September 25, 2022 at 11:22 amup1057819SubscriberHello everyone,I am running a large deflection analysis with mechanical Apdl ( NLGEOM, ON). As soon as the loading initiates the solution collapses and I get an error message that a particular element has exceeded distortion. When I check the elements ( SHELL181 Quad node element) deformation it changes from a rectangular shape to a completely irregular one.I have tried to reduce the time step and increase the number of substeps but nothing worked.Why this error occurs?
September 25, 2022 at 12:03 pmpeteroznewmanSubscriber
Does it solve with NLGEOM turned off?
You might have a mistake in the model. Check the magnitude of the loads and check the values of the material properties. Check the thickness property of the shell element. Reduce the load by a factor of 10^3 and try that. Reduce the load by a factor of 10^6 and try that.
September 25, 2022 at 2:30 pmup1057819Subscriber
Yes, it solves when the NLGEOM is off. I tried that but didn't work.If the problem is related to the connection of the elements how could I solve for that?
September 25, 2022 at 6:38 pmpeteroznewmanSubscriber
If it solves as a linear solution, it is unlikely to be an issue with element connectivity.
Please reply with images of the mesh, load and boundary conditions.
September 25, 2022 at 10:12 pmup1057819Subscriber
Here is an image of the model. The seen are restrained in ux,uy, and the first node of the row in ux,uy,uz (only one node is restrained in all three degrees of freedom). The whole structure is meshed witth an element size 0.5 ( esize=0.5). The load is applied in a form of a displacement( seen in the second picture) firstly the nodes are given a displacement equal to 10mm in the uy direction(vertical) and then in the -ux equal to 0.5. this is done in order to simulate shear stress in the core.The model is connected with AOVLAP command. Hope this is enough for you.
September 26, 2022 at 2:34 ampeteroznewmanSubscriber
What is the goal or purpose of this analysis? What is it that you want the results to tell you? Are you looking to calculate the shear modulus of the core in a specific direction?
In the graphics, I can see a row of ux, uy constraints on one edge of the top facesheet and I understand the corner node is constrained in x,y, and z. Having one straight line of nodes like that creates a hinge.
In the second image, it's not clear which nodes are given a displacement. I also don't know how thick is the core compared with the 10 mm displacement you mentioned.
I recommend switching to applied forces and don't use any applied displacements.
September 26, 2022 at 8:19 amup1057819Subscriber
The purpose of the analysis is to examine some shear stresses. The 10 mm is the same as the thick of the core. I cannot use force because I don't know the magnitude
September 26, 2022 at 3:22 pmpeteroznewmanSubscriber
A 10 mm thick displacement of the bottom facesheet relative to the top facesheet with a 10 mm thick core is an absurdly large amount. What is core material and wall thickness? What is the facesheet material and thickness?
Is the core manufactured by corrigating and bonding two thin sheets together? That creates a double thick wall in one direction. Did you do that in your model?
Here is the test apparatus from ASTM C273 -11 Standard Test Method for Shear Properties of Sandwich Core Material.
If you don't want to switch to Force, I recommend that you select the row of nodes on the bottom facesheet at the opposite end of the sandwich from the row that has the x,y constraints on the top face sheet. Use a Displacement of Y=0 to prevent rotation about the first edge. Is the sample 50 mm long? In that case, 1% strain would be 0.5 mm. Use a Displacement of X= -0.5 mm to those bottom edge nodes to put the facesheets into tension at each end. Use 100 initial and minimum substeps, 1000 substeps maximum, in the solution.
- 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.
- Limitations to Student License?
- Missing Analysis Systems from toolbox
- ANSYS License Manager Error
- Not seeing any items in the ANSYS Workbench toolbox?
- “An error occurred while starting the solver module.” – Maybe licence problem?
- FLUENT application Failed to start
- Please recommend the configuration of the computer workstation
- No license available at this time
- I am using MacBook Pro with M1chip, how can I install or any other ways to use Ansys ?
- Problem with ANSYS 18.2 SpaceClaim
© 2022 Copyright ANSYS, Inc. All rights reserved.