I have looked around on the forum and still find i need some pointers. I am modelling a bolted and welded steel structure as shown below and in the attached sat file. Actually the final model will consist of about 5 similar sections bolted together. I have used inventor to defeature the original .iam file (by saving as .sat and then deleting faces/holes in all of the hot rolled steel parts).
For this reason, I must use midplane meshing for most if not all of the parts.
I am happy to assume that the parts will behave as if they are bonded together at all overlapping areas.
The questions i have are:
1. Is defeaturing best done as I have?
2. What is the best cad format to use with ASM .iam, .sat, .igs etc? Currently I save the Inventor .iam file in another format to break the link tio the original cad file. This means I can avoid renaming in the vault -usually a massive job when the parts count is high)
3. Most importantly, what is the best way to midplane mesh the model to obtain a bond between the overlapping areas? I am using 2013 ASM with SP1. Quite honestly, I am confused by the choices with midplane meshing to achieve this i.e. smart bonding, virtual imprinting, junction method, mesh matching etc. The posts i have read so far indicate that if I am using linear stress analysis, then I can't obtain a bond between two midplane meshed parts.
This does not seem correct, because when I analyse the model, most of the parts appear bonded.
Any suggestions appreciated
I believe that defeaturing is best done in a direct modeling software (Inventor Fusion), but the delete face in Inventor also works nicely for me.
I am not sure about this, but both Inventor and Simulation Mechanical/Multiphysics use Autodesk Shape Manager, hence, ipt/iam files should be best (although I have had no problems with other CAD formats as well).
I do not think that the mid-plane mesh is able to match the mesh of 'layered'(overlapping) thin parts. Looking at your model, I can see that quite a number of the parts are layered together at the connections. Hence, I do not think that you should use midpane mesh but should stick to solid mesh. You should enable midside nodes though as your model will be likely to have only one element across its thickness. Having just one element across the thickness may cause your model to be stiffer towards bending unless midside nodes are enabled.
I honestly do not have a definite answer to your question. When it comes to meshing, I believe that different analyses require different mesh treatments. What I can share as a tip for thin models is that, instead of aiming for three elements across its thickness(which would obviously greatly increase your element count), you should enable the midside nodes. I am no expert but I think this helps with the problem of shear locking in case of bending. Other than that, you may need to do a mesh convergence study. -ilyas-
I have now had success with 8 node brick elements on this large thin steel structure. I am happy to persevere with brick elements instead of midplane meshing.
I did some trials with the accuracy of 8 node brick vs 20 node brick, 4 and 10 node tets and convinced myself that 20 node bricks were definitely the way to go.
My problem is that, I cannot get this structure to mesh in 20 node bricks. I am using 20 mm fixed mesh size and this usually gives me 1 element thick thru the plate. I can live with this in terms of solution time.
I have tried most things. Is anyone able to mesh this model with 20 node bricks (midside nodes enabled in element definition).
I have successfully used 20 node bricks on a simple large section RHS without a problem. The problem is with the complex mix of parts that I have now.
Any suggestions would be greatly appreciated.
What kind of loads/constraints you have in the analysis?
Midplane mesh will not work in this model. You can either use plate elements or brick elements to mesh you model, and the total element count won’t be high for this model.
What is the total element number now after you have meshed your whole model with brick elements?
Do you mean enabling the 2nd order element in 3D Mesh Settings>Options>Surface?
How about just using the midside node(insde element definition) without the 2nd order element(mesh settings) enabled. You do not need to remesh the model(just use the same 8 node bricks) but will still get the element flexibility of the quadratic element(20 node bricks), if I am not mistaken. The 2nd order elements may benefit you in capturing the curvature of some some arcs, but I do not think that this is necessary for your purpose.
Hxq and Ilyas,
thanks for your help here. There is about 60000 elements here. Yes, I did have success when I unticked the "generate 2nd order elements" but selected midside nodes in element definition. So that was helpful. I'm now meshing the full size structure which consists of 5 similar modules. I'm nearly there. Last thing today a few pieces "fell off". I noticed that I was using the welded contact instead of the bonded contact. More work tomorrow.
Thanks again guys.