+1 800 942 2072 |Sign In|Contact Us|
Exercises

Coupled Analysis of an Integrated Circuit Board

Problem: Bonded joints are used in the design of a circuit board. A change in temperature due to the equipment operation can introduce stresses in joined materials of dissimilar thermal expansion coefficient. In this case we have chip heating due to the applied power, causing thermal gradients in the different materials which, together with the fixed displacements, cause high stresses near the end of the lead frame. The chip dimension is 3.80 mm by 3.80 mm with thickness equal to 0.7 mm. It is mounted on top of adhesive (paste). The outer case dimension is 14 mm by 14 mm by 3.22 mm.
 
Download required files here


































































Step 1 - Enter SimXpert Structures Workspace.

1) Click Structures.



Step 2 - Set the Units.

1) Check in the lower right-hand corner for the current system of units.

2) If the current system of units is not English units (in, lb, s), Select Tools > Options.

3) For Basic Units select: Length = mm, Mass = g, Time = s, Temperature = celsius, Force = N and click OK.



Step 3 - Open Prob8_Analysis_Chaining.SimXpert File .

1) Select File > Open.

2) Select Prob8_Analysis_chaining.SimXpert File.

3) Click Open.



Step 4- Save File as Prob8_coupled.SimXpert.

1) Select File > Save as.

2) Type Prob8_coupled.SimXpert as File name.

3) Click Save.





Step 5 - Create a New Load Case.

1) In the Model Browser, right click on Load Cases and select Create Loadcase.

2) For Name (Title) enter Coupled_analysis.

3 For Analysis Type select Nonlinear Static.

4) Click OK.



Step 6 - Create a Coupled Load Step.

1) Scroll down in the Model Browser, right click on Load Steps and select Create Coupled Loadstep.

2) For Name (Title) enter Coupled.

3) For Analysis Type select Steady State Heat Transfer for Thermal Substeps and Nonlinear Static for the Structures Substeps.

4) Click OK.

5) Right click on LBC Container of the Thermal Substeps.

6) Select Lbc Set.

7) Select Thermal in the model browser LBC set list.

8) Click OK.

9) Right click on LBC Container of the Structures Substeps.

10) Select Lbc Set.

11) Select Structural in the model browser LBC set list.

12) Click OK.

13) Right click on Output Request in the Coupled Loadstep.

14) Select Nodal Output Request.

15) Select Create Temperature output Request.

16) Check suppress Print box on.

17) Click OK.

18) Right click on Output Request in the Coupled Loadstep.

19) Select Nodal Output Request.

20) Select Create Displacement output Request.

21) Check suppress Print box on.

22) Click OK.















Step 7 - Create a Coupled Load Step - Define Output Request.

1) Right click on Output Request in the Coupled Load Step.

2) Select elemental Output Request.

3) Select Create Sol 400 Nonlinear Stress output Request.

4) Select Components of Cauchy Stress and Thermal Strain in the Stress and Strain NLOUT.

5) Select Total Temperature in the Temperature NLOUT.

6) Select Equivalent von Mises Stress in the Equivalents NLOUT.

7) Click OK.







Step 8 - Define Coupled Load Steps Parameters.

1) In the coupled Load Steps, double click on LoadStep Control.

2) Select convergence Criteria for mechanical Analysis.

3) Check Displacement Criteria box on.

4) Set Displacement Tolerance enter 0.01.

5) Check Load Criteria box on.

6) Set 0.01.

7) Check Vector Component Checking Box on.

8) Click Apply.

9) Select convergence Criteria for heat transfer.

10) Check Temperature Criteria box on.

11) Set Temperature Tolerance enter 0.01.

12) Check Heat Flux Criteria box on.

13) Set 1e-5.

14) Click Apply.

15) Click Close.





Step 9 - Delete Thermo-Structural LoadCase.

1) Right click Thermo-Structural load Case and delete it.

Step 10- Modify Job Property.

1) Right click Thermo-Structural and select Properties.

2) Define Prob8_Coupled as job Name.

3) If needed select location to save the files.

4) Click OK.



Step 11 - Perform the Coupled Analysis.

1) Right click Prob8_Coupled.

2) Select Run.



Step 12- Attach the Analysis Results File.

1) Select File > Attach Results.

2) The file path will be, by default, attach the appropriate .op2 file.

3) Click OK.





Step 13 - Display Structural Results.

1) Under the Results tab, click Fringe in the Results group.

2) Select Time = 1 under Result Cases.

3) Scroll down to select Nonlinear Stresses,Stress tensor under Result type.

4) Select Von Mises under derivation.

5) Select Deformation.

6) Select Time = 1 under Result Cases.

7) Select Displacements, Translational.

8) Under Deformation TAB Activate Relative Deformation.

9) Click UPDATE.









Step 14 - Display Thermal Results.

1) Select Time = 1 under Result Cases .

2) Highlight Temperatures under Result type.

3) Click Update.





Step 15 -Save the Database.

1) Select File > Save As…

2) For filename, enter Prob8_Coupled.SimXpert.

3) Click Save.

4) Select File > Exit.







 

Share this page