Steel Connection Modelling - Frame Model => Plate 3D Model

[scudelari]

Dear All,

Our processes for the design of steel structures consist of using a Frame FEA program, such as SAP2000, to create the frame model of the structure we normally design.
Then we want to make the analysis of the main connections of the model, especially those that would be atypical.

For such connections we normally use another FEA package such as Autodesk Simulation Mechanical in order to create a model detailed model of the connection itself. In this model we can even properly simulate the bolts and the plates, considering their contact and all. We can mix 3D brick elements with plate elements if necessary, but we usually make a plate model.

The thing is, I am not entirely sure on how to properly translate the loads – and the boundary conditions for that matter – from the FRAME model to the more detailed 3D model.

For example, we have this part of the structure that has a connection that we would like to model.

Which, translates into a 3D model as this one:

http://forums.autodesk.com/t5/image...83FD287401/image-size/original?v=mpbl-1&px=-1

The basic question is: What is the best way to insert the conditions from the FRAME model into the 3D plate model?

I have had two possibilities:
[FIRST - LOADS]
a- Create nodes on the Frame model that are the same as the ones shown on the on the 3D model.
b- Read the joint forces for the cropped members on their tip for the desired combination. The following image shows this.

http://forums.autodesk.com/t5/image...A94CFD2DF1/image-size/original?v=mpbl-1&px=-1

c- One of the nodes, the node 193 in this case, is set as being completely fixed (translation and rotation).
d- Compare the loads resulted from the 3D plate model on node 193 with the ones from the FRAME model. If they are the same, the model is OK.

[SECOND - DISPLACEMENTS]
a- Again, make node 193 completely fixed.
b- Insert into the 3D plate model the displacements from the other nodes as found on the FRAME model. The problem here is that, since node 193 on the FRAME model is not fixed, it does move as well. So the translation and rotation of the other joints would have to be relative to the 193 node. For the translation it is easy, since it is just [other_node – 193_node], but for the rotation, how can this “differential” rotation be calculated?
c- Again, the residual forces found on node 193 would be compared for validation.
Does anyone have a better way to do it?
Thank you so much for sharing. I think that we can get to some interesting insight on this topic.

 

[SacovanLoon]

Make cuts in your beam model and ask for all forces, moments, translations and rotations.

Apply these to the plate model, and fix the model according to the 1, 2 ,3 method (free free) with three points. The points should be at a place, where no load or constraint is acting. If all is well, the loads in these points will be very low.
Do not forget gravity.

free free analysis in this paper:

http://www.ite.com/~itekb/whitepaper/white_paper.htm

Saco van Loon 2st

 

[UcfSE]

I would calculate the stiffness at your boundary condition nodes, like 193 if I understood you correctly. I would then provide (coupled probably) spring supports in the FEA model. That should capture the stiffness of the structure on the nodes of interest. Do this by applying a unit load in each of 6 DOF's at the node of interest with no other loads applied, not even gravity. You will get resulting deformations at that node. Then K = P/Δ

 

[scudelari]

Dear SacovanLoon,

The link you shared does not work, and, unfortunately, I did not find much information about the "1, 2 ,3 method (free free) with three points".

Do you have some document you may share to elucidate this?

----------------------------------

Dear UcfSE,

So basically the idea would be to capture the stiffness of the node 193. For that, I would create a different model in which all the other
nodes (in this case, nodes 67, 190 and 191) would be fully constrained.

Through the application of 3 loads on all direction, and 3 moment around all directions, of unit value 1, I would get the displacement that node 193 would have. From that, the stiffness is calculated.

Then, I would go to the plate model and instead o having on node 193 a fully constrained node, I would have these stiffness's.

On the other 3 nodes in the plate model, the application then of the displacements and rotations would be enough?

----------------------------------

Thank you so much!