Modeling 2 cell wing box under vertical shear loading [FEMAP] help

[carmenta]

Hello all,
I have a two cell wing box cell structure that has been idealized as concentrated areas for the flanges and stiffeners. The spar flanges and stiffeners are assumed to carry only axial loads and the skin and spar webs are assumed to take only the shear loads. My question is how would I model this in FEMAP to validate my numbers that I crunch out from the analytical solution. Currently I've modeled the problem in FEMAP using CSHEAR elements and CROD elements. The CROD elements are the for the concentrated areas and CSHEAR element for webs and flanges. The current configuration is each cell is 10 by 10 inches. I gave the model a depth of 20 inches. I have loaded the model at one of the concentrated areas (i.e CROD element nodes). I have attached the FEMAP model if anything is wondering of the configuration.

My question is whether I am modeling it the right way. I am unable to get the model to run with this configuration.

 

[rb1957]

i haven't opened your attachment ... i imagine that it is quite big. it is slightly easier of us if you give a full error message.

i think CSHEARs need rods all around (ie each side) ... you may be better off with CQUAD and use the material properties to trick them into be shear effective only.

personally i'd also use CBEAMs inplace of the CRODs ... you can use small bending properties to reduce their bending stiffness. with CRODs, what is providing out-of-plane stiffness away from your spar and rib webs ?

another thought, why have so many elements between ribs and spars ? is there a distributed load input (like pressure) ? probably not as CSHEARs don't like pressure.

another day in paradise, or is paradise one day closer ?

 

[carmenta]

I'll try the CRODS on all sides, the model runs with CQUADS though. I have a point load (in-plane shear force) at one of the nodes. A colleague mentioned I needed to apply the load on all nodes in the line of action of the shear force (i.e. on one edge of the model where load is applied). There is no pressure defined, just loads on nodes.

Thanks for the reply btw. New to this forum.

 

[rb1957]

CQUADs fill up the stiffness matrix, so that's why it runs. you can trick the element stiffness to reduce their axial load carrying (reduce, don't eliminate ! ... change E to 10^4 (from 10^7) but leave G as 4E6. also you can further reduce the elements bending stiffness, on the property card there shoold be something like 12I/t^3 ... change 0 (which is the same as 1, surprisingly !) to 0.01.

another day in paradise, or is paradise one day closer ?