February 24, 2018 at 9:18 pmozkantekin90Subscriber
I am trying to make a cutting analysis a simple analysis, whatever i select the values in animation i couldn't see plactic deformation, the cutting edge is just end its motion by the time contact the sheet metal i think i did miss something while i make mathematical model , Can somebody help me with this thaks
February 25, 2018 at 2:08 ampeteroznewmanSubscriber
I can try to help. What material model did you use for the part you want to cut? You must include a material failure model. Most materials in the Explicit Dynamics library include that. It will be easy to help you if you save an Archive of your model. That means close Mechanical, and in Workbench, File, Archive... and save a .wbpz file. You can attach that file to your post if it is < 120 MB. If the archive is too large, right click on Model and select Clear Generated Data, which will clear the mesh. Save the project, then do File, Archive... again and the file size will be smaller.
Attached is an ANSYS 18.2 archive of a very coarse and simple cutting model that runs in 15 minutes on my 4 core laptop.
February 25, 2018 at 10:33 amozkantekin90Subscriber
Thanks for your reply, I use Ansys 15.0 i think you can run it on your laptop. Also i will try to upgrade my sofware and open the project that you sent me
February 25, 2018 at 11:06 ampeteroznewmanSubscriber
You can download either 19.0 or 18.2 and be able to open that archive.
Here is a version with a flatter cutter.
February 25, 2018 at 11:29 amozkantekin90Subscriber
how can you determine the contact types actually i need to improve my analysis skills on Ansys especially explicit dynamics ?
February 25, 2018 at 11:55 ampeteroznewmanSubscriber
The model I attached only has Body Interaction and no additional Contact definitions.
February 25, 2018 at 1:07 pm
February 25, 2018 at 2:01 pmpeteroznewmanSubscriber
You have to click on the Solution, and Clear Generated Data, then Solve and wait. If you click on the Solution Information folder, you will see the progress. When it finishes, you will have results.
If I include results in the archive, the file size will be too large.
February 25, 2018 at 2:18 pmpeteroznewmanSubscriber
I opened your model, the first observation is that you have only 1 element through the thickness of the plate you want to cut and there is a gap between the plate and the tool.
You can see that in my model, I have 20 elements through the thickness of the part that is being cut and the tool is touching the plate.
If your goal is to make an animation of the cutting, it will be best if you take this geometry and scale it up 1000 times. The reason for this is that the solver calculates a time step based on the dimension of the smallest element. If you check the size of my plate, it is 1000 mm thick! But it solves in about 15 minutes. If my plate was 1 mm thick like your model, it would take 15,000 minutes or 250 hours or 10.4 days to solve.
February 25, 2018 at 2:26 pmozkantekin90Subscriber
i see i still have a lot of thing that i need to learn, thanks for your valuable informations, Also i will not use contacts like yours, in this case do i need to clamp the sheet on two side of the sheet ? thank you
February 25, 2018 at 2:37 pmpeteroznewmanSubscriber
Yes you have to have contact on both sides of the sheet, which you can see in my model. But I am not clamping. I picked the back edge of the plate and added a fixed support.
Also, instead of a displacement to move the tool, I used velocity with an equation that is number*time. That means that at t=0, v=0 and the velocity ramps up over time. Your ramped displacement creates a constant velocity so that the tool makes an impact with the plate which can cause the solution to fail due to energy error.
March 14, 2018 at 5:47 amozkantekin90Subscriber
Thanks for your help, Also i need to know how easy to cut a sheet as shearing (like scissoring) compared to usual cut as you have shown in the video above, how can i observe it on the ansys ?
March 14, 2018 at 11:04 am
April 16, 2020 at 1:55 amSaharPzdSubscriber
I am trying do a simulation with a similar concept where I am simulating a surgical staple being inserted into a block of bone. I used a lot of the techniques you mentioned above and I was able to simulate most of it except it seems like the staple does not cut into the bone but instead just deflects off of it. I had to create a new material on my own to simulate bone. The values I had were the tensile strength, yield strength, young's modulus, shear, poisson ratio, mass density, and compressive strength. Is there anything else I need to model failure?
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
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.
- How to calculate the residual stress on a coating by Vickers indentation?
- An Unknown error occurred during solution. Check the Solver Output…..
- Saving & sharing of Working project files in .wbpz format
- Solver Pivot Warning in Beam Element Model
- Understanding Force Convergence Solution Output
- whether have the difference between using contact and target bodies
- Colors and Mesh Display
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- Massive amount of memory (RAM) required for solve
- What is the difference between bonded contact region and fixed joint
© 2022 Copyright ANSYS, Inc. All rights reserved.