December 12, 2020 at 5:57 pmsankarsuresh01Subscriber
I am performing a crash test between a fixed chassis and a moving chassis frame. I have imported the model as sketch, and have made a 1d mesh on it.December 12, 2020 at 6:04 pmpeteroznewmanSubscribernWhy do you expect only 1-2 mm of deflection?nThere are two components to deformation of the moving chassis crashing into a fixed chassis. 1) The deformation of the one part of the moving chassis relative to the impact point on the frame of the moving chassis. 2) The deformation of the impact point on the fixed chassis. These are added together when looking at the deformation of any point.nDecember 12, 2020 at 6:19 pmsankarsuresh01Subscriber
@sankarsuresh01 Why do you expect only 1-2 mm of deflection?There are two components to deformation of the moving chassis crashing into a fixed chassis. 1) The deformation of the one part of the moving chassis relative to the impact point on the frame of the moving chassis. 2) The deformation of the impact point on the fixed chassis. These are added together when looking at the deformation of any point.https://forum.ansys.com/discussion/comment/100149#Comment_100149I'm supposed to find out the maximum deformation that can occur in the chassis during an impact. Actually, a static structural test was performed on the chassis by one of my friends, where he had specified the force during impact on the front bulkhead. This gave him only a maximum deformation of 1.76 mm on the chassis. I know that it might not be right, since the other parts are stationary in that case, but at least a single digit can be expected here right? nAlso, some of the chassis members, on impact, bends too much, like its too flexible.. If I play the video made on total deformation, I can see those chassis members bending too much like its a string... back and forth... Is that right? Or maybe I made a mistake?nThanks in advance.nDecember 12, 2020 at 7:22 pmpeteroznewmanSubscribernHow did your friend come up with the force during impact? Did he do a simple Energy hand calculation? I will describe that below.nWhat is the total mass in kg of the moving chassis as reported by the model? Call that m. You said the impact velocity is 11.11 m/s so call that v. The Kinetic Energy in the moving chassis is KE = 1/2 m v^2nAt the peak deformation of the frame, the KE is stored as Strain Energy SE in the two frames. The simplifying assumption is that all the KE is converted. The strain energy in a frame can be calculated from SE = 1/2 k x^2 where k is the spring rate of the frame and x is the deformation of the impact point on the chassis, which acts functionally like a linear spring.nYou calculate the spring rate of a frame k by applying a static force f and dividing by the distance the point moved d which means k = f/d or in other words, a linear spring.nIf the moving chassis was rigid, and only the fixed chassis was being compressed, then you would set KE = 1/2 k x^2 and solve for x. That is what I have done when a rigid body impacts a flexible body. Take this x as an upper limit.nIn your case, you have two equal flexible bodies, so I would divide the KE in half and assume that each frame stores as SE half the KE. This gives a lower limit for x. Finally, calculate the impact force F = k x using one or the other limits.nThe above is a hand calculation and ignores many things that happen in an Explicit Dynamics simulation. When a member goes sideways, it has buckled and the axial stiffness it had disappears, allowing other members to bend more and in different ways and resulting in a reduction in the spring rate computed for the hand calculation.nDecember 12, 2020 at 7:32 pmsankarsuresh01SubscriberThank you. Yes, he did a simple hand calculation. I think my analysis might be right in that case. Thank you for the explanation...nDecember 12, 2020 at 7:34 pmpeteroznewmanSubscribernYou should do the hand calculation above and see what you get for the upper and lower limits for x.nDecember 13, 2020 at 8:43 amsankarsuresh01SubscriberActually, I think I found out what is the problem. The displacement of the chassis model is also being taken into account in the deformation scale, when it is moving towards the other chassis. I can see the colour of the chassis changing before it even hits the other one. I'm trying to bring the chassis more closer now. I'll tell what happens after the analysis.nDecember 13, 2020 at 1:44 pmpeteroznewmanSubscribernYes, displacement and deformation mean the same thing in the deformation results plot. It is the distance a node moves from its original location.nAll impact studies should begin with the parts touching.nWhat did you get from the hand calculation?nDecember 13, 2020 at 2:52 pmsankarsuresh01Subscriber
