Modelling bolted connection using Abaqus 1

[miguelespinha]

I am trying to model a steel connection on a beam using the finite element program Abaqus.
The connection is made by means of 3 steel plates, 2 bolted to the web and 1 bolted to the lower flange of an I-shaped beam. It has 48 bolts and over 200 surfaces that are likely to become in contact/interaction. The beam supports a concrete slab. The link below shows an image with the model of the connection.

http://files.engineering.com/getfil...7b-4b7b-81dc-75f15b0ba41b&file=connection.gif

The connection will be suject to a cyclic loading of an imposed displacement and the analysis is physically and geometrically non-linear.

Due to the high number of the interacting surfaces, i am having trouble modelling the contact interactions between the bolts/plates/beam. Defining all the contact properties will make the analysis to run very slow, and fail to converge most of the times. If I define tie constraints between the parts however, the model becomes very stiff, resulting in higher stresses than those expected.

Regarding the nature of the problem, I wonder if you have any recommendations. Maybe is there a way to use contact interactions in Abaqus without a such demanding computational effort, or maybe another way to model/mesh the connection using simplifications.

Thanks a lot in advance, I hope I explained the problem clearly.

Miguel

 

[Elabbasi]

If this is the only part of your FE model that has contact, then it's not that big, and computational speed per iteration should not significantly increase when you allow contact between all surfaces. If that is true, then the reason you're getting a slow analysis is that it fails to converge and keeps subdividing.

There are many potential causes for that. However, since it works when you use tie constraints then it is probably due to contact. Are you applying bolt loads to these bolts? If you are not then the bolts will be loosely sitting on the steel plates and that's the worst for contact convergence since nodes keep switching between contact/no contact states. It's also good for contact problems like this to activate the automatic stabilization feature in Abaqus.

I hope this helps.

Nagi Elabbasi
Veryst Engineering

 

[madetoro]

Make sure your not using general contact, but pair surfaces instead (and remove overclosures to get the process started without divergence).

Also monitor where the iteration increases, how many attempts, why (using job diagnostics)and so on. It may be benefitial to have a steady small time step as this may be more stable than to try and do it in one go (can you confirm what analysis your using).

 

[corus]

I'm not sure why you have so many surfaces when you could simply have a single surface for one plate even if a number of bolts pass through that plate.
Split the analysis up so that the first step just applies the bolt preloads. and you calculate the initial prestress, and then the next steps applies your model loads/displacements.

Tata