Not sure why you're having a problem. Even using a solid mesh, this should mesh OK and run fairly quickly.
do you want to post the part and let us take a swing?
Hello Dan - Thanks! I posted a zip file with the assembly down at the bottom of the thread. I set up the fixed geometry and loads, so I think those files are in there as well (I hope!). As I said, I'm interested in the deflection of the aperture and the sensor as the telescope rotates from horizontal to vertical (aperture-down). I appreciate any help or advice you can give.
It doesn't look like you modeled the angle using a weldment feature.
Do this, and then make the extrude cut in the member and save as a part.
Build your structure as an assembly with those cut weldment parts and treat them as beams in your assembly simulation. It will still account for the cuts in the angle with variable moment of inertia, but the simulation will render the beam as a simple cylinder so any stress concentrations you may be concerned with in the angle will be ignored at that level. But like Dan said, if you're only concerned with the individual part you should be able to use a solid mesh without much trouble.
Have you checked to see if Graham Mustoe could help you out? Go Orediggers!
Yes, you can use Simulation to create a sort of meta-material definition that represents modified beam here. What you would do is create a representative model like you have done here but you would extend the cuts from end to end. You still want a slight amount of material on both ends that makes each end profile still have the uncut beam profile. From there you will use a solid element mesh, apply a dummy load to one end, and a fixture to the other to bend the model as a cantilever beam. Run the study. The result you are looking to extract from the study is the maximum deflection/displacement for use in this cantilever beam equation:
...sourced from here (Cantilever Beams - Moments and Deflections). You will have known values for these variables:
F = applied force on end of beam (N)
δ_b = maximum deflection due to bending (m, mm, in)
I = moment of Inertia (m^4, mm^4, in^4)
L = length of beam (m, mm, in)
...and be able to back calculate the new meta value for E in bending (or E_bending) for that direction of bending. You may want to assume the other bending direction is the same but you will definitely want to also run an axial pull test in this same manner and use this equation:
...sourced from here (Axial Deformation | Strength of Materials Review) to run determine the E_axial with these known values:
F = applied force on end of beam (N)
δ = maximum deflection due to tension (m, mm, in)
A = cross sectional area of beam (use uncut cross section) (m^2, mm^2, in^2)
L = length of beam (m, mm, in)
...and back calculate E_axial.
Having calculated E_bending and E_axial meta values you now make a custom orthotropic material using E_bending as E_x and E_y, then use E_axial as E_Z.
That was a lot of work already but now you have to apply this meta material definition to an uncut beam and test that the meta material values give you the same deflections under the same loading. In my experience they are close but not exact, so what I typically do is make corrections to E_X, E_Y, and E_Z by calculating the ratio between the deflection of the cut beam model and the non-cut beam model with the meta material applied. I multiply that ratio against the meta E values I have already to force the meta E values to give the correct deflection to match the solid-element cut-beam model's deflection.
Once you are done you should have a meta material definition that lets you use a plain beam element mesh to analyze a much larger structure a bit quicker than if you used a solid element mesh throughout.
I hope this all makes sense.
What is the difference between your solution and just treating the cut angle parts as beams in the simulation in a linear elastic isotropic model? I'm just curious about the accuracy you gain by going this route and the difference of this method vs treating the cut angle as a beam in a linear elastic isotropic model? Is there something going unaccounted for in the simulation if you don't create a custom orthotropic material for beams with significant cutouts?
If the cutout pattern in the angle changes, even slightly, you would have to go through the process of defining and verifying the new Ex, Ey, Ez values again so it sounds like a lot of work and it's not clear to me why its needed. Aluminum is an isotropic material, and using a linear elastic isotropic model with beam elements you get different displacement values with material removed from the angle than you do as a solid angle so the missing material isn't ignored. So why all the trouble to create a new custom material?
Beam elements would not recognize the cutouts. Beam elements, in simplifying the model, recognize only a constant and tapered profile. The cuts are complications that a beam element itself could not account for so in order to use beam elements it would need to be accounted for in the material definition as a meta-material.
The reason for creating an orthotropic material is that I might expect that the two bending tests would yield different E values than the tension test on the beam. In the spirit of putting in as much "good" data as possible I would want to express that in the definition of the meta-material in the form of an orthotropic material definition. This is just a hunch though. Doing the testing for E in all principle directions will confirm whether to use an orthotropic material or if you can leave it as an isotropic material.
Yes, if the cutouts change the testing for E would have to start over and can be somewhat time consuming. If you are willing to make the meta-material and are okay with it as a simplification of the analysis you could do an analysis of a larger structure based on these custom beams. That larger analysis has the potential to go fantastically faster than if solid elements were used instead. So, if you spend an hour calculating/refining the meta-material properties each time you do it but it saves you from having to run an analysis that takes 24 hours to complete, it is time saved in the end.
Hi William, looking at your aluminium angle it seems that the torsion and shear on the single element could be negligible. Then just model a simplified angle bracket having thew same tension and compression behaviour and replace all the brackets with the simplified ones.
Hope it helps.
Thanks for all the responses. I'm still working on the problem. Got side-tracked on other fires for a while, but I'm back to working on this (along with some Motion analysis, but that's another story....).
Here's a screen-capture of the assembly I need to do a static analysis on. It's a large-ish telescope and I need to estimate the deflections as it is rotated from horizontal to vertical. For scale, it's about as big as the freezer in your garage. That round hole in the front is a meter in diameter.
I have attached a zip file of the model, with all the unnecessary bits removed. I think I save the fixture and loading conditions, so they should be there if you open the model.
How do I tackle this?
Frame.zip 8.1 MB