@sankarsuresh01 Yes, displacement and deformation mean the same thing in the deformation results plot. It is the distance a node moves from its original location.All impact studies should begin with the parts touching.What did you get from the hand calculation?https://forum.ansys.com/discussion/comment/100172#Comment_100172This is what I did for the hand calculations. I'm not sure whether its right though.nMass of the chassis, m = 147.4 kgs (Since I'm including the chassis weight along with driver, engine and other parts)nVelocity during impact, v = 11.11 m/snKE = (1/2)*m*(v^2)nKE = (1/2)*147.4*(11.11^2)nKE= 9096.95 J (for moving chassis)nnSpring rate k = f/d nf = force appliednd = deformationnforce applied, f = 10500Nndeformation obtained, d = 0.25mm = 0.00025 mnThereforce, k = 10500 N/0.00025 m = 42000000 N/mnnSE = (1/2)*k*(x^2)nFor the upper limit of x, SE = KEn9096.95=(1/2)*42000000*(x^2)nx^2 = (9096.95*2)/42000000nx^2 = 4.33*10^(-4)nx = 0.020813 m (upper limit of x)nnFor lower limit, SE = KE/2nSE = 9096.95/2 = 4548.475 Jn4548.475 = (1/2)*42000000*(x^2)nx^2 = 2.165*10^(-4)nx = 0.014717 m (lower limit of x)nnTherefore, Impact force F, keeping both bodies as flexible (taking lower limit of x)nF = 42000000 N/m * 0.014717 mnF = 618114nIs this right? @peteroznewman, Also, since I'm importing the chassis sketch and performing a 1-D analysis on it, I'm trying to place both the chassis sketches as close as possible in the CAD software, and import it (considering the tube thickness and radius). nThanks for all the help. I truly appreciate it.December 13, 2020 at 2:56 pmsankarsuresh01SubscriberAlso, can you suggest me a good way I can follow to get the result without considering the displacement and only the deformation of the chassis members? Thanks nDecember 13, 2020 at 3:26 pmpeteroznewmanSubscribernWell done! Hand calculations are an essential tool to make sanity checks on your simulation results.nYou used m = 147.4 kg in the hand calculation. What is the mass in the model? In Mechanical, click on Geometry and in the Details window, the Properties category shows the mass. If your model only has a small fraction of this total mass, right click on Geometry and insert a distributed mass to make up the difference. All the rest of the calculations look correct.nI don't understand your final question, which result are you talking about? What is the difference between displacement and deformation? Do you mean displacement is the rigid body motion before impact? You remove that by having the two parts touching at the start of the simulation.nDecember 13, 2020 at 3:47 pmsankarsuresh01Subscriber
@sankarsuresh01 Well done! Hand calculations are an essential tool to make sanity checks on your simulation results.You used m = 147.4 kg in the hand calculation. What is the mass in the model? In Mechanical, click on Geometry and in the Details window, the Properties category shows the mass. If your model only has a small fraction of this total mass, right click on Geometry and insert a distributed mass to make up the difference. All the rest of the calculations look correct.I don't understand your final question, which result are you talking about? What is the difference between displacement and deformation? Do you mean displacement is the rigid body motion before impact? You remove that by having the two parts touching at the start of the simulation.https://forum.ansys.com/discussion/comment/100179#Comment_100179@peteroznewman, I actually added the mass of those objects on the particular members which support them, by specifying force on those members downward. nMy question was, for the analysis, I import the sketch of 2 chassis in STEP format, and provide the cross section thickness in designmodeler. So, in the sketch, in CAD, I cant give the same edge for both the chassis right. And keeping them too close also throws an error in ANSYS, which i guess is due to the intersection of the two tube meshes. So, my question was that, what can I do to give me results of displacement of chassis members alone, rather than the displacement of the chassis before impact, when I have imported the chassis as a sketch? (Since I dont think it is possible to give a common edge for the front bulkhead members).... Thanks in advance. nDecember 13, 2020 at 4:35 pmpeteroznewmanSubscribernSpecifying a downward force to represent the weight of parts attached to members of the frame is not adding mass to the model. In a static structural analysis where you want to know the deformation of the frame under a 1g gravity load downward, you get the right answer. nBut for a crash simulation, where the the g force can tens or hundreds of g horizontally, you don't get the right answer. nDelete the force and add the mass to the model, then it works for both crash simulations and statics. In the statics, add a Standard Earth Gravity as an Inertial load and you will get the right answer.nAre you using Body Interaction to detect the impact? Put the lines very close to each other, like 1e-5 m then in the Mesh Details, under Sizing, turn off Mesh Defeaturing. This is what is causing the meshing problem. Now the two frames are practically touching. There is no contact at the tube radius. The centerline itself is what makes contact. You could attach a surface to the front of one chassis so that there is an area for the other chassis to impact with.nDecember 13, 2020 at 5:33 pmsankarsuresh01SubscriberI cant find the Insert option to insert the distributed mass in Geometry. nThese are the only options available. I checked the mass in the properties tab. It was as expected. What can I do about the other loads (driver, engine)? Thanks in advancenI'm using ANSYS 17.1 by the way.nnAlso, I tried with the distance you had specified earlier. I get the same message I