Linear Simulation taking suspiciously long in Explicit. 1

[OverWorked453]

Hi everyone

I have a question regarding simulation time. In general, I want to speed up the time it takes to run my simulation. In fact, I think the simulation should take less than 2 hours but instead it takes about 2 days. I explain the details of this simulation below.

I have a simulation in which a skid landing gear falls to the ground. The material is Aluminum and I define this material as if it were always linear (I do not define any plasticity or nonlinear property). The solver is Explicit, and the simulation is set to 5 seconds with automatic time steps. The landing gear falls onto a discrete rigid surface composed of one single element. The interaction between the landing gear and surface is defined as "surface-to-surface (explicit)". This gear is connected to a node (this node has mass/intertia properties defined to it) via beam connecters defined in abaqus. Also, the mesh consists of approximately 2000 shell elements.

So, can any of you tell my why my simulation takes so long (about 2 days)? Any suggestions on how to speed this up? The material is completely linear. The landing gear falls to the platform in the same way a helicopter w/ a skid landing gear would fall for a standard drop test. I feel the simulation time should be 'short' (less than 2 hours), especially since I define the material as linear.

Any suggestions would be greatly appreciated
Thank you

 

[burningDiesel]

The problem is not linear or non-linear, its the 5 seconds.
Put your structure close (like 1e-10 close) to the surface, and assign it the velocity it would have at impact.
If this does not significantly speeds up your simulation, look into mass & time scaling.
Alternatively, try to model it using dynamic implicit.

Anyway, good luck, impact analysis are not difficult to set up or compute, but relation to the actual behavior can be very challenging, with mostly unknown damping, friction, viscoplastic effects, ...

 

[Dave442]

Hi OverWorked453,

In explicit analyses you specify a solution time and the solver advances in an incremental manner. To get an economic solution you can:

1. Reduce the solution time
2. Increase the size of the time increment

If you reduce the solution time you should be careful to monitor the energy balance to make sure that you do not adversely influence your results. Alternatively, the size of the time increment may be estimated as follows:

dt = Le/Cd where Cd = sqrt(E/rho)

Here Le is the characteristic length of the smallest element in the mesh, E is the Young's modulus and rho is the mass density. Looking at this equation, you can increase the size of the time increment by either:

1. Increasing the characteristic length of the smallest element in the mesh
2. Increasing the mass density

So you can either increase the size of the smallest elements in your mesh or increase the mass density of your material. Again, if you increase the mass density you should be careful to monitor the energy balance to make sure that you do not adversely influence your results. All of this is explained really well in the ABAQUS documentation. Have a look at Chapter 6.3.3: Explicit Dynamics Analysis in the Users Guide.

Good luck,
Dave

 

[OverWorked453]

Thanks! Both of these posts have been extremely helpful. I'm looking at mass scaling, and trying to assess whether it effects the overall results. I've also set up an implicit model.

I like the ideas of changing the density and/or minimum element length. I changed the density of the simulation, and the simulation speed drastically increased. However, I'm measuring motion of a few nodes in my sim, so changing the density effects the results. I'm working an making a mesh with longer element length, however, due to some of the geometry, some small elements are inevitable.

Also, after my troubleshooting it is clear that this long simulation time is due solely to the interaction/contact in the model. I define this interaction as surface-to-surface contact, with the constraint formulation defined as the 'kinematic contact method'. Also, the interaction property has pressure-overclosure defined as "hard".

**
** INTERACTION PROPERTIES
**
*Surface Interaction, name=MyProperty
*Friction
0.35,
*Surface Behavior, pressure-overclosure=HARD
**

Perhaps the long simulation time is due to the way interaction is defined?
If so, is there a more simplistic way to model the interaction (such that it doesn't slow down the simulation)?
It's also possible that this long simulation time is not directly because of the interaction property but because of a large/rapid load occurring in the event of the impact at this contact/interaction.
Any ideas?


The input has been very helpful so far. Thank you.

 

[burningDiesel]

It's difficult to say without more info. The contact algorithm is most likely not to blame.

What could be happening is that some elements are getting heavily distorted, changing the Le from Dave's post. You can see this in the .sta file.

If you have only few small elements, you can check "variable mass scaling".

 

[Dave442]

Hi OverWorked453,

I would probably agree with sdebock - your problem is most likely due to your mesh. Remember that the size of the time increment is dictated by the material properties and the smallest characteristic length of the smallest element in your mesh. As such, just one excessively small element in your mesh will reduce the size of the time increment for your whole model.

If I remember right, the explicit solver will issue a warning message if it detects any excessively small elements. These elements are then saved as a set titled "WarningElems...." and can be viewed in the post-processing module. Have you gotten any warnings like this?

If your geometry has a number of complex parts that require excessively small elements you should determine to what extent these parts influence the behaviour of the model. If possible, you may be able to remove these complex parts to avoid excessively small elements.

Another tip I guess would be to exploit symmetry if possible.

With regards to mass-scaling, I used to run explicit analyses with the correct mass density and note the size of the time increment. I would then use mass-scaling to reduce the size of the time increment by an order of magnitude and check the results/energy balance to determine the effect on the solution. I would continue to do this until I found the most economic solution possible without adversely affecting the results.

Although it is great for highly nonlinear problems, the explicit solver will generally take much longer than the implicit solver to obtain a solution. This is because the implicit solver is unconditionally stable and much larger time steps are generally adopted.

Good luck,
Dave