Upright FEA restraints

[Alex Vincent]

Hello, I am trying to model our upright forces, but I am having trouble figuring out what to do for constraints. Right now I have a remote load at the bearings with the A-arm attachments constrained in the lateral and longitudinal directions. I'm not sure what to do with the pushrods however, since they need to be able to deflect, and constraining puts an artificial constraint in the lateral direction.

Any help on a direction to go with these would be greatly appreciated.

[Alex Vincent]

Hello, I am trying to model our upright forces, but I am having trouble figuring out what to do for constraints. Right now I have a remote load at the bearings with the A-arm attachments constrained in the lateral and longitudinal directions. I'm not sure what to do with the pushrods however, since they need to be able to deflect, and constraining puts an artificial constraint in the lateral direction.

Any help on a direction to go with these would be greatly appreciated.

[The AFX Master]

You need to restrain only six degrees of freedom since your structure is designed to move under the deformation of one of the elements (the spring)

If your push rod is attached to a wishbone, then the ball joint pick up point of that wishbone in the upright needs to be restrained 3 translational DOF's

Your remaining DOF's are two restraints at the ball joint of "non pushrod" wishbone, also in plane with said wishbone, and another restraint aligned with your toe link.

All sum 6 DOF's

EDIT: What software are you sing to perform FEA?

[Alex Vincent]

I'm using Solidworks Simulator for FEA, and my pushrods are connected to the upright itself via a mount.

[Crispy]

I think using a translation constraint along the axis of the pushrod, at the pushrod connection would give you the desired result. I'm not sure how you accomplish this in Solidworks (I've never used their FEA, in catia it would be a user defined constraint using a local axis system).

If you can't specifically remove that dof, then maybe you can add a pushrod to the analysis (1-d beam, or something similar). Use a ball joint at the upright end and remove all translations at the other (you may also have to remove the rotation DOF along the pushrod axis).

As for the A-arm connections, I agree with "The AFX Master".

I hope this helps.

[RyMan]

First off, make sure you are using the advanced fixtures. The next part can be a little tricky without being able to see your model, but I will try and help to the best of my understanding.

Are your a-arm attachments a single bolt or are they brackets or are they something else? Specifically how are you mounting the pushrod on the upright?

When you say you have the a-arm atachments constrained in the lateral and longitudinal directions, what axis is this with respect to? Is it an overhead view, a side view, etc.?

[R. Alexander]

Non penetration contact conditions in Solidworks simulation apparently take an incredible amount of time to solve.

Don`t you need them if you`re going to have the a-arms and pull rods attached etc?

[TorqueWrench]

If you are going to model the suspension with all the links in place and the ball joints themselves constrained to "tabs" on the frame, then you will have to use a non-penetration contact. They do take a while to solve, but it will give you much more accurate results. Remember that you also have to define all of your bolts in Simulation to get correct results for multi-body analysis.

For a suspension assembly, I can't see it taking much more than 3-4 hours to run and, to me at least, that is well worth the increased accuracy of your analysis.

[The AFX Master]

In simulation, you'll need to do a remote displacement.. here's how

First you need to insert coordinate systems (insert> reference geometry> Coordinate systems) on each spherical joint (point) that you have in your upright. Commonly 3, as lower pivot, upper pivot and track rod (toe link). Notice that you'll need to make one of the planes of the coordinate system coincident with your wishbone's plane, Regarding the toe link, align whichever axis of the coordinate system with the toe link.. as follows.

http://i281.photobucket.com/albums/kk229/theafxmaster/upright.png

Then apply remote displacements set to ZERO on the convenient axes at each ball joint (depending on what DOF's are restricted by that wishbone, they're three on the pushrod wishbone, two on the free wishbone, and obviously one at toe link).


Put your loads as bearing loads on bearing surfaces, and you're done. Perform your FEA with the usual convergence and hand calculations to check a logic result. VERIFY that the upright ROTATES (a bending deformation) around the balljoints, is a common misconception that cornering loads do not bend the uprights in planes other than the rim flange plane..

Another bit to keep in mind, in the image, and for illustrative sake, i've applied the restraints on the holes where the bracket bolts are attached.. It's better to assemble the brackets, put the appropriate pin connectors, surface to surface contact sets and THEN put the restrains on the bracket surfaces that are supposed to serve as bearing surfaces for suspension bolts.

