Can I simulate impact using an acceleration load in a static structural analysis?

  • Last Post 25 April 2020
seanatwood posted this 24 April 2020

I am tasked with simulating a drop test for a sheet metal structural frame in ansys and want to know what the best approach will be to simulating this in ansys mechanical.  The engineers before me performed a static structural analysis of the frame, with the frame supported at the base where casters would make contact with the ground, the force of gravity applied to the entire frame, and an acceleration of 15g's applied to the frame in the vertical direction. An acceleration of 15g was determined using drop test onto dense foam that resulted in accelerometer data that peaked at about 15g's. To be conservative they used 15g's as the acceleration in the ansys simulation when simulating the drop test. 

Is this a viable way to simulate stresses on the frame from impact? I'm concerned that this method isn't capturing what's really happening, because in this simulation, the rapid acceleration of the frame at impact will occur on the entire frame, whereas in reality, I think only the bottom of the frame making contact with the ground would experience the impact force and this force would get transmitted through the rest of the frame.

When I've looked online for how to do this, everyone is using explicit dynamics or nonlinear simulations, and we don't want the simulation to be that complex. I'm looking for the simplest way to get accurate results, even if they are conservative, using a linear solution. 

Order By: Standard | Newest | Votes
peteroznewman posted this 24 April 2020

In Workbench, drag and drop a Modal analysis onto the Static Structural model cell.  Open the model then in Mechanical, drag and drop the supports on the four casters from the Static Structural branch onto the Modal branch. Edit the Analysis Settings and increase the number of modes from the default 6 to 24. Make sure that all the materials in the model have a density correctly defined in Engineering Data. The structure supports some heavy components. Add point masses and scope them to the faces that support them. When you click on Geometry, it will show the total mass in the model. You need to get that up to the actual weight of the structure with all the components attached. You can also add distributed mass to represent cables and pliable enclosure parts that add mass but don't add any stiffness.

It is very useful to know the natural frequencies in the Structure at the beginning of any kind of impact analysis.  Under the Solution Information folder, the Mass Participation Summary is now available. Please snap an image of that and insert that into your reply.

Please reply with details of where the accelerometer was mounted on the structure. Insert a photograph into your reply, if possible.

peteroznewman posted this 25 April 2020

One paper I read about product fragility by Gaberson described how a product was subjected to six different shocks.
Below is the plot of the acceleration vs time plot for each of those different shocks. 
Many replicates of the product were tested on each of these shocks. A new product used for each single application.
After the application of one shock, the product was tested to see if the shock broke the product.
One of these shocks never broke the product being tested. Five of these shocks always broke the product being tested.

Can you guess which shock did not break the product?

The answer is the blue curve in the top right did not break the product. The other five always broke the product.
The point is that peak acceleration is a very poor measure of the damage a shock can do to a product.
The conclusion is that Pseudo Velocity Shock Response Spectrum is a much better way to evaluate shock severity.