Learning Forum

[Scooped]

Hi everyone,

I've been modelling an impact for a bumper system and changing the bumper rails, the simulations so far have run fine but the crash box part of the model has had issues before which I have previously solved by changing the maximum energy error to 10 as from what I could see the energy summary was fine, this however is not the case this time and my energy error spikes massively, as well as deformation and stress at a single time increment. My main questions are:

Why is my model 'breaking' rather than deforming like it should behave? (its a very thin walled steel structure), I believe i've seen somewhere that you can choose to remove elements which have failed but I want the model to deform rather than shatter like it currently is. Is it my mesh not refined enough there? I want it to crumple up as if it was absorbing the energy of the crash.

What could be causing the sudden spike in energy/stress? How can i solve this?

I've tried to include as much information in photos as I can surrounding the issue.

Thanks

[Chris Quan]

The large energy error is caused by the sudden rise of hourglass energy. The hourglass energy is very large and even exceeds the internal energy. The deformation plot also shows the hourglass deformation.nYou mentioned its a very thin walled steel structure. Did you use solid elements to model the structure? If yes, convert the geometry from solid body to surface body in SpaceClaim or DesignModeler. Then the structure will be modeled with shell elements by Explicit Dynamics solver, which enables the structure to bend under crush loading.nThis should solve the energy problem.n

[Scooped]

Hi cxquan,nI really appreciate your reply, sorry I am still getting my bearings with ANSYS. I did however see that many of the papers which I was following along with seemingly used shell elements but I wasn't sure how to use them. For my geometry it is an assembly imported from solidworks as a parasolid file into design modeller, could you tell me how to convert from solid bodies to surface bodies? When I looked online it said to use a body opertation but it says it can't find any bodies, I've also tried changing the import to only have Surface bodies set to Yes and Solid bodies to No but it gives me an error, which makes me feel like I'm not doing it right. Also, would it be it be possible to select only certain parts of my geometry to set to 'surface body' (most likely the crash boxes I showed in my first post) or would it be beneficial for my entire bumper set up to be modelled with shell elements in an impact scenario?nThanks CxquannScoopednEdit: I've just seen a video online about using space claim, in the video they converted the parts using the 'Midsurface option', does doing this enable the use of shell elements on those pieces of geometry? And if so is there any way of telling which parts of my geometry are going to use shell elements vs solid elements?.

[Scooped]

Update: I've managed to change the two crash boxes in the simulation to MidSection's which I think has made the mesh on them into shell elements. I've seen on other posts here that the min characteristic length is what the simulation time is based off of, but now I have shell elements my mesh matrix is showing my minimum as 0mm, is there a way to see the mesh matrix for only certain objects in my geometry?nThanksn

[Chris Quan]

DesignModeler also has Mid-Surface tool to convert a solid body into a surface body. nOnce surface body is created, no mesh is needed through thickness. Mesh is only created in the plan of the surface body. Shell elements will be used for the surface body.nThe minimum element size could be seen when Mesh Metric is changed to Characteristic Element Length.n