March 23, 2018 at 1:57 pmThelibanSubscriber
I am the new learner to Ansys, doing my Masters in Engineering Design field. I am doing the VM250 to get some knowledge in Non- Linear Analysis. While solving the problem, I am getting the error as shown in the figure. By decoding the APDL code, I did the procedures and applied the BC. But continuously I get the error message. What should I do to have the converge solutions? Please help me to decode the APDL code.
March 24, 2018 at 3:17 ampeteroznewmanSubscriber
I would expect to see the fixed support on the underside of the bottom block (the -Y face). I can't see what kind of connection you have between the two blocks. Please use File, Archive... in Workbench to create a .wbpz file and attach that file to your reply.
March 25, 2018 at 7:23 amThelibanSubscriber
With this reply, I attached the Gasket_VM250. Thanks for your support. Please find the attachment
March 25, 2018 at 12:33 pmpeteroznewmanSubscriber
I made a change in DesignModeler, picking the three bodies and right clicking to select Form New Part. That results in the two shared faces sharing nodes, eliminating the need to use bonded contact in the model.
The changes to the model were in the Supports, you see there is now three Displacement supports, one for each axis set to zero. I made a smaller mesh since the result is a uniform pressure. I changed the analysis settings to do 20 substeps on as the pressure increases and 20 substeps as the pressure decreases in load step 2.
Attached ANSYS 19.0 archive.
March 25, 2018 at 2:05 pmThelibanSubscriber
Thanks for your support, I somewhat understood where I went wrong!
An inference from your modifications:
1) The contact bodies, make inconvenience in the model.
2) Understood the boundary conditions
1) In this model, you arrest the face of the Gasket also, is it physically possible? (While compression, it tends to squeeze out right?)
2) Through my coursework, I can visualize the Newton Raphson Method, but I am unable to understand WHAT IS SUB-STEPS? Where Can I learn it.
March 25, 2018 at 5:10 pmpeteroznewmanSubscriber
Gasket Material and Squeeze Out
A gasket material model and associated element is different from solid continuum materials and elements and is made for the special use-case of gasket compression. There is only ever one element through the thickness of the gasket solid and there is no midside node. The material model has only one input, which is the closure distance. The gasket material is not designed to model the "squeeze out" of excess material.
The nodes on the face of the block that are held by the displacement BC are shared by the gasket. The gasket element has no midside node, so you could say the gasket is attached to the block and is not controlled by the displacement BC.
If you want to model the "squeeze out" effect of some hyperelastic solid, you can use a hyperelastic material model, put many elements through the thickness and see that effect.
If you did hyperelastic material and many elements, the displacement BCs on the X and Z faces represent a symmetry BC so you could imagine that this model represents 1/4 of the full size block and hyperelastic material would squeeze out on the two free sides. If you did not want to represent a 1/4 symmetry model, you would have to change the support on the bottom to a fixed support, then you could see the material squeeze out on all four sides and you could also put a shear force on the top block and see side movement.
A gasket material model has no ability to support shear forces so you could not have just a fixed support on the bottom block, you would also need some way to support the X and Z motion of the top block.
Newton-Raphson Method and Substeps
When you have a load step with no substeps, the solver uses Newton-Raphson (NR) searching to find equilibrium for the system of equations. This is good if the solver is successful in its iterative search and if you don't want a plot of a result quantity along the way to the full load. Sometimes the solver fails to find equilibrium or the user want to see the history of a result quantity along the way to full load. In either of those cases, substeps are required. If a user requests 5 substeps, the solver takes the full load and divides it by 5 and applies 1/5 of the full load and begins NR searching for equilibrium. When it finds it, the solver writes out the results, then increments the load by 1/5 and begins searching for the next equilibrium starting with the last equilibrium. If the solver fails to find equilibrium at that increment, it will automatically bisect the load and apply a 1/10 increment instead and try again to find equilibrium.
- 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
- Colors and Mesh Display
- 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.
- What is the difference between bonded contact region and fixed joint
- Massive amount of memory (RAM) required for solve
© 2022 Copyright ANSYS, Inc. All rights reserved.