

November 26, 2019 at 9:40 pmThomsen93Subscriber
Hello Dear Sir,
We need to calculate of bending force and sheet metal's elastic deformation that dependent on top tool's displacement on the y direction.
The thickness of sheet metal is 8mm. Also the tools geometry has been defined on the model.
We have assumed nonlinearities that multi linear plastic deformation for sheet metal. We increased young modulus of top and bottom tools for behave like rigid body. And we need to see weak springs effect that occurs after the bending process on the sheet.
I used size mesh for contact surfaces and had created 2 steps in analys settings. In the first step top tool move 15 mm on y direction and in 2th step top tool has to get retain position that it started.
We have encountered some errors about weakspring and solver suddenly stopped.
Bottom tool is fixed from bot surface, Sheet metal standing on the bot tool and top tool bending it while moving 15mm for y direction.
The given hand would be appreciated deeply from our youth spirit
You can increase top and bottom tool's young's modulus multiplying with 10000.
Sheet Metal Multilinear Isotropic Hardening Properties.
MPa STRAIN (Young's Modulus 72450MPa Poisson Ration: 0,33)
250 0
269,1 0,003714
307,05 0,01172
331,2 0,02052
348,45 0,03131
358,8 0,04047
376,05 0,06199
386,4 0,07985
396,75 0,10254
414 0,15427

November 27, 2019 at 1:21 ampeteroznewmanSubscriber
Hello Thomsen,
One defect in your model is you need many elements, at least 8, through the thickness of the sheet. One element is impossible to compute.
I recommend you convert this to a 2D Plane Strain model. To do that, you need surfaces in the XY plane (Z=0). You must also set the Properties of the Geometry cell in Workbench to 2D before you open the Model in Mechanical.
At this amount of bending, the Total Strain is over 30% while the plasticity model you provided only goes up to 15%
What is the Elongation at Break for the Aluminum alloy? Perhaps it has already cracked by this point.

November 27, 2019 at 9:32 amThomsen93SubscriberHello again Could you update your properties like this?, I have increased plastic linear strain on materials so we don't want to see any cracks on material. The root cause of this fault we have taken these vaules from analys example.
Can you share your wpz file? Additionally we need to see minimum bending force that get this form on the sheet Metal. Does it consist to use 2d simplification when we re look for force and plastic deformation?
Sheet Metal Multilinear Isotropic Hardening Properties.
MPa STRAIN (Young's Modulus 72450MPa Poisson Ration: 0,33)
250     0
269,1     0,003714
307,05     0,01172
331,2     0,02052
348,45     0,03131
358,8     0,1047
376,05     0,1519
386,4     0,2185
396,75     0,2725
414     0,4042 
November 27, 2019 at 12:06 pmpeteroznewmanSubscriber
What version of ANSYS are you using? I did my example in 2019 R3 and have attached the archive. You can't open it if you are on an older version.
You can update the material and run the model. Is the data for plasticity in terms of Engineering Stress and Strain or True Stress and True Strain? It must be in the latter. Here is an example of the conversion process.
A plane strain model can compute with a plasticity material and has results per unit depth, so for a model in mm, the force is per mm of depth.

November 27, 2019 at 5:19 pmThomsen93Subscriber
Dear sir,
I' much preciated for your kindness but when I opened your wbpz file, model wanted to upload itself. When I did this, your meshes style, restrains all of were gone.

November 27, 2019 at 6:50 pmpeteroznewmanSubscriber
Not sure what you are seeing. I just downloaded and opened the attached archive. It has a Fixed Support, a Displacement and two Frictional Contacts. The results are not included. You have to clear generated data on the Solution branch and solve again.

November 28, 2019 at 7:17 pmThomsen93SubscriberHello Peter How s going on?
I m trying to solve it, while using Web digitiliazer to get plastic multi linear curves from st44 graph that taken from instron machine.
I don't like to write large paragraph, I will share my result on upcoming days.
Regards. 
December 1, 2019 at 5:32 pm

December 2, 2019 at 12:39 ampeteroznewmanSubscriber
NEQIT,100 tells the solver to keep iterating to search for convergence for up to 100 iterations. The default is 26 iterations. When convergence is not found, a bisection occurs, which means the load increment is cut in half and the solver tries to converge again. Sometimes, when watching the force convergence plot that is updated while the solution is being computed, you can see the two curves, force convergence and force criteria, converging and they just need a few more iterations for the curves to cross, but it is getting close to 26 iterations since the last convergence, that is when you want NEQIT,100.

 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.
Ansys Blog
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.
 Solver Pivot Warning in Beam Element Model
 Saving & sharing of Working project files in .wbpz format
 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
 User manual
 The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
 whether have the difference between using contact and target bodies
 material damping and modal analysis
 Colors and Mesh Display

5340

3313

2471

1308

1016
© 2023 Copyright ANSYS, Inc. All rights reserved.