Shell resultant stresses


Is there a way of calculating shell forces (membrane, bending and shear) in Calculix? In particular, I’m interested in composite materials with a layered structure (set up as *SHELL SECTION, COMPOSITE).

Let me know and thanks in advance,

It seems that output of section forces in CalculiX is available only for beam elements, not for shells.

Hello, thank you so much for the answer. Is there at least a way of getting stresses in the layers (sigmaxx, yy, and so on)?

These two sentences from the manual are crucial here:

In a composite shell there are two integration points across each layer.

Element variables (selected by the EL FILE, ELEMENT OUTPUT and ELEMENT PRINT keywords) are stored at the integration points in the .dat file and at the nodes in the .frd file.

So it seems that you will get stresses at each layer in the dat file (tabular data) but you won’t get them in the frd file (contour plots).

1 Like

OK Calc_em, thanks a lot for the support. I’ll have a look what i get in the .dat file and come back if I have other questions.

i’ve used ccx laminate composite shells with mecway and it works fine. you can view the stress in each layer. however, you can’t get a good view of the interior. ccx expands the shells into solids. because of the node renumbering that goes on with the expansion, you can’t export the deformed shape either.

Right, you can view the stresses in each layer since CalculiX expands shell elements to solids and results are displayed on the 3D representation. And, as I’ve mentioned before, you may also write the stresses in each layer (2 integration points per layer) to the dat file.

ok, thanks for the detailed answer. My question now is: Let’s assume I have a shell S8R element with 2 layers. This means that it will be expanded into a brick element with 20 nodes and 16 integration points, correct? If so how are the gauss integration points numbered and positioned? I would need to average the values of the stresses in each layer, but how do I know if an integration point is part of the first or the second layer?

Here an example:

  1068   1 -6.101508E+00 -1.058271E+01 -2.133855E-01  6.179681E+00 -5.434341E-01 -2.043240E-01 ORIENT_shell_0000001
  1068   2 -6.131492E+00 -1.113725E+01  3.538874E-01  5.390696E+00  9.246236E-01  4.443440E-01 ORIENT_shell_0000001
  1068   3 -5.797471E+00 -1.125782E+01 -2.704266E-01  6.834847E+00 -5.356335E-01  1.922444E-01 ORIENT_shell_0000001
  1068   4 -6.585393E+00 -1.307855E+01 -6.730292E-01  7.107561E+00  8.699766E-02 -4.548404E-02 ORIENT_shell_0000001
  1068   5 -5.603279E+00 -1.042116E+01 -7.329061E-02  5.798019E+00 -4.690543E-01 -1.759954E-01 ORIENT_shell_0000001
  1068   6 -6.520001E+00 -1.202259E+01 -9.241151E-02  5.725542E+00  8.970824E-01  4.162206E-01 ORIENT_shell_0000001
  1068   7 -4.607764E+00 -1.029000E+01 -7.685021E-02  6.272161E+00 -4.470338E-01  1.687185E-01 ORIENT_shell_0000001
  1068   8 -5.371363E+00 -1.157878E+01 -1.972184E-01  6.563876E+00  8.121031E-02 -3.948317E-02 ORIENT_shell_0000001
  1068   9 -5.249432E+00 -1.031033E+01  2.183007E-02  5.521565E+00 -4.143330E-01 -1.678961E-01 ORIENT_shell_0000001
  1068  10 -6.814848E+00 -1.267902E+01 -4.238535E-01  5.966693E+00  8.789641E-01  3.898530E-01 ORIENT_shell_0000001
  1068  11 -3.751447E+00 -9.589404E+00  5.846775E-02  5.861385E+00 -3.770122E-01  1.429628E-01 ORIENT_shell_0000001
  1068  12 -4.492790E+00 -1.048300E+01  1.471153E-01  6.165029E+00  8.068876E-02 -3.747116E-02 ORIENT_shell_0000001
  1068  13 -4.780394E+00 -1.016909E+01  1.418864E-01  5.147804E+00 -3.388802E-01 -1.738843E-01 ORIENT_shell_0000001
  1068  14 -7.230955E+00 -1.358648E+01 -8.827192E-01  6.290951E+00  8.570952E-01  3.460230E-01 ORIENT_shell_0000001
  1068  15 -2.600851E+00 -8.643105E+00  2.348454E-01  5.301821E+00 -2.742936E-01  9.613635E-02 ORIENT_shell_0000001
  1068  16 -3.305655E+00 -8.988847E+00  6.123780E-01  5.618999E+00  8.489323E-02 -3.803381E-02 ORIENT_shell_0000001

These are the values of the stresses in all 16 integration points of an S8R element with 2 layers.
I would like to post-process this table and get a unique value of each of the stresses for each layer. But I can’t do that if I don’t know where the gauss points are.
I know from the docs where the gauss points of the corresponding C3D8 brick element are but for my lamiate there are double these points, so I guess the numbering is different.
Let me know if I could express myself correctly.

S8R is expanded into a single C3D20R element, whose integration point scheme can be found in the User’s Manual:

You also have to add those 2 x number of layers integration points across the thickness but I would expect the numbering to follow the same convention.

Keep in mind that you can request the COORD output variable that gives you the coordinates of the integration points.


Thank you so much. Much appreciated