Mesh "Spikes" on Displacement Result

[Anonymous]

Hi Everyone!

I am Christian from PH. After searching around for a week now, I could not get an answer for my questions. I hope you could enlighten me. Kindly see the details below for your perusal.

The Model:

I am trying to investigate thermo-mechanically induced stresses and warpage on an electronic module that consists of a 3-layer "PCB", small components, and pins/terminals; all enclosed in a molding compound (very similar in construction to the common IC chip).

The Problem:

I have been getting unrealistic displacement results (upwards of 1k mm, with a model that is only cm in size!) and corresponding unrealistic stress values. Upon investigation in the results environment (mold not Visible), I am seeing "spikes" in the elements, and very irregular/rough surfaces. Almost like the elements were mangled. Please see the attached images.

The Setup:

The model includes complex geometries that necessitated meshing each piece individually to successfully generate the mesh. As such, smart bonding was turned on (fine to coarse). 3D spring support was also placed on the entire bottom face of the Mold and PCB, to make the model bend freely while being statically stable. All contacts are set to Bonded. Thermal loads are applied via Default Nodal Temp and Stress Free Reference.

I am also trying to emulate "Element Birth and Death". To simulate processing (manufacturing), parts must be activated sequentially after each thermal load step. As such, the deformation between load steps must be preserved to capture residual stresses (I plan to use make .fem) in between and at the last step. ANSYS has this native capability. Anyway, to emulate a deactivated part, I put in custom material properties with very small (1e-06) Elasticity, Poisson's Ratio, Coeff Thermal Expansion. This is so that the deactivated part would not interact with displacements and temperatures of nearby activated parts.

The Questions:

1. What is causing those "spikes" in the displacement results? Is it an artifact of Smart Bonding? Could it be solved by finer mesh still?

2. Are my settings for the "deactivated part" reasonable for the intended purpose? Could the very small values (my hunch is the Poisson's) have been the cause of the anomalous results?

3. The "spikes" look like singularities; and I've read that FEA has limitations with regards to singularities. Am I approaching any computational limit somewhere by my emulation of element birth and death?

Hoping for the community's warm support! Thank you!

Best regards,

Christian

[John_Holtz · Accepted solution]

Hi Christian. Welcome to the Sim Mech forum.

The answers to your questions are as follows:

1. It could be related to the smart bonding. A finer mesh will not help. (If the problem is related to the smart bonding, go to "Setup > Constraints > Multi-Point Constraint" and set the "Solution method" to "Condensation Method".)
2. I think the problem is the very low modulus of elasticity. Poisson's ratio and the coefficient of expansion are not the problem. Computers do not have enough precision to add numbers like 10E6 and 1E-6 and carry all of the decimals necessary to avoid round off errors. You can determine if this is the problem by entering real values for all materials and seeing if the results are realistic.

Have you tried your methodology on a different model to see if it will work? You mentioned residual stresses and exporting the displaced shape to a new model. That will give you the displaced shape but with 0 stress, so I do not know how you intend carry the residual stresses to the next phase.

[Anonymous]

Thank you John.

I will try to explore further Smart Bonding, and probably also change tolerances to see if it will have any stabilizing effect. From your input, I think an investigation into an elasticity lower limit, which can still make deactivated parts not interact, should be in place.

I have tried the method on a much simpler model, just two plates (one is "deactivated") bonded together with matched mesh, and it ran perfectly. I would agree that it has something to do with the precision you mentioned, coupled with a complex model with tiny features, and unmatched mesh. Coming from that, do you think the Nastran solver would have handled it better? I have read in the help files that the Nastran solver was "designed to handle bonded contact between non-matched meshes".

I was planning to carry the residual stresses manually, using "superposition method" where stresses are added/subtracted appropriately and accordingly in between load steps. This is to be done via exporting results and calculating in excel. As long as the displaced results in-between are captured, I think this method will be okay.

Best regards,

Christian

[Anonymous]

Hi John!

I successfully ran the method using NASTRAN! So I think this probably proves that the mesh spikes are caused by the limitations of smart bonding coupled with the extreme properties of the "dead" elements.

However, I am now having a hard time generating the deformed shape using Make FEM. I left Sim Mech run overnight (18 hrs running) to generate the new .fem file but it was still stuck at "Not Responding". My model has close to 1M elements. I haven't found much in the forums regarding the Make FEM function. If you could please point me in the right direction.

Thank you very, very much.

Best regards,

Christian

[John_Holtz · Accepted solution]

Hi Christian,

I think the "Make Fem" command is not practical for large models.

You are using linear static stress, correct? Since it is based on small deformation theory, I wonder if it is necessary to update the displaced shape before activating the next set of parts. Would this method achieve the same result?

1. Analyze model 1 with parts 1 through X "active", parts X+1 through Z "deactivated"
2. Analyze model 2 with parts 1 through Y "active", parts Y+1 through Z "deactivated"
3. Analyze model 3 with all parts "active"
4. Use the Load Combination Utility ("Results Options > Other > Tools > Combine Load Cases") to add all of the results together.

[Anonymous]

Hi John,

Yes, I am using Linear Static. I actually managed to run the load steps individually, and the deformations I am getting is only in the micron range (<100 microns). I think this time, exporting the displaced shape is unnecessary. And you mentioned a good point regarding the Make FEM function, thanks.

Anyway, I didn't know the Combine Load Cases feature until your last message! It's actually what I was thinking about all along. Now I would just have to prove that this can produce comparable results compared to ANSYS Birth and Death function.

Thank you very much for your help!

Best Regards,

Christian