I have a submarine component to analyze, and I was wondering if there is a specific type of boundary condition to use to simulate a immersed part (hydrostatic pressure all over the part). Because when I apply the pressure on every external surfaces and fix a few locations, the pressure resultant is not perfectly = to zero and my model either spin on itself or I got a huge reaction force on my contraint node.
I know for aircrafts there is a trick (using explicit elements to link all nodes to a central one that is clamped, or something like this, but I don't know how to do here.
I would love to get your insight on this topic!
Solved! Go to Solution.
You need to define variable pressure, to learn how to do it take a look to my website in the following address:
Also, variable pressure load is a function of mesh density, then if your mesh is not exactly symmetric in both sides then you could have unbalance load.
If you can't find suitable constraints for the unbalanced load, then you can try running "inertia relief" solution. This allows you remove your rigid body constraints. The solution then uses the mass inertia of the sructure to balance your applied loads. This should distribute your unbalance over the entire model(all nodes with mass) and should avoid any stress concentrations. You can activate this in Femap on the Bulk Data Options form as shown below; use the automatic method:
If your pressure load is applied to all external elements and no others, the load should sum to very near zero. Do you have some opening or attachment point which has no load applied to it?
I would place RBE3 elements on the holes (and load them with the required resultant missing load for each hole), or just fill them with phantom plates which take the load. Otherwise you will not have the right distribution of load on your object, even with inertia relief.