Applying Boundary condition to a node in an input file

[slimjimmy]

Hi Guys,

How do you apply a boundary condition to a specific node in an Abaqus input file? When an input file is generated a set is created for each node. Here is an example

** BOUNDARY CONDITIONS
**
** Name: BC-1 Type: Displacement/Rotation
*Boundary
*_PickedSet5, 1, 1, 0.1
*_PickedSet5, 2, 2, 0.2
*_PickedSet5, 3, 3, 0.01
*_PickedSet5, 4, 4
*_PickedSet5, 5, 5
*_PickedSet5, 6, 6

How can I apply a displacement to a node without creating a set? So instead of _PickedSet5 how can I change this to just a node number. The following does not work

*Boundary
1, 1, 1, 0.1
1, 2, 2, 0.2
1, 3, 3, 0.01

Any help would be much appreciated

 

[mechfeeney]

Say you want to apply the boundary condition to nodes 8, 17, and 32...

%%You must first create a node set:

*Nset, nset=MyBCs, instance = Part-1-1
8,17,32

%%MyBCs is the name of the set and Part-1-1 is the name of my part %%in the assembly. Next you apply the boundary condition type to the %%node set.

*Boundary
MyBCs, ENCASTRE

 

[mechfeeney]

Oh...I guess that didn't really answer your question. You have to have a node set in order to apply a BC. If it's just a single node, then make a node set for that single node.

 

[MechIrl]

I think you may be able to get away without creating nodesets by explicitly saying which instance the node belongs to. So for example if you wanted a BC on Node 1 of instance 'Instance1' then you could say:
*Boundary
Assembly.Instance1.1,1,1,0.1

I'm not 100% sure on this but I know it works for other keywords like *initial conditions so its worth a shot.

 

[slimjimmy]

Thanks Guys,

I got it working in the end, using a hyperworks mesh input file. I think Mech Ireland is right, you need to reference an instance each time you reference a node for a BC.