Learning Forum

[Harshil Goyal]

Hi Everyone,

Could someone please advise on how to adjust the normal stiffness factor? I'm conducting a thermal cycle simulation of a symmetric QFN package for solder joint reliability. The solder material exhibits nonlinear behavior, making this simulation nonlinear.

Here are the boundary conditions I've applied:

Fixed support at the bottom of the PCB.
Thermal conditions applied to all bodies.
Displacement specified on faces of the symmetric plane.
Element birth and death conditions.
I've attached screenshots illustrating these conditions. I believe I have a sufficiently refined mesh for my model. However, I'm encountering force convergence issues.

I constructed this CAD model in SpaceClaim, utilizing the "share topology" option to manage contacts in Workbench for structural simulation. However, when I open the model in Workbench, no contacts list is displayed, presumably because the contacts were shared from SpaceClaim. Consequently, when attempting to solve the solution, I encounter force convergence issues.

I've searched online forums and found suggestions to adjust the normal stiffness factor, but I'm unable to locate this option since the contact list isn't visible. Could someone please advise on where else I might find this option? Additionally, any alternative solutions or suggestions to achieve force convergence would be greatly appreciated. Thank you for your assistance.

Regards,
Harry

 

 

 

[peteroznewman]

When all the bodies in the simulation share any face or edge and the Share button is used to create shared topology, no contacts are permitted between those bodies.

It is possible to create components, put some bodies on one component and other bodies in another component, then open one component, use the Share button on the first component, close that then open the second component and use the Share button on that.  In that way, you can define contact between faces of the two components, while all the bodies within each component are held together by the shared nodes.

You should type in a value of 3 under the Solution Information folder to show 3 N-R Residuals plots under the Solution Information folder.  Look at the location of the Maximum N-R Force Residual in the mesh to know where is the problem that causes the convergence failure. 

I suggest you delete the Fixed Support and use a Remote Displacement, Behavior = Deformable on the face(s) that were scoped by the Fixed Support. Set all six constraints to a value of 0.  The remote displacemet prevents rigid body motion, which would cause the solver to fail, while allowing that face to have a stress-free expansion. The Fixed Support does not allow the face to have a stress-free thermal expansion and can be a source of N-R Force Convergence issues.  

[Harshil Goyal]

 

Hi Peter,

Thank you so much for your reply. Usually, I click “Share for the entire geometry under Workbench” option in SpaceClaim to create contacts (as shown in the image below). However, as you explained earlier, I want to ensure I understand the “sharing topology” part correctly. Do I need to click the “Share” option component by component, right? Referring to the attached screenshot of the SpaceClaim CAD geometry design tree, I need to keep the “Solder Mask 2” and “PCB Copper Pads” components hidden, while leaving the “FR4” component parts unhidden, and then click the “Share Topology” option under Workbench. Once this is shared, I unhide the “Solder Mask 2” components and click the “Share” button to share bodies within “Solder Mask 2” and “FR4,” repeating this process for each component sequentially. Is this what you are suggesting as the correct way?

Also, I am sharing the screenshot of my boundary conditions just to ensure I have applied them correctly. I will remove the fixed support and add remote displacement, but do I need to make any other changes to the boundary conditions, such as removing or adding any? Please suggest after referring to the screenshots of the boundary conditions attached. I would greatly appreciate your reply.

 

 

 

Displacement Boundary Condition applied on Symmetry Faces XY Plane

Displacement Boundary Condition applied on Symmetry Faces YZ Plane

 

Thermal Boundary Condition applied on Entire Geometry

Element Birth and Death on solder joints

Earlier I ussed Fixed Support at this vertex location but I will use remote displacement as per you suggestion. Could you please suggest which part of the geomtery I should apply remote displacement. Also, do I need to remove other displacements as mentioned in above screenshots?

 

[peteroznewman]

If the Fixed Support was one vertex on a solid body at the intersection between two planes of symmetry, you don't need to replace that with a Remote Displacement.  I was guessing you had selected the entire bottom face of the FR4 and that would be a problem, the vertex only is fine.

How many bonded contacts between layers do you need to define? If it is 2 bonded contacts between 3 layers, then you need 3 components. Contacts are useful if you want to turn them off and on during the simulation. You can't do that with Shared Topology.  Contacts are useful if you want to define a thermal resistance instead of having perfect thermal contact between layers, which is what you get with Shared Topology.  Contacts are required if you want a frictional contact, you can't do that with Shared Topology.

I see there are 12 components, but you may not need 11 bonded contact sets to hold everyting together. Shared Topology can reduce slightly the solution time and give clean stress results at the interface between materials. Contacts can make the stresses at the interface become noisy because the nodes don't have to be lined up.

[Harshil Goyal]

I don't neeed frictional contact or thermal resistance in between so I guess the share topology is fine the way I am doing. I will use N-R Force Residual plots to see what bodies in my geometry is causing force convergence issue. I will reach out with those plots once I have the data. Thank you so much for your advise. 

