General Mechanical

General Mechanical

Creating a mesh for a thin film

    • andrewe
      Subscriber

      Hi, 


      I am attempting static structural analysis for shown model with a force on the shortest edge. However i am having difficulty meshing due to the model being very thin. 



      I realised i cannot simply mesh the thin membrane as a 3D body, as errors occur when trying to mesh. I therefore changed to the membrane to a 2D surface in Autodesk Inventor and added thickness in SpaceClaim, which allowed me to create a 1 element thick mesh in Mechanical.


      However I now realise i require at least a 2 element thick mesh for the membrane - as warned in ANSYS 


      "At least one body has been found to have only 1 element in at least 2 directions along with reduced integration.  This situation can lead to invalid results or solver pivot errors.  Consider changing to full integration element control or meshing with more elements."


      I'd be grateful if somebody could advice me on how to accurately mesh the membrane.


      I have never used the modelling software in ANSYS such as SpaceClaim or DesignModeller so as much detail as possible would be great, I simply wish to edit my imported geometry from CAD so that I can create an accurate mesh.


       


       

    • peteroznewman
      Subscriber

      Leave the thin section as a 2D surface. In ANSYS Mechanical, mesh that with 2D elements that can have a thickness assigned as a property.


      If you wish to consider the two edges with thick beams fixed edges, then don't bring in those solids, just bring in the 2D surface and select those two edges to be Fixed Support. Finally, you can assign a force on the shortest edge.

    • andrewe
      Subscriber

      Thank you, I have exaggerated the membrane thickness here to show my issue - when i have increased the thickness of the membrane in mechanical,  the mesh generated is only 1 element thick - how do I correct this?


    • andrewe
      Subscriber

      I do not wish to model the beams as fixed edges, I need to see the behaviour of the beam also in terms of stress, deflection, strain so would rather keep the model 3D 

    • peteroznewman
      Subscriber

      You can have two surfaces, one for the membrane and another surface that represents the thick beams. That surface has the width of the thick beam as the width of the surface.


      If these two surfaces are in SpaceClaim, click on the Workbench tab and then click on the Share button. The common edge between the membrane surface and the thick beam surface will highlight indicating that these surfaces will be connected by the shell elements sharing common nodes when they are meshed in Mechanical.


      In Mechanical, you will mesh these two surfaces with shell elements that can compute in 3D, the stress, strain and deformation. A shell element is only one element on the surface. It has all the computation in 3D for the thickness that was entered, so two adjacent surfaces can have two different thickness values. There is a display setting Thick Shell and Beams that show this.


      I recommend you build a shell element model first before you spend time building a solid element mesh. It is much easier to get correct results from a shell model than a solid model.


      Please reply with the cross-sectional dimensions (width and thickness) of the thick beam and the thickness of the thin membrane.

    • andrewe
      Subscriber

      Thanks I will try this now, can i use my CAD software rather than spaceclaim to create the surface geometry and import? 


      Are shell elements created by default when imputing thickness for 2D geometry?


      membrane thickness = 0.01 mm


      beam width and thickness = 0.6 mm

    • peteroznewman
      Subscriber

      You can create the surfaces in CAD, but you must then open them in SpaceClaim to use the Share button. If you don't do that, you will have to do extra work in Mechanical to either do a Mesh Merge or add Bonded Contact to connect the edge between the membrane and the thick beam.

    • andrewe
      Subscriber

      Hi, this worked well.


      However I am now further in my analysis and am facing a new issue while trying to simulate fluid flow.


      I am trying to use a boolean to subtract the wing from an enclosure. However this fails due to the model having 0 volume due to being 2D. 



      Adding thickness to mesh worked well for static structural. However I now wish to analyse flow over the wing and couple fluent with transient structural to view the pressure distribution on the wing surface.


      Any help or suggestions would be great thanks.

    • peteroznewman
      Subscriber

      It is possible to analyze fluid flow around a zero thickness surface, you just need to slice the air at the plane of the wing and on each of the four edges so the interfaces can be marked as "wall" where there is a wing or "interior" where air is touching air.


