Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

ABAQUS Contact Analysis - Excessive Acceleration Results

ABAQUS Contact Analysis - Excessive Acceleration Results

ABAQUS Contact Analysis - Excessive Acceleration Results

Hello everyone,

I am currently working on a 3D FE (dynamic) explicit railroad model in ABAQUS, focusing on simulating wheel-rail interaction, especially at turnout crossings where there is a discontinuity of the rail (when the wheel transitions from 1 to 2 in the first attached screenshot). However, I am struggling with the acceleration results from the model which showed higher results compared to what I obtained from the field experiment (around 200 times higher).

Model overview:
I used the spring/dashpot feature to connect between the rail and rp (below the rail) to replicate the ballast and also connect the wheel and another rp (above the wheel) to replicate the truck/bogie suspension.
Based on the surface-to-surface contact interaction, I entered two steps; The 1st step was the stabilization which only applied the gravity to have contact between wheel and rail, and 2nd step was the wheel rolling on the rail using displacement B.C. (U1 and UR2 considering the radius of the wheel) and I applied the gradual amplitude.
The concentrated force was applied in both rp in the wheel center (wheel load) and rp above the wheel (bogie and truck load).

I used the SI unit of m(length), N(force), etc., and the magnitude of the contact force between the wheel and rail was similar to what I expected based on the load I applied. However, the acceleration of the node (near the impact occurs) showed around 10,000g (100,000 m/sec2) which is massive (and I don't think this can even happen). FYI, the impact happened at around 0.08 sec in the second screenshot.

I am wondering what might be the reason that induces this high acceleration which doesn't make sense.
Could anyone give me some guidance/comment on this issue I have?
Thank you in advance and have a great rest of your day :)

RE: ABAQUS Contact Analysis - Excessive Acceleration Results

Acceleration results in Abaqus/Explicit are prone to aliasing and it's important to select the output frequency properly. Antialiasing filters are also helpful in many cases. But you should check other results (especially energies - crucial in explicit) too. Take a closer look at what happens in the model (including the scaled deformed shape) when the impact occurs.

RE: ABAQUS Contact Analysis - Excessive Acceleration Results

@FEA way,
Thank you for your response!
Based on your comment, I checked the 'antialiasing' filter feature and the acceleration results actually showed really similar magnitude with that of the field measured data (but I am just curious why the Abaqus/Explicit is prone to aliasing).
Regarding the energy which I believe related with the reliability of the Explicit FE model, I only knew that the total energy (calculated based on various energies such as ALLIE, ALLVD, ALLFD, etc.) needs to be consistent during the analysis which was the case for my model, thankfully.
Are there some other parameters that I needs to consider with this regards?
Thanks again!

RE: ABAQUS Contact Analysis - Excessive Acceleration Results

Explicit dynamics analyses are susceptible to aliasing because they typically involve high-frequency, large-amplitude oscillations. According to the Nyquist Sampling Theorem, such signals with large oscillations at frequencies bigger than half the sampling rate might be distorted due to aliasing. So the sampling rate is crucial here and should be > 2*f_max to avoid aliasing but there are also built-in filters to reduce the noise (they can be even applied before running an analysis so that they act when Abaqus is solving a problem). Time integration of output results reduces the susceptibility to aliasing so it's usually the worst for acceleration and force output and less pronounced for velocity, strain, stress and (especially) displacement output.

All energies should be checked in Abaqus/Explicit results. Especially those related to numerical dissipation like ALLVD but also kinetic energy (ALLKE), artificial energy (ALLAE), internal energy (ALLIE), plastic dissipation energy (ALLPD), frictional dissipation energy (ALLFD) and so on. It depends on the case because some may not be relevant (e.g. if there's no plasticity or friction).

RE: ABAQUS Contact Analysis - Excessive Acceleration Results

10000 g is not a particularly high acceleration, for instance artillery shells experience 4000 g even without contact.

However, to get good correlation you'll need to use the same instrumentation setup (especially low pass frequency) as the physical test.

Your time history is (essentially) rubbish, you need to reduce your time step by at least a factor of 10, probably more. Try plotting displacement and velocity as well.

Your test data cannot have had an accelerometer at the contact point, on the wheel, are you comparing like with like?


Greg Locock

New here? Try reading these, they might help FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm?

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members! Already a Member? Login


Close Box

Join Eng-Tips® Today!

Join your peers on the Internet's largest technical engineering professional community.
It's easy to join and it's free.

Here's Why Members Love Eng-Tips Forums:

Register now while it's still free!

Already a member? Close this window and log in.

Join Us             Close