Defining Sections and Section Assignments for laminated composites 2

[blogan]

I am modeling a fairly simple composite box beam that has a balanced, symmetric layup (-45,45,0,45,-45). I have tried modeling the beam using two approaches because I can't find any examples of how to model a laminate.

The first approach I tried was to define one Section ("ply layup") with five plies in the correct stacking sequence. I then created one Section Assignment using "ply layup" and selected all surfaces of the beam.

The second approach I tried was to define three Sections ("layer -45", "layer 45", "layer 0") with one ply each. I then created five Section Assignments using each of the three Sections in the correct stacking sequence.

Otherwise the models were exactly the same but when I view results they are very different. I am new to ABAQUS but not new to FEA software. Please tell me why these approaches give different results and which one is correct.

PLEASE HELP
Thanks

P.S. An explanation of how to correctly model a layup would be extremely helpful. For example, what is the correct way to model ply drops, lap joints, stagered plies, etc?

 

[brep]

Your first approach was the correct one.

In ABAQUS, elements (i.e. geometric regions) must have a single, unique section assignment. The last one assigned wins. Knowing this fact you can now understand why your second approach would only have actually modeled a single -45 ply.

 

[blogan]

Thanks brep, but the problem I have with this explanation is that if I view the material orientation in the visualization window when I use the second approach I see a huge mess of orientation vectors that show 0's, 45's and -45's. Does that mean the presence of the layers with the correct material orientation in the model has no influence on the solution if the Section and Section Assignments are not defined like you said?

And another question along the same lines: is there a way to view results (stress contours, strain contours, material orientation, etc) of individual layers? One of the example problems mentions defining Section Points in the Field or History Output Requests but I don't get a ply-by-ply visualization if I use the same Section Points they use. This would be a great way to check that the layup is correctly defined in the model and would be a significant improvement over the current method of just looking at a mess of orientation vectors that may or may not be in the correct layer.

 

[brep]

If you assigned the sections as you described in method 2, you will actually only end up with ONE shell section in your model. Have a look at the inp file if you are game... Search for "*Shell Section". If you find more than one of these then you are doing something that you have not described fully in your first email.

When you look at material orientations in Viewer you will see a single triad (showing the 1,2 and normal directions) per element. Use a display group to show only a single element if your viewport is too cluttered. You can also use the material orientation options to show only the 1 direction and shorten the length of the glyph!

Now, the input file for method 2 (where you keep assigning sections one after the other) will show, as I said earlier, a single *Shell Section keyword. It might look something like this:

*Shell Section, elset=_PickedSet7, composite
1., 3, Material-1, 45.

In my test I created 3 sections (45,-45,0 orientations) and then assigned them as 5 section assignments (45, -45, 0, -45 and 45). Only the last one is actually used since it overwrites the previous ones.

The correct method, is to use a single shell section that contains all 5 plies. You will only need to make a single assignment too. The input file will look something like this:

*Shell Section, elset=_PickedSet9, composite
1., 3, Material-1, 45.
1., 3, Material-1, -45.
1., 3, Material-1, 0.
1., 3, Material-1, -45.
1., 3, Material-1, 45.

Note the 5 different plies in the stacking sequence.

As for output, I have to go home now (it's snowing hard here!!) but for starters you will need to request the output correctly. This means in the step module, under field output requests, you need to request output at the specific shell layers you are interested in. The shell you create will have 3 section points per layer --> 5 layers = 15 section points. If you want to look at output on the top middle and bottom for each of the 5 plies you need to fill out the bit at the bottom of the dialog - check the radio button next to "specify" and type in "1,2,3,4,5,6,7,8,9,10,11,12,13,14,15" These are the shell layers for which you'll get output.

In the interests of time and resadbility, please try the above on a small example model, and if you are still having trouble post your experiences and we can talk about the section point dialog box in Viewer in an next installment.

By the way, if you think this sounds a bit cumbersome, it is. But if you keep your eyes on the upcoming ABAQUS release (6.7) then you'll be pleasantly surprised at the enhancements made in this area...