beam profile. The little arm on which force F is applied is of little interest to me. I would rather draw the (hollow) square beam profile in FreeCAD, and use FEM to do the calcs.

Question: I cannot find a Torque constraint in the FEM WB. Or does it exist? If not, I assume that I need to include the little extension into the model and make it very stiff. Is that correct?


Greetz

Roland

[NewJoker]

The application of torque in FEM usually requires special considerations since the nodes of solid elements don't have rotational degrees of freedom. Shell and beam elements have this DOF available but for shells, we usually still don't apply torque directly. For both solids and shells the most common approach is to use a constraint that will couple the motion of selected nodes to the motion of a selected reference node. In CalculiX there are two basic types of such constraints: rigid body and coupling (kinematic or distributing). Unfortunately, they are not supported in FreeCAD at the moment. Some workarounds are discussed in this topic, among others: https://forum.freecadweb.org/viewtopic. ... 0&start=10

[Roland]

Thanks NewJoker,

I did find an approach that is executed by FEM WB, and perhaps gives a sufficiently reliable result. (that should be evaluated some way or another, and perhaps also looked at from the perspective that you just sketched here above).

My process was as follows:

• I defined the beam as a couple of faces. To simulate that their thickness (see next bullet point) is projected equally into two normal directions, I defined my faces in between the actual outside and inside faces of the beam.

• Gave the faces a thickness (FEM WB: shell plate thickness).

• Simulated a torque by two forces along two edges.

Simulated Torque on Beam.png (20.47 KiB) Viewed 3784 times

• Applied a bending force along one end face

Force on beam.png (21.44 KiB) Viewed 3784 times

The displacement result is as one would expect:

DisplacementResult.png (43.7 KiB) Viewed 3784 times

As said, this result should be challenged e.g. by a 'manual' (brainual?) calculation.

If I understood you correctly, your comment was about FEM & solid elements. But please note that I did not employ solid elements, but rather faces that is given a thickness by the math of FEM WB. Would your comment also apply to my approach?

[NewJoker]

This approach seems correct (if the beam has a rather thin hollow cross-section) but I also think that it should be verified using analytical calculations (treat it as a thin-walled cantilever beam under combined loading) or a model that utilizes the aforementioned rigid body/coupling constraints (you could just export the input file from your current setup, add the constraint definition as described in the linked thread and run the analysis using standalone CalculiX). If you share the model I will try to do such verification.

Yet another way to ensure the correctness of this simplified approach would be to add the lateral part mentioned in your first post and apply force directly to it.

[Roland]

The beam is a standard hollow cross section of 120x120x10 mm. Length 1000 m.

I shall gladly share the model with you, and greatly appreciate if you could make a check. I am not familiar with the CalculiX tools that you proposed. My analytical skills are limited approaches learned 40 years ago, and forgotten since (but I could, and perhaps should, recover those).

Anyway, I attach the model. I removed the results from the file to reduce file size. So the solver needs running again (10 sec)

Best wishes

[NewJoker]

So far I compared the results obtained using your approach with those obtained for the model involving rigid body constraint to transmit the torque and concentrated force. The agreement is very good:

paraview.PNG (102.29 KiB) Viewed 3603 times

I forgot to ask - what is the length of that arm to which the force is applied creating eccentricity and what is the magnitude of this force ? Knowing that I will be able to compare the results to the model where rigid body constraint replaces the arm and only the concentrated force has to be applied while the torque will be generated naturally.

[Roland]

That 's a nice result New Joker. Thanks!

Which file should Paraview open to evaluate the results in that viewer? I tried a few, but so far I failed.

I made a comparison with an analytical approach. I split the problem into 2. 1/ Bending of the beam and 2/ Torquing the beam. I developed analytical solutions for the two and also executed those problems in FEM. A first very important result was that I discovered to have made a mistake in the data input in FEM (Torque forces too large). The second result is that the solutions of the bending problem differ only by 1% from one another. The third result is that the torsion solutions differ by 14% (FEM yielding the larger tensions). This is OK for me, as this is a safety calculation for me.

The analytical approach is clearly explained on:
https://engineeringlibrary.org/referenc ... ess-manual
https://engineeringlibrary.org/referenc ... ess-manual

A further refinement that I used: I projected a torque force on 4 sides rather than 2. (Ensure to divide the total force by 4).

Docs attached.

Your question: Length of that arm to which the force is applied creating eccentricity and what is the magnitude of this force ?
10,000 N at 0.25 m

[NewJoker]

To post-process your results in ParaView you just have to export them to vtk format (FreeCAD offers such an option). Then you will be able to import them directly to ParaView.

Regarding the comparison with the analytical solution, here are a few things to keep in mind:
1) you can verify the results of the simulation involving both torsion and bending, just use the combined loading approach known from mechanics of materials to calculate the von Mises stress:

σ_vm=sqrt(σ_b^2+3*τ^2)

2) if you separately compare the normal and shear stresses with analysis then you shouldn’t display the von Mises stress but proper components of the stress tensor instead (the differences can be quite big), in the case of shells this can be quite tricky since they use a projected local coordinate system
3) avoid querying the stresses at the regions where distortions from numerical model’s simplifications occur (boundary condition, rigid body constraint, material overlap in shells and so on)
4) this cap on the top of the beam can have a negative impact on the agreement with the analytical solution
5) in analytical calculations we usually ignore the fillets
6) shell elements in CalculiX don’t use true shell formulation, they are internally expanded to solids and may not give as accurate results as other codes in some cases
7) in the case of 2D display of results on shells it’s important to ensure that stresses are taken from the proper section point (integration point through the thickness)

[user1234]

Simulated Torque on Beam.png

If you do something like that, be warned, you must apply the torque (or better said: force) in more instances and angles, else you only shear the beam and the result is invalid. Also the rotation deflection should be very low, because the applied force on the vertexes do not turn with the rotation deflection.

Greetings
user1234

[Roland]

in more instances and angles,

Thanks, User. Actually I did that like so:
.

MoreInstances&Angles.png (19.04 KiB) Viewed 3283 times

This FEM evaluation gives a 14% larger sheer stress than an analytical solution. For the purpose of my analysis this is OK.

Best wishes,

Roland