May 24, 2022 at 4:51 pmTony6SubscriberI would like to plot contact load vs displacement so i have in the output controls turned on contact forces and inserted the result tracker for contact forces. End time is 0.06 seconds. I am using Ansys 18.2
How can i match the results for contact force and deformation so that the plots are equal in data point numbers like 150 points for each plot ?
May 25, 2022 at 12:42 pmChandra SekaranAnsys EmployeeThe 'contact force' under solution information has data for every time point and is not really stored in the results file. You should instead insert a 'contact probe' and then you will have the same number of points.
May 25, 2022 at 1:00 pmTony6SubscriberHow do i do that? Im in Explicit Dynamic Analysis and need the contact forces on a car front bumper impacting a wall
May 25, 2022 at 6:27 pmChris QuanAnsys EmployeeThe frequency of results tracker output under Solution Information is defined by Save Results Tracker Data On as well as Tracker Cycles in Output Controls.
In the picture as shown in your post, program will output results for results trackers at every cycle. If your model has run 100,000 cycles, the results trackers will have 100,000 data points.
You can increase the Tracker Cycles from 1 to 100, this will reduce the number of the results tracker data points to 1000.
Or, you can change the Save Result Tracker Data On from Cycles to Time and specify Tracker Time to output results tracker data.
If the End Time is 0.06 sec and 150 data points are required, the Tracker Time can be specified as 0.06/150 = 0.0004 sec.
May 25, 2022 at 7:28 pmTony6SubscriberSo i have changed the analysis settings as in the following image based on your comment. What about the output contact forces in the settings? I would like to plot contact force vs deformation so both axis need to have same nb of points. Using the result time and tracker time, this would mean 0.06/1000 = 6e-5 seconds. I am not sure however if the total deformation result would have 1000 points now or not and if that would slow things down massively. I also dont know if i should change output contact forces to also be based on time with 6e-5 seconds
May 26, 2022 at 5:41 pmChris QuanAnsys EmployeeThe Output Contact Force creates .cfr files that include contact force at all nodes that are in contacts. It is not related to the time history plot of contact force under Solution Information. Furthermore, these .cfr files cannot be processed directly inside Mechanical GUI at the current release.
If you open the .cfr files using a text editor, you will see the nodal number in the first line and the second line lists three contact forces in X, Y, Z directions. You may use spreadsheet to organize these data and re-arrange them to get two columns of data (cycle number and contact forces) for each contact node. Please be aware that not all nodes in your model are participated in the contact calculation. Only a small portion of the nodes are involved.
You can also look at the admodel.log in the MECH folder of your project to associate the cycle number with time. From these information, you can plot time history of contact force at the selected contact nodes.
If you want to plot the relation of contact force vs deformation, you can create a new results tracker of directional deformation under Solution Information. By doing this, you can make sure that both contact force and deformation have the same number of data points and are corresponding to the same time increment.
You need to be aware that the contact force results tracker is scope to a body or multiple bodies while deformation results tracker is scoped to a vertex or a node. So make sure you select the vertex/node strategically so the deformation from the results tracker can be properly related to the contact force results tracker.
May 27, 2022 at 7:50 amTony6Subscriberin reply to this: "You need to be aware that the contact force results tracker is scope to a body or multiple bodies while deformation results tracker is scoped to a vertex or a node. So make sure you select the vertex/node strategically so the deformation from the results tracker can be properly related to the contact force results tracker."
Is there a way to scope a deformation result tracker to a face just like contact force result tracker because i have eroded particles and i fear that vertex/ node might become eroded and mess up the results ?
May 31, 2022 at 3:57 pmChris QuanAnsys EmployeeDeformation results tracker has to be a node or a vertex.
If you are concerned about element erosion, you may consider to use body results tracker "Mass-Averaged Velocity" and scope the tracker to the same body as scoped by contact force results tracker.
Mass-Averaged Velocity is the total momentum of the scoped body divided by the mass of the body. The total momentum is the sum of the nodal mass times nodal velocity.
Once you have the velocity, you can export it with Contact Force to an Excel sheet and then integrate the velocity with time to get the Time History of Displacement. Then you can plot the Contact force and the Displacement together to get the Force-Displacement curve.
- You must be logged in to reply to this topic.
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.
- explicit dynamics
- Explicit dynamics ERRORS
- turning simulation
- getting zero maximum and minimum stress value in explicit analysis
- How do get Full values instead of just minimum and maximum ?
- How to figure out impact force in Explicit Dynamic Analysis
- Monte Carlo Simulation
- Running an explicit dynamics simulation on a composite plate
- Euler Domain Restricting Simulation
- Which analysis to use for dynamic and quasi-static compression of auxetic structures?
© 2023 Copyright ANSYS, Inc. All rights reserved.