Bolted connection in Abaqus 2

[OrlandoTaddeo87]

Hi everybody!

I've been working for a few months on Abaqus, and my goal is to model a quite complex bolted connection, made of steel, for research purposes.
To practice, I'm triyng to model a simple connection between 2 plates, with only one bolt.

A photo is here:

http://files.engineering.com/getfil...f-9409-76cb4c9b1139&file=Unione_bullonata.jpg

I modeled the bolt with a single part, wich included the bolt's head and shank, and the nut.

I modeled te bolt pre-tension with a specific command in Abaqus (a particular load).

I modeled the contact between the surfaces that can get in contact during the simulation: bolt's shank with the surface of the plates' holes, bolt head with the surface of one plate, nut with the surface of the other plate, the contact between the two plates.
I used a model for the contact that takes into account:
-Tangential behaviour, Penalty
-Normal behaviour, Hard contact

In order to avoid solution problems, I chose to allow the automatic adjustment of the nodes (only to obtain a perfect "pairing" of the surfaces that would have been in contact), and to allow the automatic stabilization, with a reduction factor of wich equal to 0.001.

I created (in addition to the "Initial" step), two steps:
-Step 1, into wich the bolt pre-tension has to be applied;
-Step 2, into wich a force (that "stretch" the connection along its longitudinal direction), is applied.
I chose a total time for each step equal to 1, and the time of the first interval equal to 0.005.

When I submit the analysis, Abaqus is not even able to conclude the Step one, and the process is extremely slow. Abaqus is able to reach only the 0.5% of the total step time, and the analysis is aborted because the increment of time is smaller of the minimun requested (that is equal to 1*10^-6).

I want to ask, if you had the endurance to read all my long post so far

What can I do to solve my problem?
-Change the contact properties or remove some contact between some elements?
-Remove the bolt pretension?

Every advice is gratefully acknowledged.

Orlando

 

[corus]

Have a look on Youtube on how to apply bolt preload. Here's one, but there there many.

https://www.youtube.com/watch?v=aoxWHFo6Ln8

 

[OrlandoTaddeo87]

Thank you very much for your fast answer!

I've watched that tutorial, even before I've created the model, and I would to ask you:

-do I have to select the internal surface of the bolt's shank when the part is ALREADY meshed?

-do I have to partition the part, in order to "split" the bolt into three sub-parts, head, shank and nut? (because I've simply defined a cutting plane in the middle of the shank, in order to have a surface to apply the boalt load).

UPDATE

I've removed the interaction between the two plates, and I've removed the Step 1, so the bolt pre-tension was no longer modeled.
The analysis is much faster and Abaqus is able to apply the entire load (that is not big, though); however, there is "compenetration" between the two plates, of course, and this thing make the model less acuurate, even though I don't know the importance of this "approximation" on the simulation results.

 

[corus]

Select the plane in the middle of the bolt shank to apply the bolt load. It's irrelevant as to whether it's been meshed or not as the load is being applied to the geometry rather than the mesh.

I suspect that partitioning the bolt into 3 cells is simply to make the mesh 'better'. I'd have gone further and extended the shank surface into the bolt head and partitioned the whole thing into 90 degree segments. That way you'd get a structured mesh. It's better than just throwing the tet mesh procedure at it. You'll get better results that way and fewer nodes and elements.

Regarding your update: Removing the bolt pretension load in step 1 doesn't really solve the problem of applying a bolt pretension load.

 

[OrlandoTaddeo87]

Thank you for your advices!

I did another test, using a frictionless contact between the two plates, with "hard contact" as normal behaviour, and it worked, although the analysis took a lot of time.

With regard to what you told me about the bolt pretension load, I've removed it just to obtain a faster and simpler analysis, and to investigate what was the problem. Moreover, looking for this problem in other threads, I've read that modelling the bolt pretension don't affect too much the results. So, I've decided to try simpler models before and, little by little, to create a more complex model that take into account everything.

Now I will perform an analysis with no tangential behaviour about the interactions between the two plates, but considering just the normal behaviour (hard contact) to avoid compenetration.
Maybe, in this way, the analysis will take less time, and I'm going to compare the risults with those obtained using a "penalty" model, to investigate the importance of this "feature", and to understand if is important to take it into account in the model.

Thank you very much for your helpful answers!

 

[corus]

To help the contact use *contact controls, automatic tolerances. It'll run faster that way. In addition try using linear 8 noded brick elements. They have better contact behaviour than quad elements, though you may need more of them to get the required accuracy.

 

[OrlandoTaddeo87]

ok thank you!