April 1, 2020 at 8:15 ampedrocarneiroSubscriber
April 1, 2020 at 11:22 ampeteroznewmanSubscriber
Why do you want to turn off bending stiffness?
Please reply and insert an image of the geometry, mesh, loads and supports and an image of the Force Convergence Plot under the Solution Information folder.
Is there a plane of symmetry for the geometry, loads and supports that would cut the model size in half?
Under Mesh Controls, set the Element Order to Linear.
Under Analysis Settings, turn on Auto Time Stepping, with Initial and Minimum Substeps to 100, Maximum to 200.
Turn on Large Deflection.
Turn on Stabilization.
Add a Command Object to the Model: NEQIT,100
I assume the load creates some tension in the membrane. Try using the INISTATE command to apply some initial stress (or strain) to the elements before the solver starts. This requires a Command Object, so try the steps above before you resort to this.
April 1, 2020 at 12:08 pmpedrocarneiroSubscriber
Thanks for your answer. I will try to explain the context of the simulation.
I think that for correctly simulate a membrane it is needed to turn off the bending stiffness because it is suppose that the stress is constant along the thickness and in the specific case that I want to simulate the thickness is very small compared with the other dimensions of the membrane. However, if I try this i.e. keyopt(1)=1, the deformation is equal to zero if I apply a pressure perpendicular to the membrane so I suppose that the most correct approach is try to keep the default value of keyopt(1)=0 but I am not sure.
I pretend to validate an analytical expression described in literature (image in annex) for the maximum stress and the deflection in the center of the membrane.
In the analyze setting, in the stabilization only appears off, constant and reduce. What is suppose I select?
In annex are also the mesh and the loads.
Thanks for all.
April 1, 2020 at 1:51 pmpeteroznewmanSubscriber
Definitely use 1/4 symmetry.
What does the Force Convergence plot look like?
April 1, 2020 at 3:06 pm
April 1, 2020 at 3:45 pmpeteroznewmanSubscriber
This model may require overriding the Program Controlled Nonlinear Controls under Analysis Settings to converge. The defaults are good for 99.9% of the models I have run, but for unusual cases like this one, it may need one or more of the convergence criteria to be relaxed. Please use File > Archive to create a .wbpz file and attach that after you reply with the version of ANSYS you are using.
April 1, 2020 at 4:18 pmpedrocarneiroSubscriber
I am using 18.2.
April 1, 2020 at 4:24 pmErik KostsonAnsys Employee
These type of problems are very hard to get to converge. Peter has given some very good tips.
On top of that it seems that the material Young's modulus is quite low, so I would start with a lower pressure and see that works (say 10Pa or even 1 Pa).
Furthermore one might need:
Under Analysis Settings, turn on Auto Time Stepping, with Initial and Minimum Substeps to 200, Maximum to 2000.
This will allow the membrane to build up out of plane stiffness gradually - very important.
April 1, 2020 at 4:52 pmpedrocarneiroSubscriber
Thans for the sugestions.
It seems not work. I only achives a sucefful test if i put the pressure equal to 0.001 and with keyopt(1)=1 consedering bending and menbrane stifness.
April 1, 2020 at 5:22 pmpeteroznewmanSubscriber
Is the archive file the 1/4 geometry or the full model?
April 1, 2020 at 6:53 pm
April 2, 2020 at 4:59 pmpeteroznewmanSubscriber
Attached is an ANSYS 18.2 archive that has the proper symmetry conditions for quarter symmetry.
Most of these analytical equations are intended for deformations less than the thickness of the material. When this is the case, a linear solution in ANSYS is almost identical to a nonlinear solution. When the load creates deformation that is many times larger than the thickness, the nonlinear solution will give a very different result to a linear solution.
In the attached archive, I have your original rectangle size solved with a Linear solution that has a 2.3 inch deformation, while the Nonlinear solution has a 0.175 inch deformation.
I include the 10x24 inch example you provided and I also did a 12x24 inch version because I found a reference with a different analytical equation.
April 2, 2020 at 6:27 pmpedrocarneiroSubscriber
thanks for your attentaion and files. i still have some questions.
Why did you only considered 1 psi of pressure in the case of 10*24 inch instead of 15 of the example?
Why did you supress the commands that assings the elements?
Once again thanks for your time.
April 2, 2020 at 6:41 pmpeteroznewmanSubscriber
The thickness is 0.1 inch, and at 1 psi, the deformation is already more than the thickness. If you enter 15 psi in the Nonlinear solution the deformation is 0.155 inch while the Linear solution it is 0.423 inch so they bracket the 0.222 inch that the analytical formula produces.
I suppressed the keyop to set membrane stiffness only because that makes the nodes have no rotational DOF and it is no longer possible to clamp the edges, they become simply supported. But most important, the result was zero deformation.
April 3, 2020 at 6:51 pmpedrocarneiroSubscriber
Thanks for the explication.
Basically, there is no a clear/only solution in that cases. Being the experimental validation the the most adequate test.
- You must be logged in to reply to this topic.
Simulation World 2022
Earth Rescue – An Ansys Online Series
- 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.