Simulation of impact on go-kart chasis

[Dudiek12]

TL;DR Summary

Hi, my issue is understanding of boundary conditions in simple front impact simulation of gokart chasis.

Hello, so recently I have been doing one preetty simple project in FEA, my task was to do a front impact analysis on go-kart chasis. While the simulation itself isn't hard at all and to be honest I had easy job thanks to various sources of tutorials around the web, I feel like I don't understand what I'm doing.

This concerns me because even though my simulations are ok, If I got other task I would fail miserably to do it. My biggest problem is to understand boundary conditions and to be more exact where and why to put a fixed support. Basically what all tutorials says is to put force on the rods that are directly hiting the obstacle and to put fixed support on the rods of chasis that are on the back.

I don't get why I should put fixed support on the back, for me It doesn't make sense since they can move freely and they are not immobilized in any sense. Can someone help me in understanding how to tackle this problem? I can't find a way to put here a image, to better ilustrate my problem

 

[FEAnalyst]

So you want to simulate this using static analysis and prescribing force representing impact ? I would definitely avoid this approach and perform a fully dynamic analysis (possibly using an explicit dynamics solver) in which the chassis has prescribed initial velocity and actually hits a rigid obstacle. Unless you don’t have access to sufficient software. With static simulation, the results will be very inaccurate as it’s not even possible to correctly determine the equivalent static force of impact.

 

[Lnewqban]

To assume pivoted supports on the rods more or less aligned with the vector force of the impact allows them to deform and buckle more easily, as those will be working as columns under compression load.
Please, see:
https://www.engineeringtoolbox.com/euler-column-formula-d_1813.html

To assume fixed supports on the rods of the chassis that are on the back is the worst possible condition regarding the deformation of the rods that are directly hitting the obstacle.
The energy of impact will not be transferred or dispersed further down the chassis regarding deformation of other members.

 

[Dudiek12]

So you want to simulate this using static analysis and prescribing force representing impact ? I would definitely avoid this approach and perform a fully dynamic analysis (possibly using an explicit dynamics solver) in which the chassis has prescribed initial velocity and actually hits a rigid obstacle. Unless you don’t have access to sufficient software. With static simulation, the results will be very inaccurate as it’s not even possible to correctly determine the equivalent static force of impact.

Yes, exactly I was trying to do static. I was thinking of doing dynamic, but I have only student version of Ansys and I remember I had some problems with other dynamic simulations in the past. I will check it. So just to put your words in other way, you also think that putting fixed support on the back is bad idea, right? I should either change it for more convenient option(still doing static) or change to dynamic if possible.

 

[Dudiek12]

To assume pivoted supports on the rods more or less aligned with the vector force of the impact allows them to deform and buckle more easily, as those will be working as columns under compression load.
Please, see:
https://www.engineeringtoolbox.com/euler-column-formula-d_1813.html

To assume fixed supports on the rods of the chassis that are on the back is the worst possible condition regarding the deformation of the rods that are directly hitting the obstacle.
The energy of impact will not be transferred or dispersed further down the chassis regarding deformation of other members.

Okay, but you think in general the idea to put fixed support on the back of the chasis is "realistic"? I don't see how this is a reflection of real life case. In reality there is nothing fixed on the back while hitting a wall for example. That was my main issue, I felt like those tutorials has some weird assumption.

 

[jack action]

To be more realistic, wouldn't it be better to fix the front end and apply an acceleration to the entire frame?

 

[Lnewqban]

Okay, but you think in general the idea to put fixed support on the back of the chasis is "realistic"? I don't see how this is a reflection of real life case. In reality there is nothing fixed on the back while hitting a wall for example. That was my main issue, I felt like those tutorials has some weird assumption.

When you are facing such a complicated distribution of impact forces and reactions in members, assumptions that deviate from pure reality are common.
In general, you assume structural members that could fail to be in the worst case scenario.
Fixed supports (higher resistance to buckling) are closer to a impact-energy-transferring rigid chassis, while pivoted supports (higher resistance to buckling) are closer to a impact energy-absorbing deformable front end.

 

[Dudiek12]

To be more realistic, wouldn't it be better to fix the front end and apply an acceleration to the entire frame?

Yes, that's what I was also thinking about. The only thing that bothers me in this scenario is the fact that if the front will be fixed, will it deform due to acceleration? I must experiment a little to understand how it's affecting the results.

 

[Dudiek12]

When you are facing such a complicated distribution of impact forces and reactions in members, assumptions that deviate from pure reality are common.
In general, you assume structural members that could fail to be in the worst case scenario.
Fixed supports (higher resistance to buckling) are closer to a impact-energy-transferring rigid chassis, while pivoted supports (higher resistance to buckling) are closer to a impact energy-absorbing deformable front end.

Okay, so you think that I shouldn't care much about the simulation to be realistic. It's more about checking all the weak points in my geometry? I'm not really experienced in doing such simulations, usually I do some cfd and I have litlle clue how to approach that.

 

[Lnewqban]

Okay, so you think that I shouldn't care much about the simulation to be realistic. It's more about checking all the weak points in my geometry? I'm not really experienced in doing such simulations, usually I do some cfd and I have litlle clue how to approach that.

You have more experience in simulations than I do.
I would verify exactly what the excessive expects from you.
To do a front impact analysis on go-kart chassis may simply mean how strong the front tubes receiving a direct impact should be, so the go-kart could continue on in a race.

If so, I would need to determine the mean velocity of impact that is expected and how solid/massive the object against the kart would collide with.
The instantaneous force of impact would depend on those factors, because the time of sudden deceleration is very influencial on its magnitude, as well as on how much inertia the rest of the kart and pilot pushing behind the impacting tube would have.

Once the load on the tube is roughly estimated, I would analyze the geometry of that tube and how much its attachement to the chassis would help it to resist the impact without suffering and transferring permanent deformations to the steering geometry of the kart.

I would then analize how to achieve the best results without adding excessive weight to the chassis.

 

[jack action]

The only thing that bothers me in this scenario is the fact that if the front will be fixed, will it deform due to acceleration?

Following are examples of an acceleration (gravity) working on a frame with a fixed end (the ground). I can see the deformation.

The only difference with your car frame is that you are in the horizontal plane instead of a vertical one. The ground is replaced by a fixed wall that will impose a deceleration on your frame (which should be much much more than gravity). You will then be able to see how much deceleration your frame can take before permanent deformation begins and where it will deform first.

Note that in a car crash the deceleration will increase until it reaches its maximum value, then decrease as energy is absorbed by the deformation of the frame. This will be different from gravity where it stays constant.

Real:

​

Simulation:

​

 

[FEAnalyst]

Okay, so you think that I shouldn't care much about the simulation to be realistic. It's more about checking all the weak points in my geometry? I'm not really experienced in doing such simulations, usually I do some cfd and I have litlle clue how to approach that.

Most likely, the difference between advised dynamic simulation and static analysis that you want to perform will be huge. Not only in terms of values (those may differ by orders of magnitude) but also failure locations and mechanisms. This is a highly dynamic and nonlinear problem and should be resolved using the proper analysis type. By the way, it would be interesting to compare both approaches and find out what the exact differences are in this particular case. A student version of Ansys is limited only in terms of the number of nodes/elements (128k for structural problems). With the use of beam elements (typical approach in the case of such frames), you should be able to stay below that limit.

 

[Dudiek12]

Okay, thank you for information. I will first run static analysis and then I will try to do dynamic one, hoping that I will manage to make a beam model of my case.