Drop test, 16kg kettlebell onto a floor tile

  • 164 Views
  • Last Post 19 February 2019
dpteo posted this 07 February 2019

Hi, currently im doing a drop test of a 16kg kettlebell onto a floor tile from 0.7m height. The impact velocity I calculated is 3.70531m/s.

I am unsure which solver I am supposed to use, explicit dynamics or transient structural. The image attached below is my model. I moved the kettlebell so that it is in contact with the floor tile.

model 

Attached Files

Order By: Standard | Newest | Votes
SandeepMedikonda posted this 07 February 2019

It is typically recommended to use an explicit solver to analyze drop tests. Having said that what is the goal of your simulation?

Regards,
Sandeep

dpteo posted this 07 February 2019

Im doing a test to see if my floor tile can withstand the impact force of the kettlebell dropping from 0.7m and comparing with with an experimental results and I will be comparing the deformation between simulation results and experimental results

peteroznewman posted this 07 February 2019

How is the tile supported in the experiment?  How is the tile supported in the model?

dpteo posted this 07 February 2019

for the experiment will be using a drop tester like this where the tile will be at the bottom and the kettlebell will be attached and released from 0.7m .

for my model i inserted fix support at the bottom of the tile like this 

peteroznewman posted this 07 February 2019

A fixed support in the model is not appropriate to match the conditions of this test.

Does the tile just sit loosely on the bottom plate?  That isn't how tiles are used in a floor. There is usually a concrete-like layer, then tile adhesive, then tile. If you do that for the physical experiment, then you need all that in the model.

dpteo posted this 07 February 2019

for this experiment the "tile" will be 3D printed in either ABS or PLA material and it will rest on the bottom plate. the aim of this project is to test between honeycomb and re-entrant honeycomb shape and see which can absorb more impact and compare the deformation between the two and tally with the simulation results

as it is pretty impossible to get tile with such shape hence the "tile" will be 3D printed and tested

how would you go about setting up the simulation as close as to the experimental?

peteroznewman posted this 08 February 2019

If the 3D printed tile is resting on the steel plate of the machine, then you need a plate of steel, the tile touching that plate and frictional contact between the tile and the plate in the simulation. The underside of the steel plate can be a fixed support.

Make sure the frictional contact on both sides of the tile is closed before the simulation begins with the initial velocity of the kettle as you have calculated.

  • Liked by
  • dpteo
dpteo posted this 08 February 2019

thank you peter, i read your other post on drop test you mentioned doing such test using transient dynamics. is it the same for this case? if so is transient dynamics transient structural in ansys?

peteroznewman posted this 08 February 2019

There are two solvers for transient dynamics simulations: Transient Structural and Explicit Dynamics. The difference is Transient Structural uses an Implicit Solver while Explicit Dynamics uses an Explicit Solver.

Transient Structural is more like Static Structural with time and velocity added in terms of how it works and so may be more familiar to use. The material models generally don't include the material actually fracturing, you have to conclude that from looking at result quantities.

Explicit Dynamics is very different, the solver uses the propagation of sound waves through the media to solve and has built-in the ability to remove an element that has failed the material limits from the model and keep solving. That is why it can be very useful for modeling impact events where things are expected to fracture.

  • Liked by
  • dpteo
dpteo posted this 10 February 2019

thank you peter, how can I calculate the end time in explicit dynamics to cover the area of interest for my drop test? currently I set the end time to 0.0005 and the deformation observed is very minimal which does not seems right. Does the total deformation results show the deformation at the point of end time?

peteroznewman posted this 10 February 2019

At a velocity of 3.7 m/s, the distance traveled without impact would only be 1.85 mm in 0.0005 s so you will want a longer time than that. Yes, the total deformation is at any time you request and defaults to the end time.

  • Liked by
  • dpteo
dpteo posted this 11 February 2019

Thank you Peter, I set the end time to 0.005 which should be sufficient to get a proper impact. However instead of the tile getting impacted on and crushed, the kettlebell bounce up when coming into contact with the tile. There isnt any deformation of any sort on my tile and my kettlebell is fully red on the deformation scale.

dpteo posted this 12 February 2019

Here is what my simulation looks like at the end of the end time

peteroznewman posted this 12 February 2019

The kettle bounced off the tile and is above it at 0.005 seconds.

Which solver are you using?

What material properties are you using?

If you are using Explicit Dynamics, what Analysis Settings are you using?  Specifically, what are the erosion settings?

If you are using Explicit Dynamics, how many Output frames did you request?

dpteo posted this 12 February 2019

Im using explicit dynamics autodyn. Using the material properties of iron for the kettlebell changing the density so that the kettlebell is 16kg and ABS plastic for the tile from the engineering data

Here is the erosion settings

 

peteroznewman posted this 12 February 2019

On the Erosion Controls, You have On Material Failure set to Yes, but I assume there is no Failure criterion defined in the material definition.  In that case, you can set the Erosion to occur On Geometric Strain Limit and enter the strain on which the element will be removed. That is equivalent to using Elongation as the failure criterion.

I would recommend increasing the Result Number Of Points to 500 to see more frames of animation.

  • Liked by
  • dpteo
dpteo posted this 12 February 2019

Thank you peter, will give it a try

dpteo posted this 13 February 2019

Peter, so I changed the geometric strain limit to 0.2. I encountered this "problem terminated .... energy error too large" Anyway to work around it?

peteroznewman posted this 13 February 2019

In Solution Controls, type in a larger value for the Energy Error Tolerance.  You can review the magnitude of the energy error at the end to decide if you can accept the results.

dpteo posted this 19 February 2019

Hi Peter, despite the changes the kettlebell seems to bounce off the tile and not causing much deformation on the tile which seems unrealistic.

I uploaded the wbpz file in the opening post can you take a look to see what is wrong with my parameters and conditions?

I added 2 material into the engineering data namely, iron and PLA

Close