May 25, 2022 at 5:20 amidreesSubscriberHello everyone!
I have two questions regarding to this simulation. The bending plate thickness, width, length = 2, 2, 150. Vee shape bending die with 90 degree angle. Transient structural modal. Aluminum alloy 7075-0
How to avoid bending at the two edges of the vee die as shown in the attached file 1. Even I tried to change the radius of the fillet and remove the fillet but still no improvement. When I increase the workpiece thickness and width then this does not happen and the bending goes smooth as natural.
After the simulation is completed and the plate is fully bended there is still I can see an obious gap between the punch and plate and plate and die. Even this does not happen when I increase the thickness and width of the sheet. As shown in the second attached screenshot.
May 25, 2022 at 6:33 pmChris QuanAnsys EmployeeAre you using Transient Structural system?
If yes, are the contact between the plate & die frictional? Do you observe that the plate is stick to the die at the die edge?
If yes, you can insert a Contact Tool under Solution to plot Contact Status & Frictional Stress of the contact. If the contact shows "stick" status or has very large frictional stress in the die edge, you need to insert a MAPDL command to limit the maximum frictional stress. This will allow the plate sliding on the die.
May 26, 2022 at 7:13 pmpeteroznewmanSubscriberThe die has moved down in 0.7 milliseconds. Inertial forces at the ends of the plate have caused the bending. If you don't want the ends to bend, move the die down slowly, like 1000 times slower, such as 0.7 seconds.
May 30, 2022 at 4:27 amidreesSubscriberHello sir!
To move die means apply displacement to the die?
But I applied force to the punch and fixed support to the die. By keeping die at a fixed place I also wanna observe the springback in the workpiece.
May 30, 2022 at 4:30 amidreesSubscriberThe main problem is why there so much gap between punch, workpiece and die after fully bended, even I did correct geometric calculations. Such as die opening, workpiece length, Punch width etc
May 30, 2022 at 12:02 pmpeteroznewmanSubscriberThe punch has moved down in 0.7 milliseconds. Inertial forces at the ends of the plate have caused the bending. If you don't want the ends to bend, move the punch down slowly, like 1000 times slower, such as 0.7 seconds.
If you want to apply a force, not a displacement to the punch, add a very large mass to the punch to slow it down.
May 30, 2022 at 1:17 pmidreesSubscriberSir, If I increase the punch length, width and thickness, does it help to increase the mass of the punch?
May 30, 2022 at 8:26 pmpeteroznewmanSubscriberThe simplest way to increase mass is to go into Engineering Data and edit the Density of the punch material. Try adding three zeros. While that may slow down the velocity of the punch, it will create a large amount of kinetic energy that will squash the plate against the die, so it may not be the best idea.
A better way to slow down the velocity is to add a spring/damper from the punch to ground along the punch direction. Set the spring rate to 0 but put in a large number for the damping constant. A damper creates an opposing force proportional to the velocity. Keep increasing the damping constant by a factor of 1000 until you see the punch slow down. The benefit of the damper is that as the punch begins to push the plate against the die and the velocity is slowed by contact, the force in the damper will drop to zero.
- 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.