FEA of uprights

[Bharadwaz]

I have a doubt regarding the FEA of uprights and hubs. I have gone through other threads related to this topic and managed to piece together a set of constraints and loadcases. This is my first shot at designing(and being part of an FSAE team), so I am looking for validation of my concept. Attached below is a screenshot of my design.(front upright)

145

Here,considering X,Y and Z axis to be the usual longitudinal,lateral and vertical axes,this is basically what I've done:
1)Constrained the upper knuckle ball joint in X,Y.
2)Constrained my lower Ball joint in X,Y,Z. (we are using a pushrod setup).Basically I constrained the bolt faces at these joints.(or do I need to insert bolts and then constrain them?)
3)Calculated the tension/compression forces in the upper and lower control arms due to forces acting at contact patch. Applied these as loads at the respective ball joints. (taking braking+cornering as the worst case scenario)
4)Applied a 3g bump force as a remote load acting on the bearing through contact patch.

Are these the proper constraints and loadcases? I also wanted to know if the braking and cornering loads are applied as ramp functions(which I dont think is right) in workbench or if there is any other way it is done. Please do correct me if I am wrong.

Thanks in advance.

[Jay Lawrence]

I've never done any detail suspension design, so take this with a grain of salt (I'm sure someone more equipped will be along soon) but I would constrain the upper and lower bolt faces (wouldn't worry about doing a bolted connection interface) and apply loads in X, Y and Z directions (lateral accel, longitudinal accel, bump) plus the respective moment loads (from cornering, braking, tyre centre offset) all acting at the centre of the hub. You can't constrain the upper/lower joints and then also apply a load there

[Bharadwaz]

Yeah I'd noticed that just now. Sorry for that error. I meant to apply load only in the upper wishbone.

[mech5496]

Jay's method is what we do. You can also try clamping the bearing surfaces and apply calculated loads to ball joints, but it is easier to make a mistake.

[Kevin Hayward]

Excuse some of the terminology that follows. I will use constraint terms as per Solidworks Simulation. For parts like a machined upright I prefer to use FEA as built into the CAD software. It is more than capable of doing this sort of analysis well when setup properly, and I find iterations much faster. I tend to use ANSYS when looking at problems that Solidworks Simulation doesn't work well with such as surface and mixed mesh problems, or non-linear FEA. This hasn't been that often in the last few years. Ansys will have equivalent constraints and ways to apply loads. I also assume that you are looking at linear FEA, and that the upright is designed to have much lower than yield stress in operation to ensure decent fatigue life.

Remote loads and elastic constraints can all be very useful when analysing something like an upright. Remote loads will help you to avoid a lot of calculations when applied correctly. Also think about putting in some dummy parts to represent bolts, hubs, bearings, brake calipers. Apply the loads and constraints on them. It will increase computation time (probably from 30s to about 5 minutes or so) but the stresses are generally much more accurate.

Also note what each of the constraints mean mathematically when you apply them, usually the largest problems in FEA occur around these constraints. For example if you constrain the surfaces where the bolts for the upper and lower balljoints using a fixed connection you will allow the application of a direct tensile load (i.e. simulating the bolt welded to the tabs). This will cause inaccurate stresses around that area. The effect of this error may or may not be reduced as you move away from the constraint. Given the speed of the average PC these days I don't think it is wise to apply a fixed constraint at these points.

Try doing some very simple bracket FEA to have a look at the difference between a fixed constraint, a bolted connection, and maybe a two part model with a cylinder modeled to replace the bolt with no penetration allowed. Look at the results and assess how accurately each one represents real life. Then maybe model some simple structures that might represent the rough overall shape of an upright. Look at the effect of stress concentrations, section depth and so on. Maybe look at the effect of bearing loads on simple revolved shapes. The upright as you have drawn it is made up of a simple rough shape with cutouts (and concentrations), a few brackets for ball joints and brakes, and a revolved shape for the bearings.

By understanding the analysis of these simple sub shapes, you will be better placed to understand the analysis of the final upright. You will also likely end up with a better design. For example you have double shear at the lower balljoint, but how much of the load is taken by the lower bolting faces of that connection? Depending on the design of this detail you might have something that behaves much more like a single shear connection.

Good FEA work takes time and understanding. The results are quick to generate, but it is way too easy to do it wrong. If you are inexperienced with this sort of analysis do not start with the whole upright. Unless you have a good understanding of what to expect you will not be aware of the mistakes. It is not the passage of time that builds this understanding. Instead it is deliberate study of simpler sub-problems combined with research and practice. (I wonder if this is the place I should mention the dirty 'V' word - validation.)

