Cosmos upright contraints?

[Nihal]

I have been trying to to FEA my upright design in Cosmos (I tried using Algor but had many issues with the program not wanting to cooperate with my computer). I don't have much experiance with Cosmos and was trying to set up the contraints and bolted connections. I have been trying to apply constraints to SW smart fastners that would go through the ball joints. I then bonded these bolts to the bolt holes. I then put a bolted connection in Cosmos between the steering arm and the upright (I am using shim type camber adjustment for the upright) and bonded the two faces (upright to steering arm).

I am not sure how to constrain the specific bolts in certain directions. I am trying to restrain the pushrod in Z, LBJ in X and Y etc. I applied a remote force to the bearing face from the contact patch,

After all this I get some incorrect results. I think these results are because of my constraints being incorrect. I have been trying to set the contraints in the directions by using the refrence plane and leaving the direction magnitudes at 0. Is there a better way to apply the constraints without having to use the smart fastners?

I get some warnings that I don't understand when I run the analysis.

1. Ratio of clearnce/element size in at least one element is larger than 1.

2. Contact pair is not defined for bolt connectors. (I really don't understand this one. The two faces that are bolted together have a bonded contact defanition).

So does anyone who has used COSMOS to FEA an upright have tips on how to properly use the contraints and model the connections properly?
Thanks

[Jersey Tom]

Couple things, from having designed our uprights this year and done considerable FEA in Cosmos05

1) Take all the bolt solid models out of your assembly. Don't need em. Only things you need are your main pieces. No bolts, no bearings..

2) Make sure your global contact condition is set to "Free" rather than the default "Bonded". By default any two faces that are touching each other are thought to be bonded together.. which they aren't. Theyre free to move.

3) Any place where there's a bolt connecting two cylindrical faces, use a rigid connecter. Don't use the "bolt" fastener thing.

4) Applying the remote load through contact patch = good

5) For your balljoints, constrain them using reference geometry. For example, your LBJ constrained in X and Y should have a "0" displacement value in those directions, and should be unconstrained in Z. If you have arms coming in at odd angles (such as a tie rod), you'll have to use a reference co-ordinate system.

6) Run the finest mesh you can. Running the 'standard' mesh size gave me results of a FOS of .44, while a fine mesh gave 5.1 (on my initial design). Typically somewhere on the order of 220,000 DOF worked well for me.

7) Make sure you're defining the right material properties, and that the mechanical properties in Cosmosworks match with the material youre using, in whatever heat treatment.

[Frank]

i have to disagree a bit

dont use faces "free" (it is a contact stress analysis) unless you have to
there is no need unless you are worried about the stress at where the load is imparted on the object, remember that stress will normalise away from the point of impact

if you are worried about stress at where the load imparts on the object,
use a smaller (locallised) model

best of all; anylise single components instead of assemblies.

use statics to determine the loads at the upright. perhaps a simple fea program to calculate these loads if your not confident with the math (ie a program that uses simple beams and nodes)

for a quick calc, consider the moment from cornering to be 350 - 450 Nm "static" load at max g's (for 13" tyres)
and the moment from steering load 50-100Nm

resolve these moments into forces at the 3 upright bearings (2*a-arm, 1*steering), and reactions at the wheel bearings

it is better to make the analysis a structure instead of a mechinism (don't use "inertial relief")

dont create "artificial stiffness" ie use only one contraint, the other inputs are loads

use the default mesh size, or slightly finer
explore the options for meshing (constant size,variable size)
there is also the ability to make smaller mesh on chosen faces

im not completely sure, but i think the newer versions of Cosmos allow a "Hertzian Contact Stress Distribution" to be applied to a surface of a part

[Omer]

hi all
I agree with Frank and think analysin one solid body is better than solving the assembly,especialy if the upright is what you are really testing.
remember that those fine elements programs are gigo (garbage in garbage out) you can get easily lost with wrong results if your analayse is not correct.

do the analyse at least twice,first with the default meshing and then with a finer mesh and make sure your solution gives you the same or close results,a sign your solution is good.

fillet radius has a big influence on the results.

pls look at my upright http://w3.bgu.ac.il/sae%2Dcar/upright_f_l_new.jpg
I used the cylindrical hole for the lbj and ubj as constraints but i'm not sure on what faces to put the forces?help any one?

[Jersey Tom]

My uprights are not a single piece unit. So it has to be analyzed as an assembly and I'm quite confident in the results.