Bolt & Weld Joints Modeling? 2

[JayZ]

Hi Everyone,
I started using Nastran last few months, I am modeling a support structure that has weleded joints and boltede joints. How do I model the bolted joints? I can modle the weld joints knowing the weld dimensions and the weld material, is there any other considerations for modeling a weld joint?

Thanks
JayZ

 

[corus]

If you're only interested in the overall structure then don't model the welds or bolts but assume that you have a continuous stucture. A better way, but more time consuming, is to rigidly link the separate parts and from the links derive the forces to assess the welds or bolts. If you require a detailed assessment of the bolts then Abaqus provides a method for a prestressed bolt which you can use, with contact, to assess the joint. Use a sub model with results from the overall model of the structure to assess the detail.

 

[haynesj]

We use springs to represent the bolts in a joint. Using two coincident nodes, one belonging to one part and the second to the other part, create a 3-d spring (k1=E*A/l and k2=k3=G*A/l). This allows the bolts to more accurately share the load.

 

[prosurface]

Usually, I use MPC for the bolt load in PATRAN, assuming that is what you use for the preprocessing.

 

[Drej]

1. If you're bolting a component to ground:

Just use link8 or pipe16 elements if you're using ANSYS. You can use the CP command to couple one end of the link/pipe element to a list of nodes making up the face which the bolt will contact - be careful using the CP, though, as you'll have to constrain the nodal directions carefully inline with your fixing. Then constrain (using the D command) the other end of the link/pipe element - hey presto a bolt! If you want to pre-stress the bolt you will have to use the link elements, as the pipes don't have this functionality.

2. If you're bolting one component face to another:

Use the link8 elements again. One end of the link element to a coincident node on one component - another end to a coincident node on the other component. Pre-stress the "bolt" (trial and error to get the right pre-stress - this will actually be pre-strain this case) and use the "source" and "target" GAP area elements in ANSYS to ensure the two components stay apart (again, trial and error). You may be able to get away with using CPs instead of your GAP elements here to reduce runtime (I think!!).

Hope this helps.

Cheers!
-- DREJ --

 

[Drej]

Alternatively, see:

http://www.ansys.com/industry/nonlinear/conference_papers/methods_for_modeling_bolts.pdf