rigid connections steel frame

[Salvanto2]

Hi! I have a problem with abaqus.
I need to create a steel frame with rigid connections between the beam ends and the columns.
I create 3D wire part for the beams and columns, and I assigned the material, profile and section. After I assembly it, and I create the steel frame. How can I realize the rigid connections between the elements?

Thx in advance

 

[FEA way]

You can use tie constraints or merge parts to realize this type of connection.

 

[Mustaine3]

A screenshot, drawing or sketch would help to understand your question.

 

[Salvanto2]

For example the 3D frame in the attachment. All the columns have He340A profiles, and beam Ipe240. The connections (in red) are rigid.
Can anyone help me to understand how I can model this frame?

Thx

 

[Mustaine3]

If you connect the wire geometrically, then you get common nodes during meshing and the rods are connected to each other.

Otherwise you can use a Tie-constraint or add connector elements between two nodes and use the connector type 'Beam', which is a rigid connector.

 

[FEA way]

Tie constraints are the best option in such case. Just apply them to all rigid joints (select the two ends of wires connected at a given joint). You may have to change position tolerance if default one turns out to be insufficient.

Hinged connections can be realized using equation constraints.

 

[Salvanto2]

Thx for your response.
I connect it geometrically and I create a reference point for every floors. In this point I create a Kinematic coupling constraint and I assigned the intertia mass.
But when I try to do the Jobs to evaluate the frequency Abaqus give me this error: Too many iterations needed to solve the eigenvalue problem.
I also try to evaluate only the first shape mode.

 

[FEA way]

Kinematic coupling is not a good option in such case (I assume that you want the mass to be applied to the whole beam, not just a single node). Check this thread with the discussion about the application of remote mass in modal analysis:

https://www.eng-tips.com/viewthread.cfm?qid=460924

 

[Salvanto2]

I solve the problem, but the foundamental period is 8.47*10^-22.
There is another strange thing, in the deformed beam, a beam moves, like it's coming off the frame. I don't understand why!!!!

 

[FEA way]

Did you use tie constraints ? If yes then you should increase the position tolerance. Modal analysis is the best way to visualize disconnected regions and as you say, they occur at frequencies close to zero.

 

[Salvanto2]

No i connect beam and columns geometrically. I try to use tie constraints.

 

[FEA way]

If you want them to be connected geometrically you have to make a single part from them. It can be easily done in the Assembly module (using Merge/Cut Instances tool that I've mentioned before). Mesh nodes can be merged this way too.

 

[Salvanto2]

Sorry but I don't understand.
I do Merge/Cut in Instance tool. I select Merge (Mesh), in options Suppress and in Merge nodes boundary only.
When I do the analysis there is another error: In model....have not assigned a beam orientation, ecc...
But when I create the beam I assigned the beam orientation...

 

[Salvanto2]

I'll write down the steps I took
1) I create wire part for every type of beam/column
2) I create steel material
3) I create I profile for every type of beam/column
4) I create sections for every type of beam/column
5) I assign section and orientation at every beam/column
6) I assembly the parts with Independend (mesh on istance) and i create my frame
7) I create the step for the modal analysis
8) I create boundary conditions (Encastre) at the foundation
9) I create kinematic coupling constraint every floor with a special join in the centre of gravity. I assign to it the inertia
10) I create the mesh

 

[FEA way]

Merge/Cut Instances tool creates a new part and instance so you may have to reassign orientations. You can check if they are assigned or not using Query tool in the Property module.

 

[Salvanto2]

I have combined the various elements, but I have another problem.
The periods grow with the number of mode and they are very big.
what could be the problem?

 

[FEA way]

Take a close look at the mode shapes (deformations). Do they look correct ? Aren't some parts of the frame disconnected and moving on their own ? Make sure that all units are correct (dimensions, material properties and point mass/inertia values).

 

[Salvanto2]

All the parts of the frame are connected, i check it. I think that a possible problem is the units, but i don't understand why the periods growing!?!?

 

[FEA way]

Do you mean that each of the subsequent modes has higher eigenfrequency ? This is normal, natural frequency extraction procedure finds either selected number of subsequent modes or all modes in a given range of frequencies. Then it displays them in order from lowest to highest frequency.

 

[Salvanto2]

Yes i solved the problem. thx!!!!