Packaging 001 - FCBGA free warpage

In this example, warpage and thermal stresses due to thermal expansion are considered for a Flip Chip Ball Grid Array (FCBGA) semiconductor packaging solution.

 

Top plate hidden, translucent view

 

Translucent view, parallel projection

 

Simulation setup guide

Below, you’ll find a simplified guide for setting this up in Quanscient Allsolve.

Step 1 - Import the geometry

In the Model section, start by importing a .step file for your FCBGA model:

File download link: fcbga.step

 

Step 2 - Define shared expressions

Proceed to the Properties section, and define the following shared expressions:

Name	Description	Expression
Tsf	Stress free temperature [K]	273 + 150
Tend	Final temperature [K]	273 + 25

 

Step 3 - Define shared regions

Continuing in the Properties section, define the following 9 shared regions:

1. Define the ball grid array volume shared region v1_bga.

Tip: Text-based target picking

When picking targets for shared regions, utilize text-based picking:

1. Click the Filter icon.
2. Select Text.
3. Input target tag ranges as text.
4. Click Set tags.

2. Define the substrate volume shared region v2_substrate.

3. Define the cut rails volume shared region v3_cutrails.

4. Define the micro bumps volume shared region v4_microbumps.

5. Define the flip chip volume shared region v5_dieFC.

6. Define the heat spreader volume shared region v6_heatspreader.

7. Define the underfill volume shared region v7_underfill.

8. Define the solder balls volume shared region solderballs, which contains all volumes from the v1_bga and v4_microbumps regions.

Tip: Copy-paste ranges through text-based picking

When picking targets for the solderballs shared region, utilize text-based picking:

1. Click the Filter icon.
2. Select Text.
3. Copy tag ranges from the v1_bga and v4_microbumps regions text-based picking window, and paste them here separated with a comma.
4. Click Set tags.

9. Define the all regions volume shared region allreg, which contains all volumes in the model.

 

Step 4 - Define the materials

Finally, in the Properties section, define the model materials.

In this example, 3 new materials are created:

• SAC305
  • Solder balls
• E705GX
  • Substrate
• Underfill
  • Underfill

The 3 following predefined materials are also used:

• Aluminium
  • Integrated heat spreader
• Copper
  • Cut rails
• Silicon dioxide
  • Flip chip

See the dedicated subsections below for detailed material definitions.

Material 1 - SAC305

The SAC305 material is defined for the FCBGA solder balls.

Create a new material:

Name	Abbreviation	Material color	Target
Solder ball	SAC305	Light gray	The solderballs shared region

Add properties to the material:

Coefficient of thermal expansion	Elasticity matrix	Thermal conductivity
20e-6	Poisson’s ratio: 0.3	60
	Young’s modulus: 45e9

Now, your SAC305 material is defined.

Material 2 - E705GX

The E705GX material is defined for the FCBGA substrate.

Create a new material:

Name	Abbreviation	Material color	Target
Substrate	E705GX	Green	The v2_substrate shared region

Add properties to the material:

Coefficient of thermal expansion	Elasticity matrix	Thermal conductivity
ifpositive(T-(260+273), 7.8e-6, 2e-6)	Poisson’s ratio: 0.3	0.65
	Young’s modulus: ifpositive(T-(260+273), 16e9, 25e9)

Now, your E705GX material is defined.

Material 3 - Underfill

The Underfill material is defined for the FCBGA underfill.

Create a new material:

Name	Abbreviation	Material color	Target
Underfill		Cyan	The v7_underfill shared region

Add properties to the material:

Coefficient of thermal expansion	Elasticity matrix	Thermal conductivity
ifpositive(T-(140+273), 80e-6, 20e-6)	Poisson’s ratio: 0.3	0.52
	Young’s modulus: ifpositive(T-(140+273), 0.65e9, 10e9)

Now, your Underfill material is defined.

Material 4 - Aluminium

The Aluminium material is assigned to the FCBGA heat spreader.

1. Pick Aluminium from the materials library.
2. Select the v6_heatspreader shared region as target.

Now, your Aluminium material is defined.

Material 5 - Copper

The Copper material is assigned to the FCBGA cut rails.

1. Pick Copper from the materials library.
2. Select the v3_cutrails shared region as target.

Now, your Copper material is defined.

Material 6 - Silicon dioxide

The Silicon dioxide material is assigned to the FCBGA flip chip.

1. Pick Silicon dioxide from the materials library.
2. Select the v5_dieFC shared region as target.

Now, all your model materials are defined.

 

Step 5 - Define the physics

Proceed to the Physics section to define the project physics, interactions and couplings.

In this example, two physics are required:

• Solid mechanics
• Heat solid

See the corresponding subsections for detailed definitions.

Physics 1 - Solid mechanics

• Let the solid mechanics target default to the whole geometry.
• Add the Solid mechanics - Heat solid coupling Thermal expansion.
  • As target, select the shared region allreg, which contains all volumes in the model.
  • Set Reference temperature to Tsf.
    • Tsf is a shared expression that was defined in step 2.
• Add Constraint and name it as Uxyz constraint.
  • As target, choose a bottom corner point on the substrate volume
  • Set Constraint value to [1, 0; 1, 0; 1, 0].
• Add another Constraint and name it as Uyz constraint.
  • As target, choose another bottom corner point on the substrate volume
  • Set Constraint value to [0, 0; 1, 0; 1, 0].
• Add a third Constraint and name it as Uz constraint.
  • As target, choose a third bottom corner point on the substrate volume
  • Set Constraint value to [0, 0; 0, 0; 1, 0].

Note: Rigid body motion

To simulate free warpage, rigid body motion must be prevented. To prevent rigid body motion and make the model stable, all 3 translational and 3 rotational degrees of freedom must be constrained.

Applying constraints to the three points on the model as described above is sufficient to make the model stable, as long as the points are not along a straight line.

Now, your solid mechanics are defined.

Physics 2 - Heat solid

• Let the heat solid target default to the whole geometry.
• Add Constraint.
  • As Target, select the shared region allreg, which contains all volumes in the model.
  • Set Constraint value to Tend.

Now, all your physics, as well as their interactions and couplings are defined. Before moving on, check that your physics tree looks like in the image below.

 

Step 6 - Generate the mesh

Proceed to the Simulations section and create a new mesh:

1. Set Mesh quality to Expert settings.
2. Set Scale factor to 2.
3. Click Apply and mesh.
4. Once meshing is finished, click Show preview.

In the preview, your finished mesh should look something like in the image below.

Note: Mesh quality

A mesh generated with scale factor 2 produces quite a coarse mesh, that allows for faster simulations, but poorer results. For extracting accurate results, consider using a finer mesh generated with scale factor 1 or 0.5, for example.

For more tips to do with meshing, see Meshing.

 

Step 7 - Simulate

In the Simulations section, create a new simulation:

• In Simulation settings:
  • Set Analysis type to Steady state.
  • Set Node count to 10.
  • Set Node type to 1 CPU, 16 GB.
• In Mesh, select the mesh you generated in step 6.
• In Outputs:
  • Add u field output.
    • Enable skin only.

Run your simulation by clicking Not Run.

 

Step 8 - Plot & visualize

In the Simulations section, add plots to see value output results, or visualizations to see field output results.

To visualize the u field output, for example, add a new visualization:

• Click + next to Visualizations.
• Click + next to Visualization 1 and Select field u.
• Click + next to u and select Warp.
• Click Reset to current data next to Scale factor.
• Click Render.

 

Results

Below is an example of warpage results post-processed to an animation.