Coupled Nodes?? 1

[Jeremy1989]

Hello.

I am doing an analysis of an electronic chip undergoing thermal cycles. I am using a slice model of the chip and there is a particular boundary condition that I do not know how to apply in ABAQUS.

I want to make sure that a plane that is opposite the symmetry plane to remain parallel to the symmetry plane while the chip is expanding. I understand I can do this by 'coupling' all the nodes on that plane to cause it to remain planar while the plane moving.

I understand in Ansys,you can just simply select those nodes, then select the degree of freedom to be constrained. But I am not sure for Abaqus. I hope someone can help me with this.

Thank you

Regards
Jeremy

 

[IceBreakerSours]

Search for constraints in the documentation; equation (type of constraint) may be of most interest to you.

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[Jeremy1989]

What is the difference between using equation and kinematic coupling constraint?

I tried both (assuming I am doing it correctly). Equation allows me to run to completion but the results seem weird. But when I tried kinematic coupling constraint, it ran into warnings.

Thank you

 

[IceBreakerSours]

A) I repeat: Use the documentation; Analysis User's Manual in particular.

B) How did you write your equation and kinematic coupling constraints?

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[Jeremy1989]

For equation, I selected the all the nodes on the plane except one and named them as a set 'slave nodes'. Then I select the unselected node as 'master node'. Then I go under interaction and select Equation. For slave nodes, I used a coefficient of -1 and for master node, I used a coefficient of 1. The DOF for both are in the Y direction (The nodes on the planes are to move with the same Y displacement).

As for the kinematic coupling constraints, I created a reference point on a random node on the plane. After which, I selected it as the 'control point' and the plane to be the surface that I want it to remain planar. The constraint is also in the Y direction.

So yah, that was what I did. I did read the documentation before, but I am not sure where I had gone wrong though.

Thank you.

 

[IceBreakerSours]

In the case of kinematic coupling, which degrees of freedom (of the coupled nodes) did you constrain? Did you allow "Poissoning" of the coupled nodes?

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[Jeremy1989]

I constrained the U2 degree of freedom, I believe that's the Y direction.

Sorry, I didn't come across the term 'poissoning'. What does that mean? Like poisson effect? How do you enable it?

Appreciate much, thank you.

 

[IceBreakerSours]

I meant to ask whether you were allowing the nodes to translate in the orthogonal directions to allow for the Poisson effect. So, if you constrained the 2nd degree of freedom *only*, then you are allowing the nodes to move freely in the orthogonal directions. Also, I am assuming that the reference node in both cases is forced to move in Y direction only.

If so, then I don't see why there should be any difference in the results, unless I am missing something. If you can, you are welcome to upload your INP.

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[Jeremy1989]

I see. If I get you correctly, all the nodes on that plane will be moving together with the same Y-displacement but could have different X and Z displacements. This should keep the plane to be planar and parallel to the symmetry plane, which is what I wanted it to be.

I have uploaded the input file. I hope you or others are able to help me check if I am missing something as well, will be very grateful for your help.

Much thanks.

 

[IceBreakerSours]

Yes, that is correct.

Coming to your INP, my comments below reflect an outsiders' opinion. Everything that you are doing may be right.

Why do you have 400,000+ C3D8R elements? Given the geometry, I would have imagined a few hundred or thousand (tops!) would do the job.

Unless you expect large deformation, strains, rotations, there is no need to have "nlgeom=Yes" in the step definition.

Also, the mesh quality seems a little off the mark. C3D8 elements give you the "best bang for your buck" *if* they are as close to a rectangular geometry as possible. But if these crooked elements are far away from your region of interest, then you have nothing to be concerned about.

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[Jeremy1989]

With kinematic coupling constraints, it ran into warnings of nodes with inactive dofs. These nodes are those nodes that are both kinematically constrained and with X Symmetry nodes imposed. But at the same time, I cannot ignore either one. It ran into a lot of undercuts as well, as such, I stopped the analysis. So I was asking myself whether my kinematic coupling constraint is correctly set.

The region of interest is actually the solder. But to be safe and accurate, I created more elements for the rests. Ys, I kind of agree with you that my mesh quality seems a bit off, but that is the best mesh I can produce.

Thanks again for your help

 

[IceBreakerSours]

These nodes are those nodes that are both kinematically constrained and with X Symmetry nodes imposed. But at the same time, I cannot ignore either one.

It does not make physical sense which is why ABAQUS decides to ignore one of the constraints for it to be able to solve the problem. If the solution makes sense, then you can ignore the warning.

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083