When doing the analysis make sure you look at principal stresses, when it comes to fatigue analysis it is important to know what is in tension and what is in compression. You should definitely be considering fatigue. Also look at the deflection. Making sure it doesn't break is not even the main task of the upright. In practice once you have designed it stiff enough, and simple enough for ease of manufacture, it will usually be strong enough.

Don't just look at braking and cornering as the worst case. How much braking? How much cornering? It is easy enough to setup a number of load conditions. A lower load from a different direction may cause worse stresses. Similarly the upright's stiffness will be dependent on the direction of the applied load.

When you have done the analysis and are ready for manufacture make sure you build an extra upright. Test it to destruction. Find out where and how it breaks. See what the stiffness is. Try and test it as close to how it is simulated. Even just one test of this nature will be of great value to your team.

Kev

[Claude Rouelle]

Bharadwaz,

Why 3 G?

[Jay Lawrence]

^ What Kev said ;)

[Bharadwaz]

mech5496,let me know if I got this right. I constrain the upper and lower ball joints,apply the loads due to sprung mass(lateral,longitudinal,bump) on bearing surface,and also apply moments created here by unsprung components of that wheel due to vertical loads at contact patch on braking and cornering.Any mistake??

Thanks a lot for the inputs Kevin.We did in fact plan on getting an extra upright machined solely for tearing it apart :D. I did feel that asking about bolted connections was unnecessary as I could have tested that out by myself. Still,thanks for sharing your insight on this.

I just have one more doubt. Now when I do FEA for the hubs(we are running a setup similar to semi-floating axles) I am constraining one end of the hub(the end in the upright) and applying a load on the other end,like a cantilever.My reasoning for this is that during the upright analysis,as I am constraining the wishbones,the hub in that condition will be subjected to the moments due to vertical forces at the contact patch.Also,the rotor attached to the hub exerts a torque when brakes are applied. I hope I am right till this point. The thing I dont understand is how to apply a proper constraint to account for reacting driving torque from the shaft.Is is just a simple torque at the centre of the hub?

[Steve Krug]

Hello Bharadwaz,

Remote load transfer especially with many load configurations may be a wise route to start doing finite element studies. Remember where all of the loads are coming from, where they are being applied to on the component, and where they are being reacted on the component. Maybe the place where the loads come from change and can be higher or lower overall loads in the 3 dimension component system. This is a question worth asking, as the tire is flexible and experiences loads from different places on itself. What are the directions of the loads in all 3 directions under acceleration? Braking? Cornering? Combined?
Data acquisition can reveal (maybe a G-G diagram) where your loads are coming from and how often your loads are coming from these places. How is the tire deflecting and contact patch changing location during the events represented in the G-G diagram?

Many load cases is probably a good idea with some of these ideas taken into account. But remember, the car must hit the ground at some point.

[8Bit]

Excuse some of the terminology that follows. I will use constraint terms as per Solidworks Simulation. For parts like a machined upright I prefer to use FEA as built into the CAD software. It is more than capable of doing this sort of analysis well when setup properly, and I find iterations much faster. I tend to use ANSYS when looking at problems that Solidworks Simulation doesn't work well with such as surface and mixed mesh problems, or non-linear FEA. This hasn't been that often in the last few years. Ansys will have equivalent constraints and ways to apply loads. I also assume that you are looking at linear FEA, and that the upright is designed to have much lower than yield stress in operation to ensure decent fatigue life.

Remote loads and elastic constraints can all be very useful when analysing something like an upright. Remote loads will help you to avoid a lot of calculations when applied correctly. Also think about putting in some dummy parts to represent bolts, hubs, bearings, brake calipers. Apply the loads and constraints on them. It will increase computation time (probably from 30s to about 5 minutes or so) but the stresses are generally much more accurate.

Also note what each of the constraints mean mathematically when you apply them, usually the largest problems in FEA occur around these constraints. For example if you constrain the surfaces where the bolts for the upper and lower balljoints using a fixed connection you will allow the application of a direct tensile load (i.e. simulating the bolt welded to the tabs). This will cause inaccurate stresses around that area. The effect of this error may or may not be reduced as you move away from the constraint. Given the speed of the average PC these days I don't think it is wise to apply a fixed constraint at these points.

Try doing some very simple bracket FEA to have a look at the difference between a fixed constraint, a bolted connection, and maybe a two part model with a cylinder modeled to replace the bolt with no penetration allowed. Look at the results and assess how accurately each one represents real life. Then maybe model some simple structures that might represent the rough overall shape of an upright. Look at the effect of stress concentrations, section depth and so on. Maybe look at the effect of bearing loads on simple revolved shapes. The upright as you have drawn it is made up of a simple rough shape with cutouts (and concentrations), a few brackets for ball joints and brakes, and a revolved shape for the bearings.