got before. I had also turned off the defeaturing of mesh.nnDecember 13, 2020 at 6:15 pmpeteroznewmanSubscribernDistributed mass was added in the last few years, ANSYS 17.1 is probably more than 5 years old. In your case, you can attach a Point Mass to the relevant member for each significant mass such as engine, driver, etc.nOkay, now that you show the actual error message, it is not an error in the meshing, it is an error from the solver. Did you try switching contact detection to trajectory contact?nDecember 13, 2020 at 7:53 pmsankarsuresh01Subscriber@peteroznewman, Contact detection is already set as 'Trajectory'. And, I cant find an 'Insert' tab to insert the Point mass, in geometry. I can only find the options given in the below quoted text... I have included a picture in this. Thanks in advance.n
@peteroznewman I cant find the Insert option to insert the distributed mass in Geometry. https://us.v-cdn.net/6032193/uploads/CTR1IKKONM9Q/image.pngThese are the only options available. I checked the mass in the properties tab. It was as expected. What can I do about the other loads (driver, engine)? Thanks in advanceI'm using ANSYS 17.1 by the way.Also, I tried with the distance you had specified earlier. I get the same message I got before. I had also turned off the defeaturing of mesh.https://us.v-cdn.net/6032193/uploads/7YRMDOBIHGA8/image.pnghttps://forum.ansys.com/discussion/comment/100188#Comment_100188nDecember 13, 2020 at 11:59 pmpeteroznewmanSubscribernInsert Point Mass and Distributed Mass was available in 18.2 which is the oldest version I have.nSince it is not available in 17.1 you will have to use APDL command objects to put the code in manually. nI don't need to know those commands so you will have to figure that out for yourself or post a new thread to ask that specific question and someone else might answer.nOr you can add more geometry, assign the density so that the mass is correct, and use Fixed Joints to connect a face on the new body to the member that needs to support it.nDecember 14, 2020 at 4:59 amsankarsuresh01SubscriberAlright, I'll do that. But, I'm getting the same error as before. What can I do about that? Thanks in advancenDecember 14, 2020 at 5:04 ampeteroznewmanSubscribernMove the pieces apart and in the deformation plot, subtract that distance from the axial component of deformation.nDecember 14, 2020 at 5:32 amsankarsuresh01Subscriberok... Thanks a lot for the help... nDecember 14, 2020 at 2:46 pmsankarsuresh01Subscriber@peteroznewman, Sorry, but I have one more doubt. In my chassis, I have 2 different tubes, with different thickness. So, I apply Boolean to one kind of tube, to one chassis. So, totally, there are 4 booleans present. If I apply Boolean for all the tubes in a chassis, all the tubes are assigned the same thickness, which I dont want. So, when I use 4 Booleans, I convert the booleans in a single chassis into a part, and same for the other chassis too.. So I get 2 parts. Now, when I do the analysis with this, I get the same error I had asked about earlier. What can I do to prevent it? Thanks in advancen
@peteroznewman I cant find the Insert option to insert the distributed mass in Geometry. https://us.v-cdn.net/6032193/uploads/CTR1IKKONM9Q/image.pngThese are the only options available. I checked the mass in the properties tab. It was as expected. What can I do about the other loads (driver, engine)? Thanks in advanceI'm using ANSYS 17.1 by the way.Also, I tried with the distance you had specified earlier. I get the same message I got before. I had also turned off the defeaturing of mesh.https://us.v-cdn.net/6032193/uploads/7YRMDOBIHGA8/image.pnghttps://forum.ansys.com/discussion/comment/100188#Comment_100188nDecember 14, 2020 at 9:00 pmpeteroznewmanSubscribernDon't use Booleans on tubes with different wall thickness, use Shared Topology. If that is not working, use Bonded Contact. Either of those will allow different tube thicknesses.nDecember 15, 2020 at 5:14 amsankarsuresh01SubscriberShared Topology is giving me the same error. And, I'm not able to create a bonded contact between 2 lines. What can I do? Thanks in advancenDecember 15, 2020 at 10:11 pmpeteroznewmanSubscribernYou can create a Fixed Joint between vertices of tubes that meet at a common point. Click on the Display tab and use the Explode tool to separate the two lines so that the vertices have a space between them instead of being coincident. That makes it much easier to create the Fixed Joint.nViewing 23 reply threads
Ansys Innovation Space
- The topic ‘Material deforms too much: Explicit Dynamics’ is closed to new replies.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.Trending discussions
- Maximum Time Step
- Error 20211 (STR+211) while 2D impact analysis
- ls dyna has no solver
- LS-Dyna Prestressed
- Whereabouts of the LS-DYNA program manager
- License error : NO SUITABLE FEATURE FOUND
- Total Contact Force and Contact Pressure
- Contact not working in Ls-Dyna and Ls-Dyna ACT (WB)
- Element direction..
- TIED_CONTACT for Shell Elements – Gap between Shell-Shell and Shell-Solid
Top Rated Tags
© 2023 Copyright ANSYS, Inc. All rights reserved.Ansys does not support the usage of unauthorized Ansys software. Please visit www.ansys.com to obtain an official distribution.