Simulating Pinned Connection Nastran In-CAD

[ben.steelGXHRA]

Good day,

I am trying to simulate a pinned connection as part of a H-Frame bearing press below using a linear static study.

I don't think the behaviour of the assembly is correct and may be due to the way I have setup pins.

I am now using a simplified model similar to (https://knowledge.autodesk.com/support/inventor-nastran/troubleshooting/caas/sfdcarticles/sfdcarticl...) and went the route of beam elements and rigid body connectors to simulate the pin, following the tutorial as close as possible.

When I run the analysis, the beam element does not bend as expected, but rather hinges in the centre. Is this the correct behaviour or am I missing a something? Another concern I have is that the holes for the male and female clevis become misaligned. The pin does not fail in shear so I imagine the holes should stay aligned even with the exaggerated deformation shown.

The bottom face of the model is constrained in all directions and a 30000N load is placed on the top face. All surface contacts are separation. I have also tried using a surface contact between the inside faces of the clevises and the beam element to see if that fixes the alignment issue, but appear to make no difference.

Any help would be greatly appreciated.

Thank you.

Ben

[Roelof.Feijen]

Can you share your simplified model?

[ben.steelGXHRA]

No problem.

Attached below.

[Roelof.Feijen · Accepted solution]

Hello @ben.steelGXHRA ,

The problem is that the sketch point is disconnected from the node created on the line elements.

What you need to do is created two lines. One from the beginning to the sketch point, the second one from the sketch point to the end.

Now you know for sure that the end of a line a node is being created an d that it is connected with the sketch point.

[Roelof.Feijen]

I ran the analysis too, without editing the end releases.

When I run the analysis, the beam element does not bend as expected, but rather hinges in the centre. Is this the correct behaviour or am I missing a something?

I think this is due to the small displacement of 0.028 mm and the exaggerated deformation plot.

Another concern I have is that the holes for the male and female clevis become misaligned. The pin does not fail in shear so I imagine the holes should stay aligned even with the exaggerated deformation shown.

Have you tried to simulated it with a rod made of solid elements? It will probably show you the same "misaligned" results.

I have also tried using a surface contact between the inside faces of the clevises and the beam element to see if that fixes the alignment issue, but appear to make no difference.

I have no experience with contacts between a surface and beam element. Never used it like that. In that case I would model de rod as a solid model with solid elements.

Hope this helps.

[Roelof.Feijen]

Below the results I get when I use a rod. Note that the rod has been hidden in this plot.

Max. Deformation results is 0.036 mm.

[ben.steelGXHRA]

Thanks Roelof,

I get 0.028mm with the single line. I agree it must be the exaggerated deformation.

What diameter and material did you use for the solid rod? I used Steel-Carbon and 25mm diameter. All separation surface contacts and got max displacement of 0.067mm.

Ben

[Roelof.Feijen · Accepted solution]

I used Steel-Carbon and 25mm diameter. The only difference: I used Separation/No Sliding.

If I use Separation I get the same displacement results.

[ben.steelGXHRA · Accepted solution]

Yep, I get the same.

Thank you for your help Roelof.

[dvc-stageco]

Hi Roelof!

How would you model the rod and its boundary conditions?

If the rod is floating in the holes of the clevises, it evidently leads to a singular stiffness matrix.

So, in my opinion somehow the rod has to be kept in place untill it is activated through the contact.

As you get results, I am curious how you approached this issue.

Thanks

Daan