LS Dyna

How to get solution solved faster in 2D Explicit Dynamics

• Fernando Torres
Subscriber
Hi, currently I'm solving a 2d explicit dynamics problem with approx. 9k nodes and 9k elements with 1.6058e-8m mesh size on a server (32Gb Ram and 2 cores). Estimated Solution time is 1236 hrs (ofcrs not feasible). nAny way to solve it faster and get accurate results. Thanks.n
• peteroznewman
Subscriber
When you work with devices that have a dimension of 10 micrometers, and the element size is about 16 nanometers, Explicit Dynamics is not a good place to be.nThe reason is the minimum time step depends on the element characteristic length. The smaller the length, the shorter the maximum time step and the longer the solution will take to compute to the End Time.nIf you switch the solver to Transient Structural, then the element size is not a factor on how long the solver will take to solve to the end time.n
• Fernando Torres
Subscriber
Thanks Sir n
• Fernando Torres
Subscriber
I'll try to go transient...nBut what if I increase cores, and with a reasonable enough mesh, will this solve the problem little faster? ni.e. does solution time of a 2d explicit analysis depends on ram, cores or both (I'm asking for hardware here not cfl equation parameters)nThanks a lot.n
• peteroznewman
Subscriber
nFor any solver, if you go from 2 cores to 16 cores, you will reduce the solution time by less than a factor of 8.nIf you double the computer clock speed from 2 GHz to 4 GHz, you will reduced the solution time by a factor of 2.nImplicit solvers need more RAM, but if the problem size fit in the existing RAM, increasing the amount of RAM will have no effect.nThe maximum time step size is set by the minimum element length for Explicit, while for Implicit solvers, it is set by the highest natural frequency of interest in the structure. The ratio of the maximum time step of Implicit/Explicit for your nano-scale elements might be a factor on the order of 1000.n
• Fernando Torres
Subscriber
Thanks shifted the model from explicit to transient but the tool is getting into the workpiece without cutting anything i.e. tool just moves inside workpiece without cutting the material. Tried to setup the contacts manually but it didn't work. What could be the issue?nThanks. n
• peteroznewman
Subscriber
• Fernando Torres
Subscriber
Great Article but I have issues in material removal (chip formation). When I run the same experiment in explicit dynamics, cutting is shown with proper chip formation, BUT ONCE I shift the model to TRANSIENT structural, there is no cutting like shown below (tool moves freely into the material without cutting). I know this is a childish question but it is what it is.nthanks for your help.nn
• peteroznewman
Subscriber
In Explicit Dynamics, element removal from the model is automatic.nIn Transient Dynamics, element removal is not automatic. The article you enjoyed showed you how to do that with a script. This is more work for the user, but may end up taking less time compared with weeks of solution time in Explicit Dynamics.nGood Luck!n
• Fernando Torres
Subscriber
Thanks Sir Array, I'll check that out in more detail. Parallel processing is only available for 3d models says the AUTODYN Solver for my 2d explicit dynamics problem. I know you have stated about the hardware on top of this page but I wonder if that is still valid for AUTODYN 2D Explicit Analysis.nThanks. n
• peteroznewman
Subscriber
AUTODYN 2D has no parallel processing, so one core is all you can use.n
• Fernando Torres
Subscriber
what if I shift this material cutting simulation to LS DYNA from AUTODYN.n1. For 2d explicit analysis, would LS DYNA use multiple cores? (solution time compared with autodyn?)n2. Would results be same or different than using AUTODYN?nThanks.n
• peteroznewman
Subscriber
I don't know about parallel processing in LS-DYNA, I don't have a license.nThe results would be very similar.n
• Fernando Torres
Subscriber
Thanks I set the end time to 0.01, but the solver finished the solution for time 2.4E-4. i.e in video animation of result, the animation (and solution) stops after 2.4E-4s. Thanks.n
• peteroznewman
Subscriber
Are you talking about the LS-DYNA solver or the AUTODYN solver?nAn error occurred during the solution that caused it to stop before the end time. These solvers track various energy levels and if a specific type of energy has a threshold to maintain the quality of the solution, the solver will stop when that threshold is crossed.n
