Time Scaling

[BigLeon]

I am using ABAQUS/Explicit for structural impact problem. Unfortunately, the model become instable soon after contact. I guess there should be a user defined scale factor to control the time step like LS-DYNA. I searched the keyword manual but unsucessful. Could somebody tell me how can I control the time step.

Leon

 

[corus]

Not knowing much about Explicit, you could try having multiple steps of shorter time duration.
There may be other reasons why the contact becomes unstable, however. If you look at which nodes are opening and closing then you may be seeing "chattering" which can be prevented by using contact controls. You'll have to explain the instability better.

 

[DickButkus]

ABAQUS/Explicit contact is unlike contact in ABAQUS/Standard. The stable time increment is normally governed by the time it takes a stress wave to cross between the two closest nodes - a very short time indeed!

When /Explicit dies unexpectedly it is usually one of two things - the velocities are too high, or the material is too dense.

To artifically increase the time step you have the choice of variable or fixed mass scaling. The mass scaling may be applied such that the mass in each element is only increased enough so that the user defined time increment is reached.

It sounds like increasing the time increment is not what you are after since it appears that the problem goes unstable once contact occurs. Usually when this happens to me I have my units messed up. Remember that ABAQUS knows nothing of units, so it is your job to be consistant. This means that if you want to use PSI then your length is inches, your time is seconds, your force is lbs, then your unit of mass becomes a very convenient lbf-s^2/in^4. So the density of steel is not .283 but more along the lines of 7e-4.

A convenient unit of measure for explicit is length in mm, force in newtons, velocity=m/s, and time becomes milliseconds! It sounds weird at first, but this system works out very well for explicit.

Now, regarding contact... In 6.3 ABAQUS Inc. introduced "General Contact" this is basically automatic contact. The penalty stiffness parameters are chosen automatically so you can simply tell ABAQUS to find the contact itself. This form of contact actually occurs on element edges and not just slave nodes. This allows for a very coarse mesh to be used and even allows for shell edges to contact in space and even beam to beam contact in space. This new form of conact is very high performance (although it does not parallelize very well) and is even faster than individual 3D contact pairs. ABAQUS says that this form of contact was introduced for the crash simulation market.

I truly hope this helps!

Best regards,
KF9RI

 

[BigLeon]

Hi KF9RI,

I sincerely appreciate the kind help from you. I used the same input file using version 6.2-1 and 6.3, the failure occured in 6.2-1 does not come up when I used 6.3. Somehow, i guess this is because the force in 6.3 is distributed on the element edge. In previous version, if the contact force is exerted on node, the node will be excited to an unrealistic speed, which I believe is the reason for unstable mesh.

Best regards,
Leon