Force analysis on Honeycomb structure

    • aryansinha

      I want to calculate the strain developed in a honeycomb structure that i have designed. The following are some images of the CAD:

      Front View (25x25 Cells present)

      isometric view at a corner

      the following are the dimensions of the CAD:


      The height of the structure (in Z direction, i.e out of plane) is 1 mm

      Thickness between hexagons is 0.1 mm

      length of hexagon side is 10 mm.

      I am trying to use static structural for analysis in this case, but the meshing of the structure is taking too much time. I generated the default mesh that ANSYS suggested but that is taking way too much time. 

      The meshing progresses and then gets stuck at this point and stays the same for more than 30 minutes, that is the time i stopped meshing.

      Please suggest how i should proceed.


      Aryan Sinha

    • Keyur Kanade
      Ansys Employee

      Please reduce the problem size. 

      Take only 2 or 3 repetative structure. 

      Use different sizings. Please have a look at following and also go through sizing help. 

      Once you are successful in meshing small part, you can apply this strategy to entire model. 

      Also student licence has limit of 512K cells. Please check on that. 


    • aryansinha

      Thank you. I will follow the steps you have suggested and update this post if i successfully make the mesh.

    • peteroznewman

      In addition to using a smaller number of cells, I recommend you take this geometry into SpaceClaim and use the Midsurface tool on the Prepare tab to replace the sold body with surfaces.

      The problem with the solid body is you need several solid elements through the 0.1 mm thickness. Once you replace the solid with a surface, you need only one shell element to represent the 0.1 mm thickness.

    • aryansinha

      I replaced the solid body with surfaces as you instructed:

      Surfaces made from the mid-surface tool

      I then tried meshing this with adaptive setting and without changing the other default settings to start with.

      But i encountered an error and the meshing stopped:

      I used a smaller 9X9 model this time as compared to the 25x25 model previously.

    • peteroznewman

      Delete all mesh controls. In the Mesh Details window, set the Element Size to 0.5 mm. Turn off Automatic Defeature. Does it mesh without error?

    • aryansinha

      It does mesh for the 9X9 model after turning off automatic defeature. As it meshed for this case I also tried a similar process for 25x25 model. But when try I replacing the 25x25 model with surfaces using the mid-surface tool, Spaceclaim keeps processing for more than 1.5 hours and still doesn't convert the model to surfaces. Spaceclaim becomes unresponsive after this.

      update: Meshing for the 9X9 case finishes but i receive multiple messages of the quad mesher failing.

    • aryansinha

      Once the mesh is successfully made i need to apply a constant load on one end on the structure while fixing the other end and restraining the deformation in only the XY plane. 

      Here is an image (in XY Plane) with the leftmost faces fixed and the right most faces applied with a constant load:

      boundary conditions

      I need to calculate the net strain in the structure and then calculate the young's modulus of the structure. 

      The strain option and total deformation in solution settings provides the maximum values of each in the complete structure. How do i calculate the total strain of the structure after stress application? As in, (total length of structure in X direction after deformation)/(initial length in X direction)

    • peteroznewman

      A Fixed Support on the left edge would not allow the material to contract in the Y direction. That will create a large edge effect since the further away from the fixed edge you look, the cells will be free to contract in the Y direction.

      I recommend an X = 0 constraint on the left edge and leave Y free.

      You can't leave Y free for the whole model as there will be no solution. Therefore, assign Y = 0 to the bottom edge and leave X free.

      Finally, take all the edges on just side of the thickness of the web and set Z = 0 and leave X and Y free.

      Now when you apply a force to the right edge, you will get a more uniform state of stress and strain over the entire net. Since the strain will be so uniform, the strain can be simply calculated by the average X displacement of the nodes along the right edge divided by the width of the sample.

    • aryansinha

      Thanks for your input. I had two questions: 

      1. Can i just select all faces on the structure and apply Z=0 constraint on them, leaving X and Y free?

      2. how do i calculate average X displacement of the nodes?

      Also I haven't been able to make an error free mesh yet. As i mentioned previously, the mesh for the 9X9 model does form after conversion to shell elements but i receive multiple warnings of the quad mesher failing. And Spaceclaim becomes unresponsive trying to midsurface the 25X25 model.

      Please guide me on how i should proceed. 

Viewing 9 reply threads
  • You must be logged in to reply to this topic.