How to apply multiple boundary conditions to multiple nodes in a model?

[Mohamed Attallah]

I am using abaqus CAE (not scripting), I need to apply multiple (different) displacement boundary conditions to multiple nodes (more than 2000 nodes) on the model.
The only way I could find working is to create sets (2000 sets), one for each node, and apply the boundary condition manually, but this is exhausting!
I tried analytical mapped fields, several times but it is not working properly!
Is their any clue?!

 

[FEA way]

That’s an ideal case for Python scripting (it can be used within Abaqus/CAE). Otherwise you would have to export input file and use some advanced text editor to define these BCs semi-automatically.

 

[Mohamed Attallah]

@FEA way
Can you please explain more about the input file!

 

[FEA way]

Check the syntax of the keyword necessary to define these BCs (you can generate one of them in Abaqus/CAE first). Then open the input file in some text editor and copy this keyword as many times as needed. Now the worst part - you will have to modify each keyword so that it refers to proper node set. If you name these node sets properly (for example S1, S2 and so on) you will be able to change the copied keywords with relative ease. And you can try automating it in selected text editor.

 

[oldNail]

Analytical fields by expression or mapped would be ideal for this. What happens when you try to use it?

 

[Mohamed Attallah]

@oldNail
When I tried the analytical fields by mapping (both via coordinates and Grit), ... I did this .... I chose the displacement boundary condition ... I selected U3 and added a value of 1, so that it doesn`t affect the field variable values added later ... on running the job ... it seemed that the displacements were all equal ( not corresponding to the field variable I desired and entered) ... I thought may be it is not ideal for this job! ... However on adding multiple displacement BC for multiple sets of nodes ... the results were reasonable.

 

[oldNail]

Analytical Fields allow you to map a non-uniform distribution onto your model as Boundary Conditions, Loads, etc. If you're getting a uniform displacement then it sounds like you don't have it setup correctly.

Are you sure that you have the Analytical Field selected as the "Distribution" in the Boundary Condition dialog box? It may still be "Uniform" by default, even after you have defined the Analytical Field.

If you're mapping coordinate based data then your mesh coordinates might not match with the data you are mapping. Maybe the length units are different, parts are in different locations, or axes are oriented differently.

You may review the Boundary Condition distribution before you run the model to make sure you have it setup correctly: Switch to Visualization module, select your "Model-1" as the model (not an .odb), and the Analytical Field Boundary Condition should be available as a "Field Output" for contour plot.