13 Replies Latest reply on Nov 4, 2014 10:14 AM by Jared Conway

    Require some help perfoming impact simulation

    Jessie Brambell

      Hello everybody,

       

      So I'm trying to perform a basic crash test in SolidWorks of a model I have created. But first, I'm trying to figure out how to exactly perform a crash test! From what I've read online, impact tests are normally done in nonlinear dynamic studies. My long term goal is to extrapolate what I learn here to a larger, more complex model for impact testing. Here is what I have so far:

       

      http://i.imgur.com/M58O6cH.jpg

       

      Right now, I'm more concerned with just getting the basics of crash simulation down, so I've chosen a very simplistic model to learn from. The large wall is fixed, and there is an initial condition of 20m/s set on the smaller cube in the direction of the wall. There is a no penetration contact set between the wall and the cubes front faces, and a global contact between the two parts (I've tried running it with Global contact off, when I did I received the error "no initial contact is detected"). Currently when I try to run the simulation, I get some pretty weird results, indicating to me I've obviously done something horribly wrong. I've also tried looking up YouTube videos and help guides on impact simulations, but unfortunately it doesn't look like there is a whole lot to learn from. This is the best example of what I'm trying to do I have found so far:

       

      https://www.youtube.com/watch?v=JnO3wfnQXLs

       

      From his simulation, I know its possible to perform an impact test, I just can't figure out for the life of me what I am doing wrong!! Anyways, If anybody is willing to give me any information they have on performing an impact test using nonlinear dynamic simulation, I would love to hear it. Also, for anybody who wants to take a look at the assembly:

       

      https://www.dropbox.com/s/v4fd90nal7vs1an/Impact%2...

       

      Thank you for your time.

        • Re: Require some help perfoming impact simulation
          Jessie Brambell

          Hello again everybody, a little update, I did manage to get the impact simulation to run and produce correct results! 2 reasons I found why the model would not simulate before:

           

          1) Cube was not properly constrained, added a fixture in X and Y to a vertex point on the cube to only allow motion in Z direction.

          2) I was not aware you could apply the initial condition to the ENTIRE body of the cube.

          3) Most importantly, the cube must be in contact with the wall when you initially run the simulation, or else initial contact will not be detected, and the simulation will fail.

           

          Now that I have this simulation going, I want to be able to extrapolate this to an impact test using beams, but from what I've read so far, it looks like SolidWorks doesn't like doing contact sets between beams and solids. From what I have read, a face on a beam is not valid face (not entirely sure why), and therefore cannot be used in the setting of a no penetration contact between a beam and a solid. I have also tried setting no penetration contact between the wall and a beam on my models body, and just as I read I receive the error "invalid entity on beam body was selected". Regarding this fact, I have two new questions if anybody is willing to take a stab at them:

           

          1) Is it possible to define a no contact penetration between a beam and solid body?

          2) If it is not possible, what is usually done in nonlinear dynamic studies when dealing with beam bodies?

           

          Thanks again.

            • Re: Require some help perfoming impact simulation
              Jared Conway

              3) Most importantly, the cube must be in contact with the wall when you initially run the simulation, or else initial contact will not be detected, and the simulation will fail. >> this shouldn't be the case. otherwise how would you do impact analysis of something hitting an aircraft for example. I suspect maybe your issue is that you're trying to use global contact vs a contact set.

               

              as for beams and contact, the faces don't exist. they may look like it on the screen but they are basically 1d elements. if any contact is available it is between the length of the beam and something but even then, if it was large and flat, it wouldn't know what the contact looks like. your only option is to use solids.

                • Re: Require some help perfoming impact simulation
                  Jessie Brambell

                  Thank you both for the replies!

                   

                  As far as initial contact is concerned Jared, you were correct, removing global contact on the simulation seemed to fix the issues the solver had with initial contact. Thanks for the correction!

                   

                  Alessandro, I really wish I could do the impact portion as a solid, and the rest as a beam, but I believe this might not work for the simulation I am doing. I'm testing to see how strong a roll cage I have modeled is, which is comprised completely of beam elements. I might be bad intuition on my part, but I feel like using both beam and solid elements in the analysis for the roll cage might produce some weird results. What do you think?

                    • Re: Require some help perfoming impact simulation
                      Jared Conway

                      Mixing and matching element types is standard procedure. You could go with shells if you were looking to standardize.

                       

                      are you sure this is a worthwhile endeavor for simulation? Have you at least checked everything else out? This is a complicated simulation. In the automotive industry there are dedicated software packages for this and dedicated analysts.

