Strange low convergence of axisymmetric problem

[flowglow]

Hello everyone.

I wanted to make a very simple simulation - compression of cylindrical specimen. I was very surprised, when the solution was not converging.. and it is when more complex models work quiet well.
It is a second day, but still I didn't found completely the reason of this strange behaviour of my model.

Model:
Problem:
Cylinder (Arruda-Boyce hyperelastic model, height = 34 mm, diameter = 34 mm) is compressed between two analytically rigid plates. Axisymmetrical approach is used to solve the problem.
Contact:
between plates and specimen - surface-to-surface contact, with friction coeficient=0.1. Normal behaviour "Hard" or "Exponential" (I tried both).
BC:
Bottom plate is fully fixed, Top plate is going down(displacement BC) in order to compress cylindrical specimen with total 15mm displacement.

Abaqus/Standard:
First of all I started with Abaqus/Standard - problem is static, material is rate independent. Approximately at the middle of a step (~7.5 mm) time increment starts to decrease dramatically and finally reaches the minimum limit. On my opinion, large deformations leads to problem in contact zone, and as a result to very small time increment.

Abaqus/Explicit:
It is well known that generally Explicit approach manages large deformation problems with better success. So I switched my model to Abaqus/Explicit solver.
In explicit I tried two variants of time step:
(a) Total time of loading = 1 sec.
(b) Total time of loading = 10 sec.
The Amplitude was created in correspondence with this time.

I expected:
Bigger influence of inertia effects in the case (a), and so more reliable solution in the case (b)

I've got:
Big element distortions and "waves" in the case (b) and stable and fast solution on the case (a)

Could someone explain what is wrong? Maybe Explicit just can't solve problems with big times? Do you have any idea?

In attachment you can find a python script to create this problem on your machine.

Some pictures:
1. left picture: case(a), Time=0.55s; right picture: case(b), Time=5.5s

2. End of solution. left picture: case(a), Time=1.0s; right picture: case(b), Time=10s

 

[StefCon]

Hi,
Did you use double precision for the explicit runs? If there were a lot of iterations, maybe the error will be noticeable. Abaqus gives a warning at more than 300k iterations saying that one "should" use double precision.

Is mass scaling ok?

Cheers!

 

[Mustaine3]

What element type is used?

 

[flowglow]

Hi,
Did you use double precision for the explicit runs? If there were a lot of iterations, maybe the error will be noticeable. Abaqus gives a warning at more than 300k iterations saying that one "should" use double precision.

Is mass scaling ok?
Cheers!

Hi,
Yes I am using a double precision and yes for the case(b) (10 seconds) number of increments is very high (about 2 millions).
I didn't use mass scaling this time. What is better in this case: increasing of a deformation rate or increasing a mass?

What element type is used?

In CAX4RH from Standard library for problem in Abaqus/Standard and CAX4R from Explicit library for the problem in Abaqus/Explicit

 

[Mustaine3]

Try again with CAX4H/CAX4 and also parabolic elements in /Std.

 

[cooken]

This looks like a great candidate for the implicit dynamic solver no?

 

[flowglow]

Try again with CAX4H/CAX4 and also parabolic elements in /Std.

According to documentation only hybrid with constant pressure elements can be used with hyperelastic material (so CAX4H or CAX4RH in mya cese). It doesn't work, stable time increment decreasing dramatically.

This looks like a great candidate for the implicit dynamic solver no?

Truly speaking I've never used implicit dynamic solver, and I can't find a lot of examples of its implementation. For example in the lecture of iMechanica about QS problems there is not a word about implicit dynamic solver(

http://imechanica.org/files/l5-quasi-static.pdf).

If you have experience, what is general purposes of this solver? According to documentation Implicit dynamic analysis can be used to study "quasi-static responses in which considerable energy dissipation provides stability and improved convergence behavior for determining an essentially static solution". Seems that a lot of simulation can be done using this solver, but still only few examples can be found.

 

[cooken]

You can find plenty of info in the Abaqus documentation. This solver is often overlooked but is quite useful in many applications. It shouldn't be too much work to re-configure your model, and I would highly encourage you to just run a simple test and see what you come up with.

Here's an excerpt from the Analysis Manual:

A direct-integration dynamic analysis in Abaqus/Standard:
[ul]
[li]must be used when nonlinear dynamic response is being studied;[/li]
[li]can be fully nonlinear (general dynamic analysis) or can be based on the modes of the linear system (subspace projection method); and[/li]
[li]can be used to study a variety of applications, including:[/li]
[ul][li]dynamic responses requiring transient fidelity and involving minimal energy dissipation;[/li]
[li]dynamic responses involving nonlinearity, contact, and moderate energy dissipation; and[/li]
[li]quasi-static responses in which considerable energy dissipation provides stability and improved convergence behavior for determining an essentially static solution.[/li][/ul]
[/ul]

 

[flowglow]

Yes, thank you, I've looked the documentation already of course, and tried to run too. In this simple case results in explicit (1 second load) and implicit dynamic (1 second also) are almost the same. Implicit dynamic solver works longer (2 min against 20 seconds in explicit) and final reaction force is a little higher (~ 4% difference). So the think is I don't know how to justify results to be sure, that more complex model will be fine too.

 

[cooken]

Why not try the 10 second sim, since that one gave you the problem? A 4% difference is not that bad, and I'm sure you could figure out where it comes from. What numerical damping parameters did you use? Also, have you checked your energy balance in both? That might tell you quite a bit. Another thing to check is the friction enforcement (elastic slip).

Another nice thing about the implicit solver is that you can use second order elements (as Mustaine alluded to). May not help in this case but as with any numerical foray a mesh study is always good to do.

Also can you show what your displacement vs time looks like for the top plate?

 

[IceBreakerSours]

Given the sort of questions you have asked, I suspect you are new to FEM. If that is the case, then you must take it slow - your current strategy is the famous kitchen sink approach

Given what you have mentioned, Abaqus/Standard will get the job done in a static procedure. There is NO need to invoke a dynamic procedure in Abaqus/Standard. Also, Abaqus/Explicit is a terrible tool to use in this situation because of the time duration of concern (1/10 sec).

a) I can not zoom into the images but it looks like there is some hourglassing going on as well; try fully integrated elements in case you are using reduced integration elements, as Mustaine3 recommended with Abaqus/Standard. While I am not sure when the solver gives up, you might also look at the hourglassing energy in the history output; I imagine it must be increasing just before the solver succumbs.

b) Zoom in into the radially outermost region at the top, animate the displacement solution, and ensure the (slave) nodes of the puck are NOT penetrating the rigid (master) surface. While you are doing that, ensure that deformation scaling factor is 1 - although you might want to play with it a little for investigative purposes. If penetration is occurring, then just bias the seeding for the contacting edge so you have smaller elements at the top and bottom.

DS Learning Community has lots of free content on hyperelastic material characterization; join it.

*********************************************************
Are you new to this forum? If so, please read these FAQs:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083