Creating Mesh regarding particular carbon composite part for static analysis.

[Anonymous]

So, during a simulation through linear static stress analysis on the carbon fiber tube is to be conducted, i tried the simulation just by creating a custom material, where i had chosen the tetrahedral composition by giving the corresponding density, modulus and temperature, but not the lattice or the nodal information.

So the results were very crude and unsatisfactory for the carbon fiber,

So can you enumerate the steps for doing so for following parts in attachment in JEPG format.

*and is there a way to save the custom material in the simulation for further use, in time limited edition.

[John_Holtz]

Hi varadude2,

You want to define the element type to be composite (either thick or thin, whichever is appropriate), so you will want to create a mesh that is appropriate for plate elements.

You only need one part. In the element definition, you will define the lay-up (0/+45/-45/90/0) with the appropriate thickness for each layer.

You can create a material library and save the material properties to it. You need to set the material model to orthotropic since that is the material model used for the composite element lay-up. In other words, when you edit the Element Definition to define the lay-up, and click the control to choose a material from a library, it will only show materials in the library that are saved as an orthotropic material.

I hope this helps.

[Anonymous]

Thank you for the reply,

But the problem is the input of the data for the carbon fiber woven tube,
it's very tricky, can you please enumerate the steps for the following
example i have sent you in the previous mail (JPEG) file regarding twill
1.615 inch inner diameter carbon woven tube, with wall thickness 0.125 inch.

* And this tube for my project has to be subjected to a vertical force for
large magnitude, is it possible to simulate that without lumping a flat
surface bonded to the tube.

*And also suggest the best way of meshing, for example, consider these tube
symmetrically arranged to an axis like six tubes arranged in 360 degree
axis, for accurate results should i consider the whole thing or should i
take a section for symmetry.

*And for that purpose how to setup the mesh for composite tube, like
arrangement, for example ,first surface orientation is cross section (i
have attached the image regarding this), and the second stage it gets 90
degree towards the first surface, here's where it gets tricky, can you
please explain.

[AstroJohnPE]

Hi,

1. I suggest that you download the accuracy verification manual and the corresponding archive files. If you go through examples 40, 120, and 131, you will have a better idea of how to enter the lamina information. (Getting the orientation correct is the only tricky part, but that is usually not difficult depending on the situation, and your situation looks easy based on the little information you have provided. The input is not that difficult.) Note that there are other examples in the verification manual that use "composite elements", but not for orthotropic material like you are using.
2. For the vertical force, it sounds like you want to select the edge at the end of the tube (if using a CAD model) or the vertices (nodes, if using a hand-built mesh) to apply the load. You do not need to apply the load to a surface. Use the "Selection > Select" menu, then make your selection, then choose the "Setup > Loads > Force" command.
3. In general, the accuracy will be the same if you do the full model or a symmetry model, but this requires that the geometry, loads, AND lamina input AND results are symmetric. Are the lamina in the tubes symmetric about the symmetry planes? I cannot answer that because I am not a composite expert. But you can answer that question quite easily. Model the whole assembly, but split the model so that you can hide parts in order to do a symmetry model. Run both analyses. Let us know what you find out.
4. You are using composite elements. The mesh for composite elements are just like the mesh for plate elements: the mesh does not model the thickness. The mesh is like a piece of paper; it has no thickness. The thickness is a number that you enter in the Element Definition, so the same mesh can be used for any thickness. (If you were modeling the structure using a solid model and brick elements, you would need to change the model for each different thickness that you wanted to analyze.)

Feel free to attach an archive of your model if you get stuck and ask questions about it. See "Create, Post, or Provide an Archive of your model"

[Anonymous]

Hi, thanks for the solution

I got the results which i determined by the examples you gave in the material regarding thin composites in accuracy verification documents, And as per the info, i applied the material properties of epoxy carbon fiber prep reg 230 G Pa. with the lamina orientation as 0/90/0/90 4 layer, and results obtained were confusing as per my project is concerned can you clear me on this.

[AstroJohnPE]

Hi v.

Can you be more specific? Why are the results confusing? Keep in mind that we know nothing about your analysis (except for the approximate size and that it is a 4 layer composite).

You might want to check the reaction forces to be sure the load is applied properly.