[Harshil Goyal]

Hi Peter,

Quick question: I was able to converge the solution, but I'm not getting the expected results. The total deformation on the Yz plane differs from that on the Xy plane. However, the expected deformation should radiate outward from symmetric corners. I'm not sure what's happening, but I suspect it could be due to the boundary conditions. Do we only need to apply displacement, or is there something else I need to define for the symmetric plane? I read on an online forum that the symmetric face should be applied as a symmetry region in the model in Workbench. Should I add the symmetry region to my analysis, or is applying these displacements as boundary conditions sufficient? If not, how can we apply the symmetry region in Workbench, and if I apply that, do I need to remove displacement as my boundary conditions, or should I still keep it as part of the analysis?

[peteroznewman]

If you have a face created by cutting a solid body with a plane of symmetry, create a Displacement BC on that face to prevent nodes from moving normal to that face, leaving the other components Free. You don't need to use a Symmetry Region. You can use one and that is what it will do under-the-hood.  The benefit of a Symmetry Region is if you have the edge of a shell mesh on that plane, it will apply the 2 rotational constraints that must be added to the translational constraint you are applying with the Displacement BC.  Another benefit is to expand the results to mirror them to the other side of the plane that wasn't meshed.

[Harshil Goyal]

Thank you so much Peter for your sharing your great knowledge on this topic. I really appreciate your help solving this simulation problem. 

[Harshil Goyal]

 

Hi Peter,

I was able to complete simulations for the model mentioned above, and it has successfully generated a solution. However, the file size is quite large, approximately 285 GB. Upon attempting to evaluate the results using the solution, an error occurred at the end. The error message reads:

”Update failed for the Results component in 6×6 QFN Simulations V2 (Design B). Update of the Results component in 6×6 QFN Simulations V2 (Design B) did not mark container as updated (final state is Modified).”

I am hesitant to discard this solution or rerun the simulations, as it would entail a significant amount of time. Is there a method to resolve this issue and still utilize the current solved solution for results evaluation?

 

 

[peteroznewman]

Open Mechanical and look through the results. One of them has an issue. You can freely delete result requests and make new result requests. This will not harm the solution. Once you have all the results correctly displayed, you can update the Workbench project and save the file with all green checkmarks.

[Harshil Goyal]

 

 

 

 

I did that. I removed the results and and tried requesting to evaluate the new result for only Total Deformation however It is not showing evaluate results options, but only shows solve and start solving the model. My solution file is still in the the folder. When I click reset results (Figure 1 with red cross results) in the project schematic Window, the red cross with yellow flash sign in front of  results changes into green tick (Figure 2 attached) and after this when I open the workbench to see the solution, it still has yellow flash sign. Now I come back to project schematic and right click on results and click update, it starts evaluating results but at the end shows the error that I  shared above (Figure 3). When I see total deformation results, it shows results but not with green tick but yellow flash sign (Figure 4).

Figure 1

 

Figure 2

Figure 3

 

Figure 4  Results Outcome

 

 

Below are the attached other pics from solution window:

 

 

 

 

 

[Harshil Goyal]

Hi Peter,

Please advice if there is a way to fix it. It will be really helpful if you can help sort out this issue. Thanks 

[peteroznewman]

You show only one image of Mechanical before the result has been evaluated. You don't show the image of Mechanical after you request the evaluation. What do the messages in Mechanical say after you Evaluate All Results?

[Harshil Goyal]

 

 

Just so you understand correctly, Figure 4 above is after I evaluate results.

I am adding another figure below that shows before evaluation both outside window and inside the mechanical when the results are reset. Outside everything is shown with green tick but inside the solution shows yellow flash sign. The reset automaically delete the total deformation evaluation and solution shows yellow flash sign.  

When i add Total Deformation option and evaluate (which I am only able to do from outside window as inside it shows solve option only), You can see the yellow flash sign remains same inside mechanical after evaluation even though the total deformation results are produced (evaluated results shown in Figure 4) with the error at the end (outside mechanical in figure 3). The state of evaluated results are not converting into green tick.

 

 

 

[peteroznewman]

With no result request, solve the model in Mechanical and save the Project. Insert the Deformation request but change Calculate Time History from Yes to No. Change the scope from All Bodies to a single selected body, then Evaluate All Results. Does that make a difference?

[Harshil Goyal]

It didn't help, but I simulated the model again as I was running out of time and had to share the results with someone. Thank you anyway for your advice.

I have another QFN package model similar to this one. However, in the new model, I have a quarter model of the package on both sides of the PCB solid body as I'm trying to simulate dual PCB packaging stress. Can you suggest where to apply the Fixed Support boundary condition? I feel like if I apply it to either one of the bottom vertices, it will be closer to one package compared to the other. I don't have any vertices in the middle of the PCB as it's one single square-thick solid body. Any suggestions for this? Should I slice the PCB body into two parts from the middle and then apply a fixed support at one of the vertices from that mid-plane?

[peteroznewman]

If you have two planes of symmetry, XZ and YZ you can pick any vertex in the model and apply a Displacement (not a Fixed Support) of Z = 0 leaving the X and Y Free which will constrain the model and allow thermal stress to be correctly calculated.  You will get the same stress no matter which vertex you choose.  Only the Deformation plot will be different since the Z value will be zero at the vertex you chose.

If you really want the Deformation plot to show the zero Z value at some point in space between the two PCB packages, you can insert a Remote Displacement, type = Deformable and choose an edge on each package. Edit the global coordinates of the Remote Displacement to be on the Z axis.

Please reply with an image of the geometry.