[Alex Vincent]

Here is a picture of the rear uprights. For the a-arms, I have been constraining them along the ground plane to get just vertical movement.

http://img.photobucket.com/albums/v611/VinniCanadian06/Uprights.jpg

http://img.photobucket.com/albums/v611/VinniCanadian06/pushrod.jpg

[Chris Allbee]

While including the a-arms and springs and everything is cool and such, for a static analysis they are unneeded.

[Dash]

<BLOCKQUOTE class="ip-ubbcode-quote"><div class="ip-ubbcode-quote-title">quote:</div><div class="ip-ubbcode-quote-content">Originally posted by TorqueWrench:
then you will have to use a non-penetration contact. They do take a while to solve, but it will give you much more accurate results. </div></BLOCKQUOTE>

I have been trying to run simulation similar to this one in Solidworks Simulation, and on the bellcranks that I have designed. EVERY time I click the "run" button, STAR crashes. If by a miracle it doesn't, then it takes like an hour to try and do the simulation then it fails. Same thing happens when i try to use the hinge fixture. Any ideas what my problem could be? Just need a better computer?

EDIT: Another thing to add that might help diagnose my problem. When I try to use the hinge it says that I have excessive displacement that is "Too large to be real", but if i fix the hinged joint, it will run just fine. I have a high factor of safety when it runs that way, so I'm pretty sure the part isn't "breaking".

[billywight]

<BLOCKQUOTE class="ip-ubbcode-quote"><div class="ip-ubbcode-quote-title">quote:</div><div class="ip-ubbcode-quote-content">When I try to use the hinge it says that I have excessive displacement that is "Too large to be real", but if i fix the hinged joint, it will run just fine. I have a high factor of safety when it runs that way, so I'm pretty sure the part isn't "breaking". </div></BLOCKQUOTE>

Forget the fluffy SolidWorks constraints and use the "advanced" constraints with local coordinate systems as necessary. This way you can see what you are really doing. The error you get is due to your model being undercontrained. When the simulation runs it is being pushed off into space somewhere by the applied forces. An easy way to see what is underconstrained is to run a modial analysis of the same model and look at the results.

[Chapo]

@Chris Allbee

I beg to differ, while including the spring is unnecessary, the different stiffnesses of the wishbones can significantly alter the outcome of the analysis. Initial, ball park, analysis can be done as individual components, but you need to model everything to account for deflections as the force will go through the stiffest load path. It does chew up a lot of time, but its the only way to get a reasonably accurate result.

my 2c

[billywight]

<BLOCKQUOTE class="ip-ubbcode-quote"><div class="ip-ubbcode-quote-title">quote:</div><div class="ip-ubbcode-quote-content">I beg to differ, while including the spring is unnecessary, the different stiffnesses of the wishbones can significantly alter the outcome of the analysis. Initial, ball park, analysis can be done as individual components, but you need to model everything to account for deflections as the force will go through the stiffest load path. It does chew up a lot of time, but its the only way to get a reasonably accurate result. </div></BLOCKQUOTE>

In a static analysis, the simulation is assumed to be in equilibrium and therefore the extra components are of no significance. If you're running a dynamic analysis, then they may be of importance, depending on the dynamic conditions and the stiffness of the restraining components. It is unlikely that you will be running a dynamic analysis on a suspension upright that will produce any substantial results that differ from that of a static analysis though, especially if the suspension linkages are sufficiently stiff (properly designed). Even so, where do you stop modeling components? Why wouldn't the chassis stiffness at the a-arm attachment points be of significance?

[Chapo]

Respectfully I disagree, I haven't done this analysis in the context of an upright, but while analysing our pedal box base, including the rails (its attachment points) dramatically changed the loading of the component, it wont have the same effect due to the use of spherical bearings, but I do believe that it is still important to take into consideration the effects of the whole assembly. my 2c

[Chapo]

Im going to take my foot out of my mouth now, the implications i was talking about were due to bending which wouldnt be applicable in this situation due to the spherical bearings. My apologies.

We live and we learn

[billywight]

<BLOCKQUOTE class="ip-ubbcode-quote"><div class="ip-ubbcode-quote-title">quote:</div><div class="ip-ubbcode-quote-content">Im going to take my foot out of my mouth now, the implications i was talking about were due to bending which wouldnt be applicable in this situation due to the spherical bearings. My apologies.

We live and we learn </div></BLOCKQUOTE>

No problem, after all, that's the goal of FSAE.

[Dash]

Thanks for the tips guys. After rebuilding the assembly from scratch and using your tips I was able to get the models running like champs. Although I don't think my laptop much appreciated all the computing it had to do. http://fsae.com/groupee_common/emoticons/icon_biggrin.gif