                        • Re: Require some help perfoming impact simulation
                          Jessie Brambell

                          Its without a doubt a worthwhile endeavor if I can get it to work! The impact analysis is for a school club, and really all we have available to us for this type of analysis is hand calculations and SolidWorks. We do not have funds for anything else, so at this point I'm just trying to put in the time and effort to get the simulation to hopefully produce some semi-accurate results that may be of use to us. By the way, sorry for the delayed response, school is quite busy at the moment, and I only get to work on the simulation for a couple of hours every second day or so. Currently I have actually managed to get the impact analysis to solve once or twice, but it ended up producing some pretty inaccurate results. I do have another question, however, which I hope you don't mind answering!

                           

                          I keep running into the same error for the most part: "PCGLSS0102:Assembled Stiffness Matrix has a negative diagonal". From browsing the forums, I have read that the two main reasons for this error are:

                           

                          1) Lack of adequate restraints for one or more parts.

                          2) Load increment may be too large or too small.

                           

                          I don't believe the problem is number 1, just because I have tried numerous different constraints on the "wall" I am using for the impact fixture, and I receive the same error regardless. What I think it may be causing the error is number 2. See, currently the analysis is set up for a 100lb roll cage made of steel to impact at 15m/s into a 2 inch thick rubber wall. This creates some pretty high load increments for the rubber wall, which I believe may be the reason for the error.  Here is where I get stuck though, I'm not quite sure how to get around this. I'm still very new to nonlinear analysis, so I'm not 100% sure if there is even a way to make this work. What do you think, Jared? Do you have any suggestions or tips for where to go from here?

                           

                          Thanks again for all the help!

                          • Re: Require some help perfoming impact simulation
                            Jessie Brambell

                            Here is the link to the model Jared.

                             

                            Dropbox - Tire impact test.zip

                             

                            Final study is the one I am working on, since I have already managed to get results from study 1 (Only difference was Study 1 was done at 55km/h, while the final study is at 80km/h). Basically, I figured out how to fix the negative diagonal error (Reduced singularity elimination factor to 0.5), but then I got stuck on the "incremental strain is too large" error, mostly because of the high deformation occurring from the impact with the rubber. I used mesh control and reduced the size of the mesh to very fine, and today after 6 hours it worked! Although now, I've started to attempt to run the simulation at 80km/h, and it seems SolidWorks really does not like the amount of deformation going on, so I figure using the finest mesh is my only option, meaning the solve time is going to be well of 6 hours. Anyways, if you have any suggestions for my setup, I'd love to hear them!

                             

                            Thanks again Jared!

                      • Re: Require some help perfoming impact simulation
                        Alessandro Tornincasa

                        Hi Jessie,

                        what Jared said is correct, you need to use solids.

                         

                        Modeling the whole beam with solids will make your non linear dynamic calculation too much time consuming.

                        Why don't you model the first portion of the beam with a beam element, and the the final portion (the one that will go in contact) as a solid ?

                         

                        Alex

                         

                        www.solidworksacademy.blogspot.com

                      • Re: Require some help perfoming impact simulation
                        Sean Screws

                        Exactly what results are you interested in?

                         

                        For example, some nonlinear dynamic simulations I've seen are trying to see wave propagation through the solid and associated stresses. Very difficult simulations to try and perform. Can you decompose the problem to a peak impact force so you can run a linear/nonlinear static analysis?

                        • Re: Require some help perfoming impact simulation
                          Jessie Brambell

                          Real quick question for anybody interested, about how much can you increase maximum incremental strain in the nonlinear dynamic options before it starts to the effect simulation results? I'm constantly running into "incremental logarithmic/plastic strain is too large" in my solver, which causes SolidWorks to reduce the time step, although the study does end up solving, it just takes a large amount of time (26 hours...). To get an idea of what I'm dealing with, its an 80km/h impact into a solid wall. I expect there to be large deformations, and thus large strains. So, if anybody can possibly give me a range of what the maximum incremental strain I can set is, that would be fantastic!

                            • Re: Require some help perfoming impact simulation
                              Jared Conway

                              So, if anybody can possibly give me a range of what the maximum incremental strain I can set is, that would be fantastic! > i do not think that there is a specific range for this. this is basically a last ditch effort. and i do not think that this is what is changing the timestep. are you sure the setup of the problem is optimized? using shells, that you really need nonlinear dynamic, using linear elastic material, solves as a static and then linear dynamic before moving to nonlinear dynamic?