bearing loads and corresponding contraint

[Orion07]

Is it possible to apply bearing loads at all hole locations of the rod and still adequately constrain the model? Does anyone have any suggestions for this? The rod is in tension so the loads would be equal and opposite. I was trying to avoid doing a contact analysis. I've tried two different techniques:

1. Apply loads at the clevis end and constrain the bottom hole with free rotations
2. Apply a load at the bottom end and constrain the holes at the clevis with free rotations.

Both techniques give different stresses especially around the holes but also at the round in the neck region just below the clevis.

Any suggestions would be appreciated. Thanks.
View attachment 3695

 

[miya]

Orion07,

On your model, try any one of these:

1. "Inertia Relief"

- see attached image

2. "Three Point Constraint Scheme"

- see http://www.ptc.com/cs/cs_23/howto/mst727/mst727.htm

3. "Quarter Symmetry Plus 1 Point Constraint Scheme"

Thanks,
Ray.
---
Ray Miya


View attachment 3697

 

[Kaz Z06]

Orion07,


Ray's first suggestion is best, but all will work. One important point, your "free rotations" from your other ideas have no consequence. In other words, you cannot constrain rotations for solid elements. Only beams and shells can have rotations constrained or allowed to move freely. Solid elements do not respond to DOFs in the rotational directions and in a sense are already "free".


Cheers

 

[Orion07]

Ray- Thanks for the suggestions. However I have not been able to figure out how to apply them. I do not see the Inertia Relief check box in the Static Analysis Definition window. I am using Wildfire 2.0. Also, as far as I'm aware our license does not support Independent Mode for ProM, so I don't think I can use suggestion #2. Can you supply more info for suggestion #3? I see the quarter symmetry but how do I constrain motion in the Y direction (see above pic from previous post)? The y-axis is normal to only two surfaces which need to be able to deform in that direction. I apologize for my ignorance in advance. I'm a little rusty using ProM and FEA. Thanks.

 

[miya]

Orion7,<?:namespace prefix = o ns = "urn:schemas-microsoft-comfficeffice" />

Sorry for the ambiguity in my response. Below are further clarifications.

1. "Inertia Relief" is new functionality for WF 3.0. i.e. does not help you in WF 2.0. Another good reason to upgrade from WF 2.0 to WF 3.0.

2. Even though the Suggested Technique was written for Independent Mode, the concepts are the same for Integrated Mode. i.e. it is still applicable to you.

3. Cut your model in Pro/E. In Mechanica, apply two "Mirror Symmetry" constraints to those two symmetry surfaces. i.e. On your model, apply one "Mirror Symmetry" constraint on the XY symmetry cut plane, and one "Mirror Symmetry" constraint on the YZ symmetry cut plane. That leaves one rigid body mode of translation in theY direction. Just pick any point and constrain that point in theY translation only. There will be negligible reaction on that constraint, and therefore negligible singularity (recall that stress = F / A and even thought the A is zero for a point constraint, the F is negligible for that reaction, so the stress contribution from the singularity is negligible)

Hope that helps.

Ray.

 

[esundman]

Orion,

In cases like these I have had luck with attaching very weak springs to the model in the x and z directions. Even something like 1lb/in will be enough to satisfy Mechanica. Mathematically, it can't have a zero constraint along an axis (even if you're not applying force in that direction) because it results in a stiff matrix (which can be impossible to solve).

Eric Sundman