• Fernando Torres
Subscriber
Sir,using AUTODYNnSolver hasn't shown me any error or warning upon completion. It was quite long simulation, I used to pause, then save and then resume from cycle. But it did not show me any warnings or errors in messages. n
• peteroznewman
Subscriber
nThe solver may not show you an error, you might have to go into the folder structure and look for errors in one of the files. I don't know which file or folder that is, but I have seen replies in other discussions in the Explicit Dynamics forum that say which file and folder to check. n
• Missy Ji
Ansys Employee
If you wish to use parallel with Ansys Explicit, you may extrude your 2D model one element side in the third direction to make it 3D, then you can use Parallel.n
• peteroznewman
Subscriber
Please describe the boundary conditions that must be applied to the nodes on the offset plane.n
• Fernando Torres
Subscriber
Hi Array , I was thinking to shift that 2d material cutting simulation to 3d in explicit dynamics. Please elaborate ALL the changes I should make as you have stated  describe the boundary conditions that must be applied to the nodes on the offset plane, do you mean those surface displacement constraints or something else? Please let me know any other important points (conditions) too (if we have)nThanks as always!n
• peteroznewman
Subscriber
nI was asking to describe the boundary conditions that must be applied to the nodes on the offset plane.nIn a 2D model, the Z DOF at each node does not exist. Once you have a 3D model, now you have a node on the Z=0 plane that has a Z DOF. I expect that node must have a boundary condition of Z=0 applied. But what about the nodes on the Z=1 plane, where the 2D mesh was extruded to become 3D with a unit depth in the Z direction. If the nodes with the coordinate Z=1 are assigned a displacement boundary condition of Z=0, that would create a Plane Strain condition. But if the nodes with the coordinate Z=1 have no displacement boundary condition, that would create a Plane Stress condition.nAre you analyzing a Plane Stress or a Plane Strain condition?.
• Fernando Torres
Subscriber
sorry for my ignorance. I should have stated that. It's plane strain case. And please let me know how to assign these displacement bc's in 3d. What I used to do is to select a side surface of 3d model and constraint it by giving z=0. Is this condition applies to the surface only or on whole 3d model (in this case a simple rectangular workpiece).nThanks.n
• peteroznewman
Subscriber
The mesh must have linear elements so there is no midside node. In that case, every node is on either Z=0 or Z=1 planes. That means the entire body (or two faces) can have a Displacement BC of Z=0 leaving X and Y Free. Some nodes will need to constrain X and Y to be 0 for a Fixed Support and it will be important to capture nodes on both the Z=0 plane and the Z=1 plane for those Fixed Supports. This is simply a side face of the extrusion.n
• Fernando Torres
Subscriber
Hi Sir Array,paper states the fracture strain of silicon is set as 0.01. I have created a material model for Silicon but where to put this fracture strain value in my ansys wb material model? Thanks.n
• peteroznewman
Subscriber
nIn ANSYS Help, Mechancial APDL, there is the Material Reference section. In there are many material models. Some of them include Failure Criteria. You will need to do some research and find a material model suitable for brittle fracture. I can't help you more on this. Perhaps someone from ANSYS can answer this question.n
• Fernando Torres
Subscriber
just a friendly request. You should be among the speakers too at ANSYS LEVEL UP ? Let's vote for Sir Peter guys ?.
• peteroznewman
Subscriber
Ha! Maybe next time n
• vibrachid
Subscriber
how to do Strain modal analysis on ansys Workbench and how to find strain mode shape, please answer, i dont know how to do new discussion on this forum, i am new.n
• peteroznewman
Subscriber
Modal questions belong in the Structures category, not the Explicit Dynamics category.nGo to this page: https://forum.ansys.com/categories/structuresnClick on the yellow button Ask a Question.nGive the discussion a title and put the question in the box.n