      After you slice the air solid using those 5 planes in SpaceClaim, use the Share button on the Workbench tab to mark the 18 pieces with Shared Topology. If any Contacts are created automatically in the Meshing program, delete them. Shared Topology will connect the mesh.  Use Named Selections on the faces to name the "wall" and "interior" faces, as well as "inlet" and "outlet".  You might find the Explode feature to be useful to spread out the 18 pieces.

    • andrewe
      Subscriber

      Hi thanks for the response,


      Okay I am attempting this currently, I am losing the membrane geometry when opening mechanical.


      I only have the thick beam and the created solid bodies. Why is this?


      Also where can I find the exploded view option?


      I have attached my file.

    • peteroznewman
      Subscriber

      The membrane is just a face of one of the solids.



      I see that the Spar part is imprinted on these solids. For Structural models, a surface body for the thick spars worked well because you could assign a thickness to the spar to represent its stiffness. But for Fluent models, the thickness of the spar has to be physically present to carve out that volume of air to create flow around the thickness of the spar.


      You could either go forward with what you have and ignore the spar thickness in the fluid flow, so it will be an approximation, but it will be simple to set up a structured mesh, or you have to go back to CAD and add planes on every surface of the solid spar and end up with something on the order of 100 small pieces.


      Or you could do an unstructured mesh on a single air volume.

    • peteroznewman
      Subscriber

      Here is the Explode function, but it doesn't work for the solids in multibody parts, it only works for assemblies with multiple parts (components in SC).


    • andrewe
      Subscriber

      An approximation is OK.


      I am simply trying to apply air flow to the wing to roughly simulate the surface pressure experienced during flapping (like a virtual wind tunnel) and maybe apply a non-uniform air flow to apply a grater velocity of air at the tip and lower velocity on the inner wing edge (to roughly mimic flapping). It is more for analysis of the design structure rather than airflow - to see the distribution of pressure on the surface of the wing. 


      So I would like the progress with whatever makes this possible -> using system coupling to see pressure distribution on wing and how the wing deforms under this pressure)


      I would therefore like to use the simplest method to achieve this?

    • peteroznewman
      Subscriber

      Go back to SC, set the Spar surface to Suppress for Physics, then on the Repair tab, merge the faces on the solids that had the Spar width imprinted on them.  Redo the Share button on the Workbench tab.


      In Meshing, make the Named selections as I indicated above. Then the meshing will be straightforward.


      In Fluent, on the input faces, you will want to set a direction to the uniform velocity to make the wing see an angle of attack to the airflow. That is how you get a pressure difference on the two sides of the wing.


      I recommend you start a New Discussion to get help with the Fluent model setup. Post that in the Fluid Dynamics section.

    • andrewe
      Subscriber

      Hi I have attempted this but cannot seem to get it to work ready for fluent. I have suppressed the spar and membrane and created the named sections suggested. 


      I will attach my file to this message if you could please possibly explain my issue.


       


      To clarify, will this allow me to analyse the pressure on the wing surface and how the structure reacts? 


      I apologise for the many questions, I am facing a steep learning curve as I have limited experience with ANSYS and FEA.

    • andrewe
      Subscriber



       

    • peteroznewman
      Subscriber

      Here is a working example.


      Ask CFD questions in a New Discussion in the Fluid Dynamics category.


    • andrewe
      Subscriber

      Thank you for your help with this

    • andrewe
      Subscriber

      When i change the angle of attack of the inlet components to Y and Z = 0.707 to represent a 45deg angle of attack the imported pressure to static structural does not change?

    • andrewe
      Subscriber

      I can't use pressure results from fluent to perform one-way fsi with wing model in mechanical in static structural.


      I need to apply the pressure on my model wing, but i cannot link the geometry from fluent to static structural. I need to use the pressure result to apply to the model wing for structural analysis.


      How do i do this?  Is this possible?


      Thanks for your help, I am running out of time on my project and have been stuck at this point for many weeks now trying to get achieve this setup. 

Viewing 19 reply threads
  • You must be logged in to reply to this topic.