Point based fasteners

[jball1]

I am trying to use Abaqus’s “point based fasteners” to model a bolted connection which connects two large structures with 200 bolts. This is a dynamic analysis of a large structure. I can't significantly refine my mesh in way of the connection or the problem will become prohibitively computationally expensive. The bolts are in groupings of 4, with extra space every 4 bolts where there is a stiffener on one side of the connection. My model has a node for every bolt, and then additional nodes at the location of the stiffeners. Other than the locations of the stiffeners, there are no nodes in between bolts.

I am not very familiar with Abaqus’s connectors, and so I’ve been reading the documentation. From what I have read, it sounds like Abaqus requires each connector element to be associated with a minimum of three nodes on each end of the connector (see “Defining the radius of influence”). For my model, this is undesirable. I want each connector to only affect a single node of each of the bolted components. Is it not possible to force Abaqus to only include a single node in the region of influence? Here is the relevant section of the Documentation:

Defining the radius of influence
Each fastening point is associated with a group of nodes on the surface in the immediate neighborhood of the fastening point called a region of influence. The motion of the fastening point is then coupled in a weighted sense to the motion of the nodes in this region by a distributed coupling constraint. Several weighting options are available and are discussed in the next section.

To define the region of influence, Abaqus computes an internal radius of influence based on the geometric properties of the fastener, the characteristic lenght of the connected facets, and the type of weighting function used. The default radius of influence is always chosen to be the largest of the internally computed radius of influence, the physical fastener radius, and the distance of the projection point to the closest node. You can also specify the desired radius of influence. However, Abaqus overrides a user-specified radius of influence that is smaller than the computed default radius of influence. In any case each region of influence will contain a minimum of three nodes.

Any thoughts/guidance would be much appreciated!

 

[FEA way]

Internally, point-based fasteners consist of a connector and distributing coupling constraints so some region (even small) on each of the connected faces is needed. If you want to connect only one node on each side, you may have to use a different type of constraint. Probably MPC, like MPC Beam. Check the Knowledge Base article "Abaqus/CAE plug-in application to automatically generate point-to-point springs, dashpots, MPC constraints, or wires for connectors".

 

[jball1]

Thank you, that makes sense. I feel dumb, but I can't seem to get to the knowledge base article you mention. I am logged in at support.3ds.com/knowledge-base/. When I search for any combination of the words in the title you mentioned, it comes up with nothing. I get "Your search for XXX yielded no results." Do I need some sort of special access to get to it?

 

[jball1]

I would like to define the stiffnesses in each direction, so I don't think MPCs will work, unfortunately. I can do springs, but defining 4 springs (axial, 2 shear, moment) for each bolt is pretty tedious. I'm bummed that connectors won't work. That seemed pretty promising.

 

[FEA way]

It's likely that this Knowledge Base article is available only to users with a customer account. The plug-in would help you define multiple connections between parts but you could also use scripting for that or do it manually. Connectors alone (not as part of mesh-independent fasteners) may help you but you have to connect them properly to the mesh of your model.

 

[jball1]

Ok, thanks. I have an account but our company is currently having trouble with our account. This gives me an excuse to ping on the guy who is supposed to be fixing our access...

I currently have a model of this assembly where I use "CONN3D2" connector elements. They connect directly to vertices on each of the connected pieces. I had to partition the surfaces at every element to get this to work.

As far as I can tell, the CONN2D2 elements only affect one node of each of the connected parts. I just went through the process that I followed to create them to confirm that I didn't have to define a radius of influence. Also, their definition in the input file (see below) specifies one node from each part:

*Element, type=CONN3D2
1, BHD.312, Frame.373
2, BHD.313, Frame.371
etc.

 

[jball1]

Someone shared with me a way to solve my issue. I was able to create attachment points at the locations of the nodes being attached (one set of points for each of the two plates being attached). I then created connectors between the two sets of attachment points. Finally, I used tie constraints to tie the sets of attachment points to the two plates being connected. I set up the constraints so each connector would only grab one node. I was able to do all this with a python script, so it wasn’t as difficult as it sounds.

 

[FEA way]

Do you mean MPC type TIE ? Does it seem to work well when you check the results ? Are the loads transmitted correctly ?

 

[jball1]

FEA way, thanks for the good questions - always important to check results!

I mean a regular tie constraint (see below). I have a version of this model that is partitioned at every node to create vertices there. Results from this older version of the model match results from my current model, so it seems like they are doing the same thing (i.e. each connector finds one node on either side to connect to).

*Tie, name=Frame_to_Fastener_pts, adjust=no, position tolerance=0.1, type=NODE TO SURFACE
"Attachment Points_Frame_CNS_", Frame_at_Fasteners_CNS_
*Tie, name=BHD_to_Fastener_pts, adjust=no, position tolerance=0.1, type=NODE TO SURFACE
"Attachment Points_BHD_CNS_", BHD_at_Fasteners_CNS_