Timber modeling (engineering constants)

I have considered modeling a simple cylindrical piece of wood in tension. I think that the definition of the material should be using ENGINEERING CONSTANTS, indicating different coefficients according to the longitudinal and radial directions, according to:
first line: E1,E2,E3,v12,v13,v23,G12,G13,
second line: G23,T
I understand that it could be like this:

*Material, Name=oak
*Solid section, Elset=timber, Material=oak

These lines have been entered with the “Edit CalculiX Keywords” option.
Could someone tell me how I can ensure that the 1,2,3 directions with which the constants are defined correspond in the finite elements to the global Z,X,Y directions of the model?
Thank you very much in advance for your attention.

By default, this is the case but you could use the *ORIENTATION keyword to change it.

How to check it ? Just load the model (possibly a cube) in different directions and check the displacements.

1 Like

Should I understand that the local axes 1,2,3 refer to the part, not to each finite element separately?

Each element uses global (or local if specified) directions. You could run a single element test (with one hex element) to see how it works. That’s the best way to check and understand material behavior.

Visualization from Abaqus (of course, 1=X, 2=Y, 3=Z):

Is there a way to visualize those local element orientations in PrePoMax?
Thank you very much for your help.
My problem is that, if I have to assign a local system to the elements with ORIENTATION, I should know what the proper axes of each one are like, right?

No, because ortho- and anisotropic materials and thus also local orientations are not yet supported in PrePoMax.

Check how *ORIENTATION is defined. You just specify the coordinates of 2 points forming a new coordinate system to be used for the whole element set (e.g. for the whole part). Normally, it’s not necessary to add spatial variation to this.

1 Like

I have created 3 cubes, with the same material and loading and support conditions, but using ORIENTATION so that the greatest rigidity varies from one to another. And what I get is absolutely zero results. The problem comes from ORIENTATION, since if it is not included it does offer results (obviously the same in all 3 cases).
Do you have any ideas about what I’m doing wrong?

*Material, Name=test
*Orientation, Name=orientationZ, System=RECTANGULAR
*Orientation, Name=orientationX, System=RECTANGULAR
*Orientation, Name=orientationY, System=RECTANGULAR
*Solid section, Elset=Solid_part-1, Material=test, Orientation=orientationZ
*Solid section, Elset=Solid_part-2, Material=test, Orientation=orientationX
*Solid section, Elset=Solid_part-3, Material=test, Orientation=orientationY

cubes.inp (4.1 MB)

This one is incorrect because it uses the same coordinates for both points.

1 Like

You are absolutely right, I didn’t see it! Thank you so much!

You can further define per-element orientation using the *DISTRIBUTION card, followed by element ID and the 2 axes (X- and Y-axes). I have used this to model the changing material orientation through - for example - a log with knots.

Thank you very much for your contribution. I will try it