PLANE182 X SHELL181

  • 671 Views
  • Last Post 15 March 2018
  • Topic Is Solved
Fabricio.Urquhart posted this 06 March 2018

Hello,

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.

 

Order By: Standard | Newest | Votes
peteroznewman posted this 07 March 2018

Fabricio,

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?

Attached Files

  • Liked by
  • Fabricio.Urquhart
Fabricio.Urquhart posted this 08 March 2018

Hello Peter,

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.

Fabricio.Urquhart posted this 14 March 2018

Hello Peter, I modeled the plate and the results were OK.

But now, I am modelling two plates 2D in contact with a moment in the top plate's edge like the picture below.

But there are two messages, and I did not understand. Can you explain these messages?

peteroznewman posted this 15 March 2018

Fabricio,

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.

 

Close