By understanding the analysis of these simple sub shapes, you will be better placed to understand the analysis of the final upright. You will also likely end up with a better design. For example you have double shear at the lower balljoint, but how much of the load is taken by the lower bolting faces of that connection? Depending on the design of this detail you might have something that behaves much more like a single shear connection.

Good FEA work takes time and understanding. The results are quick to generate, but it is way too easy to do it wrong. If you are inexperienced with this sort of analysis do not start with the whole upright. Unless you have a good understanding of what to expect you will not be aware of the mistakes. It is not the passage of time that builds this understanding. Instead it is deliberate study of simpler sub-problems combined with research and practice. (I wonder if this is the place I should mention the dirty 'V' word - validation.)

When doing the analysis make sure you look at principal stresses, when it comes to fatigue analysis it is important to know what is in tension and what is in compression. You should definitely be considering fatigue. Also look at the deflection. Making sure it doesn't break is not even the main task of the upright. In practice once you have designed it stiff enough, and simple enough for ease of manufacture, it will usually be strong enough.

Don't just look at braking and cornering as the worst case. How much braking? How much cornering? It is easy enough to setup a number of load conditions. A lower load from a different direction may cause worse stresses. Similarly the upright's stiffness will be dependent on the direction of the applied load.

When you have done the analysis and are ready for manufacture make sure you build an extra upright. Test it to destruction. Find out where and how it breaks. See what the stiffness is. Try and test it as close to how it is simulated. Even just one test of this nature will be of great value to your team.

Kev
A few questions for you Kevin.

1) What are your thoughts on Brick Mesh versus Tet mesh as far as accuracy and mesh sensitivity are concerned for something that is potentially as geometrically complex as an upright? (This may be related to the simple sub-shapes)

2) In the "If it's simple and stiff, it's strong" paragraph, I've often wondered what other teams use for criteria in terms of stiffness or compliance as well as number of cycles to failure. Could you give some insight on this? I often find myself using 100K cycles, but I realize 1M cycles is more typical of an "infinite" life case.

3) Yes, the dirty 'V' word. I can't stress enough how valuable this is. I am of the opinion that engineering is full circle, in that you analyze the problem, design a solution, and then validate that solution. Many teams never quite get to the last portion of the part and I often wonder why. This is the most valuable stage to me, in that you can truly gather data with which to refine the design over time or potentially discover (and fix) an issue which had not been caught in the beginning before flat-out failure in a competition.

[Kevin Hayward]

8Bit,

Sorry for the late reply. I have been on a nice long holiday :)

Responses to your points:

1) For the purpose of iteration speed I try to avoid adding any time to the meshing process. This tends to mean automatic meshing with few controls using Tets. It ends up being a little more CPU intensive, but in real life you make up more time by the lack of fiddling with the meshing than you do with slower computation. For reference I wouldn't consider an upright very complex.

2) When it comes to stiffness you need to think in the way of degrees per g (toe, camber, caster), and compare it to your kinematic objectives. Unfortunately this is where you should consider all the suspension. There is no point having your upright contribute only 0.00001 deg/g when your bearing arrangement might produce 1deg/g. One of the best things you can do is measure it on car, and try to determine where the deflection is coming from. While a high end K&C rig is fantastic you only need a few straps and dial gauges to do a pretty decent job. Number of fatigue cycles is also a tough one. Some of the cars I have been involved with see a competition, a little testing and not much else. Others have been pounded for years beyond expected. I would look primarily at 1M cycles. Most of the uprights on the cars I have been involved with have been steel. This lets you get close to the idea of "infinite" life. However don't assume infinite life with an aluminium upright.

I will note that none of the programs I have been involved with have ever been sorted enough to do NDT of components that have been on a FSAE vehicle for a very long time. If you are in a similar situation where inspection might be cursory visual at best then it is well worth being incredibly conservative with fatigue. The bonus is that it very rarely adds much weight to a structure when done right.

3) Validation in all things. Testing the car prior to comp is validation of your full vehicle. Your results at comp provide validation of your team. I think the main issue with lack of part validation (or system validation) is that it takes a reasonable amount of resources. These do not tend to get allocated. When a team has $40k sitting there they tend to use it for parts, materials and comp expenses. For teams to get a start I suggest picking a few of the key components and make test samples of those. Maybe an upright one year, a wheel centre the next. Maybe allocate a couple of grand a year to test parts, and make sure you budget it up front.

Kev