Learning Forum

[MTayyab]

I am trying to do a drop test. The body to is 10m in the air and i apply standard earth gravity and velocity as initial condition of 15m/s. I tried different end time values from 0.001 to 0.5 seconds. I reduced the maximum number of cycles to 10000 to reduce the calculation time. But after the solution the object does not move as expected. It seems to be stuck in space. Even if i reduce the distance between the fixed support and the body to 200mm the same happens.

[peteroznewman]

Reduce the distance to 0.  You want the body being "dropped" to be in CAD just touching the surface it will impact. The body being "dropped" is instead assigned an Initial Velocity that is calculated from the drop height using a calculator like this or just using the simply accelerated motion equations.

In Explicit, under Output Controls, increase the Number of Output Points from the default of 20 to 2000.  If you set the End Time 10 times bigger, then you need to set the output results to 10 times more output points.

[MTayyab]

thank you for your reply! i noticed in the solution information that the incremental time is very small so, if i run the simulation for 10000 cycle it will progress very little as compared to 1e^07. So, to completely capture the whole phenomenon the number of cycle should be high or the time increment should be greater. Is there a way to increase the time increment because it takes too long for the solver to solve for this high number of cycles even if the end time is very small.

[peteroznewman]

Welcome to Explicit Dynamics. 

The maximum time increment is computed from the smallest element size in the mesh. If you make the smallest element larger, then the time increment will be larger.  Use the Mesh Quality Metric Characteristic Length to find out which element has the smallest value in mm.  Then use Mesh Controls to make the smallest element many times larger.  Changing element size doesn't change the dynamics of the model, only the time increment.

The maximum time increment is also computed from the density of the material.  If you use higher density materials, the time increment will be larger. If you increase the density by a factor of 100, the time increment will be 10 times larger.  Changing density changes the dynamics of the model.

The maximum time increment is also computed from the Young's Modulus of the material. If you lower the modulus, the time increment will increase. Changing Young's Modulus changes the dynamics of the model.

If you just want to see some results of a model with different dynamics than your original model, just temporarily increase the density by a factor of 100 and see how it looks. Then you know it will take about 10 times longer to do it with the correct dynamics using the original density.

[MTayyab]

Thank you very much for the information! Can you please tell me if the number of result points in analysis settings effect the simulation run time?

[MTayyab]

 one more question! Is it possible to find out the amount of force one object  inside another would exert on the outer one while impact? Do the contact force in solution information gives these forces?

[peteroznewman]

Number of result points has a small effect on run time since solver has to write out more data.

Try the model with one object inside another and see what you get, but make sure to request contact forces or you don't get those results in the output.