TAGGED: ansys-mechanical, ansys-workbench, workbench
June 8, 2021 at 4:44 pmRaghu79SubscriberJune 8, 2021 at 9:49 pmpeteroznewmanSubscriberPlease show all the information you have on the epoxy resin.
June 9, 2021 at 7:50 amRaghu79SubscriberHi Peter Thanks for responding. I have used the built-in material in Ansys Engineering Data under Composite Materials for the epoxy resin.
My queries are:
1) How can I make Ansys understand that the epoxy resin is the adhesive bond between the concrete and steel? For now, I have set a Bonded contact between the epoxy face and concrete face and a No Separation contact between the steel face and epoxy face as I would want the steel beam to slide downwards (displacement) until failure as the load is applied gradually.
2) Is probing a force reaction with displacement as the boundary condition the right method to obtain the displacement values of the steel beam? These values are useful to me to plot the force-displacement curves.
Your reply is very much appreciated. Thanks in advance
June 12, 2021 at 4:08 amRaghu79SubscriberI would appreciate your advice on my queries, many thanks!
June 12, 2021 at 1:04 pmpeteroznewmanSubscriberThanks for using because that makes it easy to find your reply.
DESIGN FOR STRENGTH MODEL
A simple model would consist of the three solids: concrete, epoxy and steel, having Shared Topology applied so that no bonded contact is required. This is easily done in SpaceClaim if the three solids are in one component, just go to the Workbench tab and click the Share button. Before doing that, on the Design tab, click Split Solid and split the steel at the end of the epoxy, and then repeat to split the concrete at the end of the epoxy. That will allow the bodies to continue to have clean hex meshing applied.
In Mechanical, use Mesh Controls such as Sweep to ensure there are at least four elements through the thickness of the epoxy. I suggest using the fixed support only on the bottom face of the concrete so that there is no boundary condition on an edge that the epoxy can touch.
Solve the model and plot the applied Force vs the Von Mises Equivalent Stress. Look up the Force that just exceeds the value of Tensile Yield Strength in the Equivalent Stress column. That is one measure of the failure load. For many design tasks, that is all that is needed since the design goal is to size the area of adhesive so that the Equivalent Stress stays below the Tensile Yield Strength by some factor of safety at the maximum load expected during the product lifetime. This is the most common type of analysis, though I have used the Tensile Ultimate Strength as the threshold and the Max Principal Stress as the metric to evaluate the failure load.
You can plot the force vs deformation from this model and you will find it is an almost straight line. That is because the definition of Yield Strength is when the material stress deviates just 2% from a straight line.
SIMULATE TOTAL SHEAR FAILURE MODEL
Unfortunately, what you want is to simulate the Force vs Deformation plot that the testing machine plots during the total destruction of the joint. That is because the joint continues to be present for loads much higher than the point when the yield strength of the epoxy is reached. This is a much more difficult model to build and to tune up to match experimental data. It requires a lot more material data about the Epoxy than you have. There is a whole chapter in the ANSYS help guide on this. Section 4.11 of Mechanical APDL Theory Manual (R2019 thru R2021) covers how the Cohesive Zone Model (CZM) works in both interface elements and contact elements.
June 15, 2021 at 4:36 pmRaghu79SubscriberThanks for your reply I am working on to find a way to simulate the total shear failure model. I read through the ANSYS help guide and found that the Cohesive Zone Model (CZM) could be the solution I need. Based on my understanding, I need to perform an analysis with Contact Debonding. I have basic queries that I would like to ask and I hope that you or there is someone that will be able to help me as I am still new to the software. My apologies if the questions are silly, but I would appreciate any help.
1) I would like to know how to 'use' commands such as the picture uploaded below in workbench? Is this automatically generated based on my inputs or do I have to manually type it in? I believe this applies to other examples such as SOLID185,186 and so on.
2) You have stated that I require a lot more material data about the Epoxy that i have. Extracted from the Cohesive Zone category in Engineering Data, are these the data you mentioned about? If yes, unfortunately, I do not have the exact values and will be forced to make assumptions to validate the push-out test. Please suggest on what can I do to make this happen.
I would sincerely appreciate your reply on this as I will be able to move forward. It would also be great if this discussion could be left open if more concerns or questions arise. Thanks in advance.
June 16, 2021 at 12:52 ampeteroznewmanSubscriberHere is a current discussion: https://forum.ansys.com/index.php?p=/discussion/27969/non-convergence-of-the-model#latest
The link below shows 151 search results for CZM on this site:
The link below shows all the YouTube videos on CZM.
I hope you find answers to your questions. There is a lot to learn and I don't have all the answers.
June 16, 2021 at 7:35 amRaghu79Subscriber
Appreciate your response. I will refer to the links you have shared on CZM. I hope my first question above could be answered in simple terms as I am unable to understand how the commands are used in workbench. Once again, thanks for your time and effort.
June 16, 2021 at 12:43 pmpeteroznewmanSubscriber@raghu79 How to use APDL commands in Mechanical.
June 26, 2021 at 7:44 amRaghu79Subscriber
I have tried my simulation incorporating CZM but I am still unable to plot the destruction of the adhesive bond. Are there any other methods to your knowledge that I could apply to succeed in this simulation? Like using Explicit Dynamics for instance. Your help is very much appreciated to complete my work, thanks in advance.
June 26, 2021 at 4:19 pmpeteroznewmanSubscriberWhat do you mean "unable to plot the destruction of the adhesive bond"?
Do you mean the solution would not converge?
In that case, you need to do some work to get convergence.
The simplest change is to replace the Force load with a Displacement load, and instead of plotting deformation, you plot the reaction force for the applied displacement.
After that, you need to change the Analysis Settings and set the Minimum number of substeps to a number 100.
If you still haven't managed to converge, there are more advanced techniques.
Yes, you could replace the implicit model with an explicit model, but then you need a material model for the epoxy.
June 26, 2021 at 5:00 pmRaghu79SubscriberThanks for the idea. I have plot the reaction force for the applied displacement and I believe this is a decent convergence. But, I have two concerns on this outcome that I hope could be resolved with your knowledge:
1) The forces that are probed seem to be unrealistic and what could possibly be the way to control the output force as I have tried to reduce the displacement load but see no changes.
2) Will I possibly be able to observe the total shear failure of the adhesive bond in Static Structural? I have attached an example image of a similar experiment, but using a different software. It is best if I could simulate as close as these results.
June 26, 2021 at 5:19 pmpeteroznewmanSubscriberTo reduce the reaction force, you need to reduce the properties of the CZM model.
February 3, 2022 at 7:57 pmKonnaSubscriberIs there any simulation/video on how to perform a push out test on Ansys?
February 3, 2022 at 8:49 pmpeteroznewmanSubscriberPlease start a New Discussion. In that discussion, include as much information about your project as you can. The geometry, the supports, the loads, the material data you have available. Include some images of the geometry.
Viewing 14 reply threads
Ansys Innovation Space
- 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.Trending discussions
- Saving & sharing of Working project files in .wbpz format
- Solver Pivot Warning in Beam Element Model
- Understanding Force Convergence Solution Output
- An Unknown error occurred during solution. Check the Solver Output…..
- What is the difference between bonded contact region and fixed joint
- whether have the difference between using contact and target bodies
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- User manual
- Colors and Mesh Display
- material damping and modal analysis
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.