Hello again!
Is there a way to add a rigid wall that has a mass and initial velocity? I'm currently using a 3D solid, giving it a material card that essentially rigid properties, and assigning its nodes an initial velocity. It generally works fine but the contact often results in extremely deformed/negative volume elements on the "softer" material that is being impacted. The kinetic energy from the rigid impactor (with a mass and initial velocity) gets dissipated as it contacts the receiving material. I'd like to have the same scenario with a rigid wall that has initial kinetic energy that gets dissipated. Any ideas?
Hi @jhaley,
When dealing with impactors like rigid walls, you need to think about what you are trying to model. It's easy to model something hitting a rigid wall because all you have to do is constrain the wall in space. Any resulting forces will be a result from the object hitting the wall.
However, when you are applying a velocity to a rigid wall, you need to make sure that the wall is representing what you want it to represent. If it's a vehicle with a mass of 1300 kg then you need to to define inertial properties to represent that. Example: You have two cases, a 10 mm thick wall and a fully modeled vehicle. Both are modeled with a rigid material but the wall has a much higher density so that both weigh 1300 kg. The wall is going to behave differently during an initial velocity impact than the fully modeled rigid vehicle. Something that you can do is measure the inertial properties of the rigid vehicle and then apply these to the wall so that it behaves "similarly" to the vehicle. You can measure this by going into the Element side tab -> Measure -> Inertia -> Active elements only (only have the object to measure active) -> All. https://feassistant.com/forums/ls-dyna/ls-prepost-measurement-tool/#post-12
You can apply inertial properties to a part by changing from a standard *Part to *Part_Inertia.
Long story short: Apply an initial velocity to the parts of the simulation that you are analyzing and not the rigid wall if you aren't restricted by a certain testing setup. But if you have too, make sure you have the correct inertial properties for the rigid wall.
Regarding the issue with your elements during the contact: A rigid wall impacting very soft materials is going to be prone to instability, especially at high severity impacts. You can adjust your contacts to counteract this with some additional parameters like Soft=2 coupled with Depth=5 or Soft=1 which is meant for a contact between hard and soft surfaces. I've attached a picture of how to access these other options and a link to more info.
https://www.dynasupport.com/howtos/contact/soft-option
You should also mess around with different types of entities used for the contact (segment sets vs parts) especially if you have solid parts which may perform better with segment sets in a contact. You can also vary the master and slave stiffness values (SFS, SFM) as well as the viscous damping coefficient (VDC) which can help with values around 20 to 40 usually.
You should also add your soft parts to *Contact_Interior which is necessary for minimizing instability of soft components. Just make a *Set_Part of all of the parts that are soft (yes it can be just 1 part) and then reference this part set in the *Contact_Interior card. You can only have 1 *Contact Interior so don't try to make more than 1 of them, but you can add as many parts as you want to the part set referenced by it. (Just FYI)
And finally your hourglass formulation of the soft part can play a large role in the stability of that part. Here's a helpful resource that explains it all better than I can in a few paragraphs. Feel free to ask any specific questions, I hope this helped!
http://ftp.lstc.com/anonymous/outgoing/jday/hourglass.pdf
