COSMOS Analysis of Rocker Arm

[B Kope]

I am doing an FEA of our rocker arm in COSMOS. So far I have set the following constraints and loads:

- A hinge restraint on the pivot point, allowing for free rotation

- A cylindrical restraint on the shock connection surface, restraining circumferential and axial to 0, but no radial restraint

- A bearing load on the pullrod connection surface acting in a plane parallel to the pullrod.

Can anyone tell me if I have the right idea? The numbers are coming out reasonable, but this is the first time I am using FEA, and have no formal training. The bearing load I set is equal to the maximum pullrod force we expect. Will these restraints and loads create the assumption that the suspension is fully compressed and the rocker arm is at its highest stress?

I'm pretty sure that the hinge restraint is appropriate, but any feedback on the method I used for creating the pullrod and shock forces would be greatly appreciated.

Thanks

[Jersey Tom]

Account for a couple degrees of misalignment in that pushrod. Can change FOS by a lot.

[Ashley Denmead]

dont forget to account for the load and geometry when the spring bottoms out and everything becomes solid!

[Maurini]

dont forget to account for the load and geometry when the spring bottoms out and everything becomes solid!


If your spring bottoms out your problems are just beginning.

1) You are correct in that it is very hard on the damper/spring/pushrod combination.
2) It sends impact loading through the suspension (and driver) that is hard to calculate.
3) and MOST IMPORTANT-If you bottom out the springs, that end of the car instantly becomes infinitely stiff. This will result in sudden loss of grip making the driver more or less a passenger.

Regards,

Marc

[Gareth]

I'm not a Cosmos user and I'm an FEA snob...so I hope this is useful. :-)

I've run OptiStruct topology analyses on bellcrank/rockers, which should probably have a similar setup to your Cosmos Analysis. At the pivot I used a 1-6 constraint to hold a CBAR element that represented the rigid part of the pivot. This probably could have been rigid, but it's a bit of a hack to let me use RBE3's to represent the bearings' connection to the bellcrank. This is a little 'softer' than just using a rigid spider and doesn't have the problems with multiple dependant nodes. It also let me release the local x rotations (4 pin flag) on the CBAR, creating something like your hinge joint.

I used a similar setup at each of the bolt locations. I connected the pushrod point with another bar element to the outer pushrod point where I constrained 1-6. This CBAR had nearly all rotations released (456 on one end and 56 on the other - you need to keep a 4 rotation locked to avoid rigid body motions). At the damper and A/R points and fed in my predicted loads. For the optimization I just used typical service loads to look at the compliance of the part. For the damper point I used worse case damper force plus highest deflection spring force (damper forces are significant!). For the A/R point I just used the force corresponding to full roll at 1.5 G's or there abouts. I looked at the maximum mis-alignment that these forces could achieve from the kinematics of the system and setup those up as my separate sub-cases.

Admittedly after that I coulda-shoulda done a ultimate loading case that could be contrived from a bottoming-out scenario. These loads would be difficult to derive so I ignored it. :-) As Maurini put it, if your spring bottoms out your problems are just beginning! Our chassis would bottom before our suspension bottomed...and the plan was to have bump rubbers...

If anyone has questions about OptiStruct I can probably help.

[billywight]

Gareth - did you use any gap elements around the bolt holes? It can be suprising what a difference they can make in an optimization run. Also have you tried the new stress design variable in Optistruct 8?

Cosmos is quite different from Altair's software, it's a lot more user friendly, although you don't have nearly the same control over the mesh or other parameters and there is no Topology optimization available.

[Gareth]

Billy,

No I did not bother with gap elements, though that may have been interesting. I just use RBE3's to allow the bearing bores to move around a little. If I was looking to do a detailed analysis on the bore itself I would probably take the time to use gap elements. All results surrounding an MPC constaint are garbage so you've gotta use some 'engineering judgement' to design your parts in those areas.

I've seen a case study on the difference between linear and non-linear gap elements and apparently there can be a significant improvement in predicted stress distributions. I personally like the 'hard contact' that ABAQUS uses as it takes out the guess-work of generating a good approximation of 'penalty stiffness'. Nevertheless, it's better to have some kind of contact method that can be used within optimization. Did you let OS auto-generate your K values?

Stress responses were available in OS 7, but not for topology design space. In 8.0 they've added a 'soft' stress constraint within the DTPL card (topology optimization definition). It's apparently not trivial to do and is an approximation. It allows 'small' violations around stress concentrations so that the optimized shape isn't driven by localized areas. A perfect example is around fastener constaints where the stresses can be artificially high. Or at the interface between design and non-design space.

Anyway, I've 'TOYed' around with 'mickey-mouse' solvers like Cosmos a little, but I'm generally not impressed. :-) I don't put a lot of faith in an auto-generated 1st order tet-mesh. I'll use 1st order tet's for quick iterations in an optimization, but a tet10 or hexa-mesh validation is necessary.

I've also found that a shape optimization is a integral step in squeezing most out of the material. Topology gives you the rough layout of the part, but to size the members you need to use morphing and a shape optimization.

Btw, you should check out the hexa meshing in HM 8.0. It has some semi-automated hexa-meshing, which I think is unique.