March 6, 2018 at 10:28 pmFabricio.UrquhartSubscriber
First of all, I would like to know if it is possible in workbench, define the element PLANE182. Because in my problem, I have only one plate with loads in the plan. Like the picture below.
Is it possible to define in the workbench?Because with apdl, I know that it is possible.
Thank you, very much.
March 7, 2018 at 6:24 pmpeteroznewmanSubscriber
You can create PLANE182 elements in Mechanical Workbench.
Step 1. Drag a Static Structural system into the project page, click on Geometry and set the Analysis Type to 2D.
You must do this first!
Step 2. Create a surface in the X-Y plane using either SpaceClaim or DesignModeler.
Step 3. Open Mechanical, your model will be a Plane Stress model by default with quadratic elements.
Click on Mesh and in the Details, change the Element Order to Linear,
since the PLANE182 element is a 4 node quad element and is therefore a linear shape function.
Attached is an ANSYS 18.2 archive that you can reference along with the Input file to Mechanical APDL that shows the element type.
Why do you want a linear element instead of a quadratic element?
March 8, 2018 at 4:13 pmFabricio.UrquhartSubscriber
Thank you, you helped me a lot.
I will compare a plate compressed like the model in the picture with a model using 2d contact between two plates (by the edges). I will apply the same load and the results maybe similar, but I am waiting for a contact pressure. Today, I will do this model and send here if I have doubt. Thank you, very much.
March 14, 2018 at 11:53 pm
March 15, 2018 at 1:37 ampeteroznewmanSubscriber
Warning messages like these are often of no consequence to the solution.
If your solution has small deformations, you could turn off Large Deflection under Analysis Settings, solve and get the same results without the warning.
An example of a support that can become invalid under large deformation is a compression only support, which is a quick and easy way to add frictionless contact to a model without manually creating another face. ANSYS automatically makes a copy of a selected face of the model to become a fixed rigid surface. The selected face of the model has frictionless contact elements to the invisible rigid surface. However, if the model has a significant lateral motion on the rigid surface, nodes can "fall off" the surface and the support becomes "invalid" because the user probably did not want that to happen.
The second warning is very common and very often understood as acceptable. If the lower body has contact elements on the top edge, and a displacement BC on the left or right side, the node in the corner has both, which generates the warning. It is possible (but unnecessary) to eliminate the warning by applying the displacement BC to all the nodes on the edge except for the corner node, which eliminates it from having two masters. In fact, there is no conflict in what the solution is asking that node to do, it can do both.
It is possible to add incompatible BCs to a model, and that is when the warning should be heeded and corrective action taken. For example if a Fixed support is added to the bottom face, and a displacement BC added to an adjacent face, nodes on the common edge can't both move and not move at the same time.
- 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.
- ANSYS Workbench Measuring within Design
- How to resolve Mesh Failure
- check element type
- The mesh file exporter could not resolve cyclic dependencies in overlapping contact regions error
- Meshing Error
- Error in meshing
- Conformal vs Non-Conformal Mesh
- Ansys 19.0 – will not create mesh
- Dealing with inflation layers around sharp corners in Ansys workbench meshing
- execution error inside the mesher. The process suffered an unhandled exception or ran out of memory
© 2022 Copyright ANSYS, Inc. All rights reserved.