Proper Boundary Condition for Metal Strip Warpage

[ctesguerra2010]

Hi Everyone,

I have a metal strip that I wanted to analyze for thermally induced warpage. This metal strip is composed of a discrete number of "unit" patterns. So to save computing resources and time, I would naturally model and analyze just the unit pattern, and apply an appropriate boundary condition on concurrent/opposite faces so that it would behave like it was in the strip.

Now, after reading online documentation, I think neither Symmetry nor Anti-symmetry would be the proper BC on the opposite faces. If I imagined it correctly, corresponding nodes between the opposite faces must equal in X, Y, and Z displacements, so that the warpage is continuous when you put the model side-by-side to form the strip.

The Questions:

1)    Would the BC I just described accurately depict the analysis intent?

2)    If yes, how do you set the corresponding node pairs to have the same XYZ displacement? I tried using Multi Point Constraints, having one equation per direction, for each node pair. I set the Constant to 0, and the multipliers to 1 for a node, and -1 for its partner node. But somehow it did not work on a simple test model that I analyzed. Maybe rigid elements can tie node pairs together?

       2.1)    Is there a quicker/more efficient way for Multi Point Contraints to select a bunch of nodes on a surface, and make them displace the same way as another surface, instead of writing 3 equations for each node pair, on a rather large model?

3)    If no, how do you setup the BC for a unit participating in a strip?

Best Regards,

Christian

[John_Holtz]

Hi Christian,

I understand the general concept, but I do not understand the details of your analysis, and I think that we need to understand the details. Can you provide a sketch or figures showing some details (such as what portion of the entire model is being analyzed, what is the load, what are the constraints on the full model, what is the general displacement expected, and so on.)

For example, is you model cut on two sides from the full model, so you need the boundary conditions on two sides? Is it cut on four sides? Is the model the same length as the full model but only a fraction of the width?

I would think that some of the displacements on opposite sides would be the same, but I cannot visualize how all three components would be the same displacement. For example, if the strip were in the XY plane, then the X and Z displacements may be the same on opposite sides, but the Y displacement would be equal and opposite?

Any way, the answers to your questions are:

1) Not sure yet. Will know better after seeing a sketch or something.

2.1) No. The MPCs were added to the software for another capability, and the interface to let the user define equations was a "bonus". It was never developed beyond the initial, simple interface.

[ctesguerra2010]

Hi John!

Due to proprietary reasons, I cannot divulge the actual model or drawing. What I can tell you is that the metal strip I am analyzing is an IC package lead frame assembly. It is very much like the attached picture. The problem is how the mold (different CTE; placed at the center of each unit pattern) will react with the strip, in terms of warpage, during temp cycling.

It is a strip with unit pattern, cut on two sides. To simulate Free Warpage while maintaining static determinacy, I set the entire bottom face of the strip with a very low stiffness 3D spring. The only loads are nodal temperatures with varying magnitude, and applied to specific parts only.

I think the two sides that the unit pattern is cut from, must have the same displacement in all directions in order for the faces to "match" when multiple units are "assembled" side by side. The caveat of this method is that it simulates as if the strip is infinitely long; whereas in real life, two ends would be totally free. But I think this is the only way I can get close to reality without modelling the entire strip and gorging on computing resources.

If you need more info, just let me know and I'll do my best to describe the details required.

Thanks!

Best regards,

Christian

[John_Holtz · Accepted solution]

Hi Christian,

It sounds like what you want is a repetitive constraint -- the displacement repeats on the cut face. The software does not have anything that would do that automatically. This is a far out suggestion, but I wonder if cyclic symmetry would be a good approximation? If you could place the axis of "rotation" at an infinite distance, that might simulate repetitive constraints. (I haven't given this enough thought to know for sure, so I may be wrong. And of course the rotation axis cannot be placed at infinity, so the question is how far is good enough and still work within the precision of the computer.) A simple rectangular model where you could do the full model and a "strip" would show if this approach would work or not.

Otherwise, it sounds like the Multi-Point Constraints are the way to go, which either limits you to entering things through the UI, or writing a program to create the input.

I do have one other comment about the temperature load. You mentioned using nodal temperature. I suggest that you check the temperature loads in the Results environment ("Results Contours > Other Results > Applied Loads > Temperature"). If working with a CAD model, the nodes inside the part are not shown by default, so using nodal temperatures may not apply the temperature to the interior of the part. (Instead of using nodal temperatures, you may be able to use part temperature, or use a combination of the stress free reference temperature and default nodal temperature to accomplish the same thing.)

[ctesguerra2010]

Hi John,

Just a follow-up question, is the Cyclic Symmetry applied as an MPC? I just found out that in the same way as Smart Bonding (also an MPC) is not read by the Nastran solver, all MPCs manually inputted are also not read (or applied correctly).

So if I use Cyclic Symmetry, and then use the Nastran solver, will it recognize this BC?

Best Regards,

Christian

[John_Holtz]

Yes, cyclic symmetry is solved using MPCs (multi-point constraint equations). So if MPCs do not transfer to Nastran, then you will need to use the Sim Mech solver.

By the way, Nastran has its own form of smart bonding. So if you are planning to use the Nastran solver, you can right-click on the contact pair in the browser (or the "Contact (Default)" branch), choose "Edit Settings > Nastran contact options".

[ctesguerra2010]

Hi John!

I am having trouble implementing the cyclic symmetry, it does not seem to want to accept the very long radius to the symmetry axis. I think I would prefer the MPC method.

I actually already have the node IDs of the faces I want to match in XYZ displacement. Is it possible to manually edit the ds.cst file for this? Would you know the format/syntax?

Best regards,

Christian

[John_Holtz]

Hi Christian,

It should be possible to edit the MPC file manually (DS.CST) and then run the analysis from a command prompt. (The DS.CST file is overwritten every time the analysis is performed from within Sim Mech.) To run the analysis from a command prompt, see the article How to run a Simulation Mechanical analysis from the command prompt (DOS window)

The only documentation on the format of the CST file is for the old file format. See the page Multi-Point Constraints in the Help > Users Guide. I think that you will be able to figure out the current format easily enough from that.

[ctesguerra2010]

Hi John,

If I could ask for your assistance again.

I cannot seem to figure out two numbers in the DS.CST file. Please see the attached picture, and find the encircled numbers.

The two middle numbers are what boggles me. The second number ("32") does not seem to change between equations. So I'll just do the same and copy it. But on the third number, I cannot figure out any pattern of some sort, to know what it specifically signifies. It looks like it "groups" equations together and is somehow consecutive.

Could you ask Autodesk guys over there for this?

Best Regards,

Christian

[John_Holtz]

Hi Christian,

I think the second number ("32") is related to how the MPCs are created (by cyclic symmetry, smart bonding, the user, and so on). I do not know what the third  number represents.

Essentially, you want to create "user" equations. Try using 0 for the second and third numbers.