FEA in SolidWorks For The Cassis

[thatoneguy]

Hey! I'm running FEA in SolidWorks and as I am going through the list of tests that need to be ran, I'm having an issue determining what joints should be fixed for different tests. The biggest concern I have is for the Front Bulkhead and Bulkhead Supports off axis. It says to have a max deflection of only 25 mm, but there is no way I can get anything close to that. I can't get below 100 mm with 120 kN head on and 10.5 kN sideways. The only joints I have fixed are the engine and suspension mounts on the back. I was reading the rules and noticed the Boundary condition section, can anyone help to decipher this or let me know where you have fixed different joints for theses tests?

Thanks,

thatoneguy

[Claude Rouelle]

And you are?

Wouldn't it be decent and courteous for you to introduce yourself... unless you want to just remain "that one guy"?

[thatoneguy]

Hello Claude,

My name is Cody. I am a student at the Oregon Institute of Technology. I am in charge of developing the chassis for next year's car. My apologies for the short comings in my post, I am unfamiliar with the norms of this community. I haven't lurked long enough and was forced to pose this question before I was able to adequately familiarize myself with such norms.

Again my apologies, you are absolutely correct.

Cody W.

[Adam Farabaugh]

If you are trying to do this to satisfy the AFR/SRCF, give up. For that they (rightly) require a NASTRAN deck for review, and whatever the hell SolidWorks is using to do calculations, it's not NASTRAN.

The minimum-weight standard frame will not come close to passing the AFR. You are right to find large deflections in the off-axis front impact load case, although 100mm means you have a serious lack of triangulation in top-down views.

The AFR rules are pretty clear on BCs: fix translation but not rotation of the bases of roll hoops for nearly every load case, and the shoulder harness attachment points for a few load cases.

[Luniz]

Please, if you are trying to produce an accurate FE Analysis of anything, do not use SW but rather something with a decent preprocessor (Ansys, Hyperworks, whatever) where you actually have some influence on meshing, element type, constraints etc. SW can be useful for comparing different versions of some part, but can imho not be used to obtain any quantitative result because of these shortcomings.

And when you start doing a decent analysis with a decent tool, you will have to familiarize yourself with finite element theory so that you actually know what you are doing.

If you haven't got a proper tool available at your uni, you can ask Altair Engineering for sponsorship (I happen to work at their German office...) and they will probably be happy to sort you out. For a starter, you can download an eBook that explains the basics of FEA and has been produced by our academic team. As it focuses on the theoretical background, it is largely product independent, so it applies to all FEA solutions on the market. You can find it here: http://www.altairuniversity.com/free...a-study-guide/

Regards, Luniz

[thatoneguy]

It's not that I don't improper triangulation, it all moves together. It comes down to the Force multiplied by the lever arm. The longer, the more it will deflect (you know what I'm talking about.)lame.jpg

Thank you,

Cody

[TiJei]

Hi Cody,

doing a FEA according to AF-Rules with Solid Works could be challenging because of documentation requirements.
Regardeless of that I agree with Adam that it is useless to try to use AF-Rules. The resulting design will be allways heavier than a conventional design. It might be a different storry if alternative boundary conditions according AF5.6 are used. I haven't tried this yet, how ever I judge it unlikely as AF-Rules consider lateral load cases where the conventional rule set does not.

Regarding the improper triangulations: Yes you suffer from it - in top view. However top view is not rule relevant (for reasons I don't understand) so your design could be rule compliant for the conventional rule set. For sure it suffers from a massive lack of bending stiffness around vertical axis. This is also what can be seen from your picture.

Short summary up to now: Your frame FEA so far does not support your efforts in finding a good frame design in any way. Lets talk about what could probably help.

I would define following requirements to a good frame design:

1. Rule compliance
2. low weight
3. sufficient stiffness according to the assumptions made during the suspension design of your car

FEA helps in achieving targets according point 3 while minimizing mass. In absence of targets for stiffness you could also define a mass target and maximize the frame stiffness.
There are two different types of analysis you could perform:

1. Modal analysis of your frame inclding the major unsprung masses
- Stiffness at a given mass distribution results in a certain resonance frequency --> The higher the frequency the higher the stiffness
- masses and inertias of components can be estimated - results have comparative character therefore estimations should be kept consistend
- the mode shape will also allow you to see weak sections in your design - target would be a smoth displacement distribution along the longitudinal axis
- This analysis can be done free-free which avoids mistakes because of boundary conditions. It will not give a stiffness results according to point 3 of the requirements.


2. Static analysis of the wheel to wheel stiffness of your frame design
- The model consits from your frame and stiffening structures like the engine - no mass is required
- Loads could be aplied via displacements, forces are results --> stiffness is calculated.
- This analysis needs loads as applied kinematically correct. In my expirience the easiest way is to include a kinematic model of the suspension and aply loads and restraints at tire contact patches

Side effect of the 2. analysis: If detailed enough you can get results for hidden compliance in support points for a-arms or rockers. However don't get to picky while setting up the model and be careful during result interpretation.

The analysis described can be done with any FEA package I am aware of, including CATIA's in house solution. Therefore I do not see necessity to switch to a dedicated FE-Package. (Sorry Lutz, however Hypermesh would be my favourite preprocessor :-) ) Just use whatever you are most comfortable with.


That's it for the moment. I hope I have given some inputs to improve your design.

Timo

[Karam El Hady]

Hi cody

the rules is obvious in this section
the boundary conditions "Fixed displacement but not rotation of the bottom nodes of both sides of the main roll hoop and both locations where the main hoop and shoulder harness tube connect. "
note that if you work with solidworks the force you selected in the structural analysis (per item) it's not permitted to select a total force
that's mean every member or node you select added a force with a value of 120 KN so you must divide the force by the number of members or nodes to get the total force applied in the selected members or nodes
in case of unequal length members you can also get the total force on the members by using the tool (per length) found in the property manager in the tree of simulation and divide the total force applying on the members by the total length of these members

best wishes

---

karam
Mansoura formula student