Hi, I’m currently solving a problem which requires me to use build a 3 layer composite with beam elements (B32). The way I approached this was defining nodes and elements for a single B32 beam and then duplicating these elements 2 times with unique element numbers but using the same nodes as the original beam. After that I apply Offsets to create the composite. I’m not sure if this is the best way to do it though with beam elements though, as I’ve read other posts that this creates knots and over stiffened models, but most of those posts dealt with surfaces. Does anyone have any suggestions to run this problem without running into a knot issue?
My work is mainly with composite materials.
If the laminate stack is simple, or if I’m mainly interested in the displacement, I combine the properties of all the layers into one material using my own lamprop software. Then I create the laminate as a bunch of he20r elements using
This way, I generally need fewer elements to get a decent result.
If I am interested in the stresses in the layers, I will create different meshes of he20r elements for each layer, and then connect them with neigh. Then I will assign the appropriate properties and orientations to each layer.
In both cases, I make sure that the elements are smaller in the thickness then in their plane. That way, I can use my auto-orient software to align the material properties with the layers of elements if the laminate is not aligned with the global coordinate system (There is an example in the linked repository.)
Thanks for the reply. I would love to use he20r elements, however the program which I use only meshes B32 (and B32R) elements for beams. Is there anything specific to B32 elements that you know of?
This small test case doesn’t crash or produce an error.
*HEADING Beam test *NODE, NSET=Nall 1,0.0,0,0 2,0.1,0,0 3,0.2,0,0 4,0.3,0,0 5,0.4,0,0 6,0.5,0,0 7,0.6,0,0 8,0.7,0,0 9,0.8,0,0 10,0.9,0,0 11,1.0,0,0 *ELEMENT, TYPE=B32, ELSET=ES1 1, 1,2,3 2, 3,4,5 3, 5,6,7 4, 7,8,9 5, 9,10,11 *ELEMENT, TYPE=B32, ELSET=ES2 6, 1,2,3 7, 3,4,5 8, 5,6,7 9, 7,8,9 10, 9,10,11 *BOUNDARY 1,1,6 *MATERIAL, NAME=AZ31B ** magnesium alloy *ELASTIC, TYPE=ISO 44.8e9,0.35,293 *MATERIAL, NAME=EN_AW_5083 ** aluminium *ELASTIC, TYPE=ISO 71e9,0.33,293 *DENSITY 2660 *BEAM SECTION, ELSET=ES1, SECTION=RECT, MATERIAL=AZ31B, OFFSET2=0.5 0.03,0.01 0,1,0 *BEAM SECTION, ELSET=ES2, SECTION=RECT, MATERIAL=EN_AW_5083, OFFSET2=-0.5 0.03,0.01 0,1,0 *STEP *STATIC *CLOAD 11,3,-1000 *NODE FILE U,RF *EL FILE ZZS,ME *END STEP
To check, I calculated the same situation with C3D20 elements and with the standard formula for beam deflection. Those two agree with a Z-deflection of -0.29 m.
The problem as defined above only yields a Z-deflection of -0.192 m.
So this formulation is indeed too stiff.
deflection may still acceptable for narrow beam and slender type member related to length, but probably is not for deep beam and stocky members.
since only deflection is a problem, it’s commonly used to modify and adjust the stiffness by reduction values of elastic modulus.
it seems required to digest the source code and implementing similar as
Composite option in shell element (S8R S6)
may i correcting my previous comment. After several tests i found some conclusions: the more stocky member and dense mesh divisions the knot is not to make stiffening the model. In contrast, wider mesh aspect ratio will lead to stiff model. So, it seems the knot existence and disadvantages are related to mesh, not the member slenderness. Interesting me to check further by multiplying division along members then reporting back.
still puzzling me, for a slender member knot still shown over-stiffening the model no matter of mesh aspect ratio being refined.
shear deflection are being ignored in previous hand calculation, after including the effect result shown more consistent with discrepancy around -30% and more. Currently, only by reduced elastic modulus is it possible to refine the models.