I have been experimenting for many hours trying to get this simple wing simulation to work. I squared off the leading and trailing edges to further simplify the model. I fix the edges at the proximal end (base) and apply an upward force at the distal end (wing tip). I have hidden the top wing “skin” surface in the screenshots below for the purpose of illustration.
I am trying to mesh the parts with 3D Shell Gmsh transfinite 4-sided elements with Blossom recomb algo (essentially 2D quad elements).
The parts seem to mesh perfectly. After I mesh the parts, I assign material and create Shell Sections. I make sure that the wing “skin” surface normals are all facing outward and I offset the “skin” 1/2 the material thickness so that the Shell Section “wing” elements do not “collide” with the Shell Section rib and spar elements.
I try to do the same with the rib and spar parts, but I think that I have some issues with the intersections of the ribs and spars. I can offset the ribs where there is a “T” intersection, but what do I do in areas where there is a “+” intersection? Which way do I offset the Shell Section ribs so that they do not collide with the spars???
I then create TIE constrains. I “search for contact pairs” to create the TIE constraints. I have experimented with large and small tolerances, and I allow for the elements to adjust.
There can be some material overlap when modeling such connections with shell elements. It’s not always feasible to get rid of all overlaps.
But apart from that, what’s the problem ? The analysis doesn’t run or the connections don’t work ? Did you try running a frequency analysis to check them ?
Per this suggestion a couple of weeks ago with another simulation I tried running a frequency analysis, but I was not really sure what I was looking for. The frequency analysis simulation completed, but I did not know what to look for in the results.
Look at the frequency values and deformation of the model (not displacement values) in the different mode shapes. Animations may help too. If there’s something wrong with the connections, parts will detach and even fly away in the low frequency (close to 0 Hz) modes.
I have also noticed that when I search for contact pairs, I get master-slave and slave-master of the same connections. When I eliminated the redundant TIE connection, the model final solved.
But when I have many parts, the number of connection becomes too large to visually inspect and to delete individual TIE connections.
How do I configure SEARCH CONTACT PAIRS to only find one version of each TIE connection?
I have gotten most of this to work. I had to adjust several parameters including:
Element coarse-ness on master and slave sides of TIE constraints as suggested in a previous post.
TIE constraint tolerance - The default value was too small so I tweaked the tolerance until the simulation ran successfully
I had intersecting ribs and spars inside of the wing. I modified the parts in SolidWorks so that I had a 1/2 thickness gap on either side of the intersecting ribs and spars. So I essentially left the rib as-is and then created the 1/2 thickness gap between the spar end and the rib on both sides of the rib. I then offset the shell section of each ribe by -1/2 thickness (e.g. 4mm thick rib, therefore offset -2mm).
Thank you for the suggestion. This would GREATLY simplify my model as I would have far fewer tie constraints to apply. But when I tried to create a compound part, the geometry disappears from the screen. I looked at several posts that described this issue. I currently import a STEP file, so this should certainly work better than and IGES file. But I still have this issue.
meshing as a compound part certainly a good option in this situation. I open ur model in Rhino and found a few odd things. I partly rebuilt it into a clean set of surfaces. I then split all the intersecting surfaces and imported them to prepomax and it allowed a compound part. This allowed me to load the model up with no need for any tie constrains
