Hello,
I am trying to simulate a plate lying on a frame- both parts modeled as shell, but I can’t get results of the simulation- every attempt ends with “too many cutback error”, and only displacement results are avalible. Contact is set to hard with 0.3 friction coefficent.
Firstly contact wasn’t working at all- and plate was “flying away”…, then without any significant changes in analysys settings everything started to working, but with a “too many cutback error”.
I known that this error could by made by wrong mesh dimensionsh, second order elements in mesh, wrong distance of plates (currently I have a plane of upper part of frame and a plate on the same plane, but I also tested 2 different cases- with gap between 0,01mm and 1 mm- it also dosen’t work).
Maybe could You suggest what to do, to solve that problem?
Edit
Oh no, I noticed it’s exactly the same case… If you remove the corner nodes from the BCs (these nodes are shared by elements with different shell offset directions), the solution also converges with shell offset:
You could use the Thicken Shell Mesh item to convert the mesh of the frame to solid (pretty much what you get with shells expanded internally to solids anyway) in order to avoid such limitations of shell elements in CalculiX.
Thank You Guys,
Just tested both methods, and both seams to work. I see that in option with thicken shell part deformation is about 2 times higher. I will try to test it tommorow, but i think that is due to overlaping of shells at the corners of the frame profiles
Make sure the thickness is correct. There’s also a matter of element type. Your mesh mostly had S4 elements which are expanded to C3D8I solids. And of course, you can use multiple layers.
Not necessarily. You can use it with one material just to have multiple layers of elements in the thickness direction, providing more accurate results in bending. It depends on the element type but C3D8 is typically too stiff while C3D8R needs a few layers (even 4-5) to avoid hourglassing.
Ah, I see,
Is there a possibility of changing element type, from C3D8/ C3D6 to C3D8R/C3D6R? I remesh model to have 4 layers in Thicken shell Mesh, and i see that c3d8 and c3d6 elements are present. Tried to change this just in notepad, but importing inp file resulted in error (it was probably obvious, but i wanted to known what will happen )
Edit, found that C3D6R are not supported. Only c3d8 changed do c3d8r, and file imported (view of the file was strange, but calulation giva no errors) Result are much different than with c3d8, or i make something wrong in midtime..
You can change the element formulation in the FE Model tab. Right-click on the part and choose Edit. You will be able to choose between different formulations for the current element shape(s).
I wonder which element type is really the best for the frames like that (all test with 4 layers of shell thickness, reults for frame not for plate):
C3D8- 51 MPa, and displacement 0,23mm
C3D8R- 31,18 MPa, and 0,288mm deflection
C3D8I- 60,37 MPa, and 0,26 mm of deflection
Tommorow I will try to find some time to making bending simulation of simple beams and compare with “manualc” calculation, but maybe could You share Your opion, which type of element You preffer in simmilar cases? R looks great, when computing time is important, but stresses are suspicious low for me.
In short words, C3D8 elements are too stiff (so-called “shear locking”), C3D8R elements are good but you need multiple layers to avoid hourglassing. C3D8I is great for bending as long as the elements have good shapes (they lose accuracy really quickly with the distortion).
Be aware that imposing BC Z=0 is, apart from preventing the table displacement in z it also is constraining any base rotation.
¿Are you planning to weld the legs to the ground?
That’s indeed another source of convergence issues but I was more refering to the fact that objects that simply rest on the floor can rotate. When one set up Z=0 in a solid base like here, one is additionally also removing the posible rotation. Like in the picture.
FeaAnalyst thanks for the link, especially this from Abaqus, second one I also found yesterday.
ANYS, it won’t be welded to the ground (actually it is just an example only), but to avoid overconstraining, only one edge (I known, better will be probably one point) is constrained in X, Y directions also.
Of course there is a better option- making a additional part, acting as a flor, and making new contact (actually, firstly i tried to focus on stresses in a plate only, and a frame was considered only as support, but this example became more interesting for me).
Or maybe there is a something better than constraining all legs in Z, and simpler than introduce another element with contact?
I tried this already, but without any satysfying results unless I constrained 2 legs (1 node in them) in x,y diretions, I think it is due to frictionless nature of compression support, and i can’t find out how it should be done yet
Stress distribution then looks strange, and unbelievably
)
