Contact US

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

Plastic product "crush" or "buckling" test with Solidworks Premium

Plastic product "crush" or "buckling" test with Solidworks Premium

Plastic product "crush" or "buckling" test with Solidworks Premium

Hello everyone,

Let's first talk about my background in FEA : everything I learned I got it through colleagues, browsing software help and googling a lot. So, no official training nor advanced mathematics class doing matrix calculation to understand the basic theory behind FEA. I got a diploma in mechanical engineering but no FEA training.

So, now you know who's posting, let's face the problem smile.

Here at my company we are manufacturing pails using plastic injection process. One of our quality control tests consists of snapping a lid on the pail which is then inserted into a "crushing" machine (Instron, tensile-test type machine). We basically put the pail (and its lid) between two thick metal plates and crush it to measure the maximum force it can withstand. The result of the test is the maximum value of the curve generated by the machine.

We are currently trying to reproduce that test using Solidworks Simulation Premium (which is the full simulation package with all analysis types unlocked). We used both Buckling Analysis and Non-Linear static analysis. We don't get success even with trying multiple parameter variations, geometry simplification, mesh variations. We tried both SW materials and our own material created with a stress-strain curve we got from our own labs.
  • Most people doing that kind of simulation, like our subcontractors, use Abaqus / Ansys+LS-Dyna. Why is no one using SW ? Are we using an inappropriate tool which is unable to do what we want to ?
  • From the description of the real-life test, what kind of analysis would be appropriate ? Buckling, non-linear static/dynamic ?
Thanks a lot everyone !

RE: Plastic product "crush" or "buckling" test with Solidworks Premium

I currently work for a SOLIDWORKS Simulation and Abaqus reseller. Here are my thoughts:

1. Your boundary constraints may not represent reality
2. Your mesh isn't sufficiently fine for your desired accuracy.
3. Though you developed your own material data, occassionally strain rate matters. Measuring material through a slow increase in load may yeild different data than a faster increase in load.
4. Depending on the physical test, there maybe damage that isn't being modeled correctly that redistributes loading.

If you would like to discuss this offline, PM me. We can exchange e-mails and possibly I can help you out.

RE: Plastic product "crush" or "buckling" test with Solidworks Premium

Thanks for your answer gravityandinertia.

About points 1 and 2 : we tried multiples variations of boundary constraints and both shell and solid elements. We went from coarse to fine-as-in-so-fine-the-computer-is-going-to-melt-down elements.

Point 3 is interesting, I found this article googling : http://www.ptonline.com/columns/the-strain-rate-ef...
I will definitely discuss that with my colleagues.

Point 4 : we actually think that what the software is having a hard time with is when the model reaches the snap-through point (ie when the walls of the pail snaps abruptly toward the interior/exterior). Typically, the analysis stops with a dialog that reads like "The analysis may have reached the buckling point and, if that's the case, that's where it ends."

RE: Plastic product "crush" or "buckling" test with Solidworks Premium

I actually don't think there is a way.

The only thing I can add is to your part 4. If it's stopping at the snap through, you must be using force control as you solver type. You need to use arc length control for a problem where you want to see the snap through. That may very well be the problem you are facing.

RE: Plastic product "crush" or "buckling" test with Solidworks Premium

I use both Abaqus and Swx sim. You can get a decent approximation with Swx sim in my humble opinion. You need to get rid of the plates in the sim and just use restraints for the top and bottom - fixed should be fine but it depends on what elements are and what the geometry is. The lid contact needs to be bonded to the barrel. You do all this because you don't have arc length or displacement control option in Swx with contact. These assumptions tend to be reasonable in most cases but they may not be if say a failure mode you want to check is the lid coming off but that seems unlikely in a well designed lid. The other thing is that it is very likely, having done a lot of similar container types, that the buckling mode is symmetric so if you know that you can use a symmetrical sector of the model. If the wall thickness is more or less constant (as opposed to tapered) you can use shells. This type of analysis is a lot more challenging in Swx after they changed the arc length control set up back in say 2012 or so - now it takes a crazy number of steps to solve. Stick to displacement control. Even if you can't get past the point of buckling the solution will fail in force control as it approaches the buckling load. Depends on how close you need to get. You can plot the response to see how flat the load deflection curve is at the point of solution failure to get some idea of how close you are - typically pretty close.

Bill McEachern, P.Eng.
Redstone Six Consulting Ltd.

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