Modelling a Shackle - Pin connection in Inventor Nastran

[marius.buculei]

Imagine a Pin in a Shackle assembly with a Bearing Load applied in the middle. As the pin can rotate and also have small axial movement, how should I model the constraints using Inventor Nastran?

A simple Inventor FEA, where the supports (contact surface with shackle) are fixed, gives realistic results (sort of...), but a small play between shackle and pin will slightly bend the pin, and the contact will not be uniformly distributed on the whole axial contact surface.

Attached is a typical example, with red I've tried to highlight the bearing load applied.

Should I isolate the pin and replicate the shackle action using connectors? I'm completely lost, any help much appreciated. Thanks

[John_Holtz]

Hi @marius.buculei . Welcome to the Inventor Nastran forum.

I have added a coordinate system so that my description can use directions. This is what you can do.

1. Use separation contact between the pin and the holes in the shackle. As you mentioned, the bending will cause the pin to move away from some surfaces and possibly come into contact on the top (+Y) side of the hole.
2. The pin can rotate in theory, but it does not rotate freely in operation. It may rotate some angle but then stops in some new position. The new position looks just the same as the old position, so you can ignore the rotation and prevent the pin from rotating. If the face "A" is parallel to the XY plane, you apply a Tz constraint to the face. That prevents the pin from rotating freely about the X axis but allows the pin to move appropriately in all other directions. (This constraint also prevents the face "A" from rotating about Y which is not realistic, but that should not be occurring if the geometry, loads, and results are symmetric about the XY plane.)
3. The free motion of the pin in the axial direction is not important, meaning whether it moves in +X or -X in real life does not matter for the analysis. Fix a single point "B" in Tx direction will prevent the pin from moving freely in X but allow it to expand or contract in X and bend about Z.

Let us know how the analysis works out.

(It might help if I add the figure! Added now.)

John

[marius.buculei]

Hi John,

Thank you for the valuable information! Did you mean to attach a file, or am I just missing it?🙄

Would you analyze the shackle-pin assembly or just the pin part, and apply the constraints and bearing load as you've described?

Kind regards,

Marius

[John_Holtz]

Hi Marius,

Yes, I forgot to include the image in my reply. I edited the post to add it, so you may need to view it on the forum to see the image.

The analysis will include the pin and shackle parts. The contact will be defined as separation. See tips 18 and 19 in the PDF document attached to my forum post Suggested Reading - Tips and Tricks on the Inventor Nastran forum for the proper definition of the maximum activation distance input, depending on which method of contact you use.

John

[marius.buculei]

Hi John,

I really appreciate your support. I've tried to replicate your advice on the shackle pin assembly, but I ended up with huge stresses (over 100,000 MPa for a bearing load of 17 Tonne). I have simplified the pin, but taking out the threads, small greasing holes and engravings, got rid of the small anti-rotation plate at the head end and nut and split pin at the far end. I have also "machined" a small cut-out at the far end of the pin to be able to apply the Tz constraint. I've added the Tx constraint on an edge of the cut-out and sliding contact between the PIN and the shackle's holes.

I must be doing something very wrong.. I'm afraid... 🙄

[John_Holtz]

Hi @marius.buculei 

You need to look at where the high stress occurs and determine if it is a problem with the setup, or is the high stress expected. In other words, simulation is good, but it is not perfect. The mathematics are only an approximation of real life, so large stress values at isolated points is a common occurrence. (See Why do stresses keep going up when the mesh is refined in Nastran for example.)

Also look at the displacement values. If the displacements are reasonable, the stress is likely reasonable (other than a singularity at sharp changes where the results will never be accurate.) If the displacements are unreasonable, you should not trust the stress results even if they look reasonable.

Assuming Constraint 3 is the machined slot held in Tz and Constraint 4 is the Tx constraint, what is holding the shackle and resisting the load on the pin? The analysis needs to be statically stable in order to get the most accurate results.

Also, images of the results might be helpful. The model files would be more helpful so that someone can look at the model and tell you specifically what is wrong. See What files to provide when the model is needed - Autodesk Community.

John

[marius.buculei]

I can't thank you enough, John, for your support. I've "fixed" the top of the shackle, but also attached the model for you to review it properly, as the results haven't changed a lot. Very good the documentation in the links you suggested, but once identified the "corners" of high stress how can I remove them from the analysis to have a meaningful set of results?

I couldn't attached the FEA results files, due to size limitation (71MB), so just 2 screen captures. Even though the stresses are to the roof, the deformation is "realistic" around 0.2mm max.

[John_Holtz · Accepted solution]

Strange. The model you provided has no setup for the Nastran analysis. Did the pack-and-go file get created before you saved the file?

Based on the image, the maximum stress is "only" 10,000 MPa which is better than 100,000 MPa. 🙂 But all the stress that we can see in the image is between 0 and 400 or 800 or 1000 MPa. You need to check where the maximum stress is. If it is a single node, you ignore the values that occur at a singularity.

In other words, how much of the volume is in the acceptable stress range and how much is above? (Nastran will not show a number; you need to eye-ball it.) Set the "Results > Options > Contour Option > Specify Min/Max" range to get a better idea of how much is above the allowable. Changes are everything is okay.

John

[marius.buculei]

As I mentioned earlier, even after being archived, the FEA files (located in the InCAD\FEA folder) are too large to be attached here. I found a mistake in my analysis, where I didn't suppress the CONTACTS generated automatically, so running the analysis again, I got far more credible results. There is a way to double-check the results and they are very close to the calculated ones.

Boundary conditions are ok, thanks a lot for the tips. The stress results are very similar to the ones obtained from simple stress analysis on the pin alone, with fixed constraints applied to the contact areas on the pin (see attached), which encourages us to tackle more complicated assemblies in Inventor Nastran.

I really appreciate your support, I'd consider the issue raised solved.