Learn how to perform a thermal-structural analysis in Simcenter 3D. Take advantage of Simcenter multidisciplinary capabilities to greatly simplify the workflow for PCB analysis.
- PCB warpage under thermal loads
- Thermal-structural analysis typically requires different tools/environments to be used
- Learning curve prevents engineers from mastering different environments
- Single environment (CAD-thermal-structures) simplifies learning curve
- Integrated environment shortens analysis cycle
- Multidisciplinary capabilities enable engineers to capture all applicable physics
- Synchronous modeling enables design exploration
Thermal Analysis of PCB
In this technical blog we will be performing a thermal-structural analysis of a PCB. In designing PCBs, thermal effects must be considered. Thermal analysis enables engineers to identify regions of poor thermal management. These may be good areas of design iteration and improvement. Simcenter 3D makes iteration easier by combining multidisciplinary tools in a single environment. This is shown in the graphic below. The simulation (*.sim), modeling (*.fem), and geometry (*.prt) data is readily available to the user so changes to geometry can be made easily and propagated effortlessly. The solution environment also makes it easy to carry data from one solution to another by allowing users to add different solution sequences in the same environment (thermal, structural, dynamics, etc.).
Simcenter 3D unified modeling environment
Before we can improve on a design, however, we would like to establish a baseline. To do this, we will start by performing a thermal analysis.
Setting up a thermal analysis in Simcenter 3D is quite simple. To begin, a PCB was created in NX. The resulting board is shown below.
PCB created in the modeling environment of Simcenter 3D
The board features several prominent components, including a chip with a heat sink that includes pin-shaped fins. This chip will be the primary source of heat generation in the analysis. We would like to see the warpage of the PCB under the thermal strains resulting from this heat generation.
The next step is to create a mesh of the above PCB. Since the geometry is simple, no defeaturing was required. A simple TET mesh was created and is shown below.
3D TET mesh of PCB
Simcenter 3D simplifies meshing by allowing us to use mesh mating conditions to match meshes across interfaces. Mesh mating conditions were used to connect each board component to the board itself. Orthotropic material properties were assigned to the PCB, while isotropic properties were used for all the chip components. The material properties are summarized below:
Material properties used in thermal-structural analysis. Left FR4, orthotropic. Right, chip isotropic properties.
The next step is to define the thermal loading boundary conditions in the simulation module. A heat generation boundary condition of 1.5e-2 W/mm3 was applied to the chip. Forced convection (i.e., externally forced air using fan) was assumed on the fins of the heat sink with h = 5e-5 W/mm2-°C and T=22°C. Finally natural convection (naturally occurring fluid motion) was applied to all other component surfaces with h=5e-6 W/mm2-°C and T=22°C.
Boundary conditions – natural convection (yellow), forced convection (blue), heat generation (red)
Solution 153 (steady state nonlinear heat transfer) was used for the analysis. The nodal temperature results for this simulation are shown below.
Nodal temperature results for thermal analysis
Structural Analysis of PCB w/ Thermal Loads
Now that the temperature field for the PCB has been determined, a structural analysis can be used to determine the warpage of the component as well as thermal strains and stresses.
To perform the structural analysis with thermal loads, we need to do a few things: 1) set up a structural simulation, 2) define structural boundary conditions, 3) apply temperature results from the previous step to the model.
To start, we will create a simple linear static analysis in the simulation model (SOL 101). With that defined, we can go ahead and define our structural boundary conditions. To do this, we will define a cylindrical coordinate system at each bolt hole and constrain UR, UZ, and all rotations as shown below. This boundary condition is designed to emulate a standoff.
UR, UZ, and all rotations constrained at bolt holes to simulate stand-offs
Finally, we need to apply the temperature solution from the thermal simulation to our solution. One way to do this is to use a field. The result of the mapped temperature field is shown below. Notice that the contour matches the temperature field from the thermal simulation very well. Fields allow us to easily map results from one solution to another, even if the meshes between the two solution sequences are different.
Mapped temperature field applied as load to structural solution
With the temperature field defined, the solution can be run.
Let’s start by looking at the displacement results.
Displacement results of thermal-structural analysis
We can see a peak deflection of about 0.23 mm and a small amount of warpage, which is within acceptable limits. We can also look at the stress results.
Stress results (top: von-mises stress, bottom: worst principal stress)
The stresses are greatest at the bolt holes and are less than 27 MPa (4 ksi), which is acceptable for FR4 material.
One of the amazing things about Simcenter 3D is synchronous modeling. Although the above design is satisfactory, we could easily investigate other design options (positions of chip components, holes, etc.), fin geometry, etc. As an example, we can move one of the holes as shown below:
Using synchronous modeling to move bolt hole on PCB
Once we move the hole, we can go back to our FEM, and click update as shown below:
Updating FEM modified using synchronous technology
With a few minor updates to boundary conditions, we have results in less than 10 minutes of work (including solution time)!
Worst principal stresses for PCB with modified hole location
While this change may seem trivial (moving a hole), imagine the power of this technology to enable innovation and design space exploration.
In this technical blog we used Simcenter 3D to perform a thermal-structural analysis on a PCB. The tools within Simcenter 3D made this straightforward and allowed us to leverage a single user environment during the whole process. Synchronous technology was also leveraged to investigate bolt hole positioning options. If you would like to learn more about synchronous technology, Simcenter 3D, or thermal-structural analysis, please contact us!
Written by Vitaliy Rezekulov
Vitaliy Rezekulov is a Senior Engineer with a background in structural analysis. He has worked on some interesting linear and nonlinear problems. Outside of work he enjoys spending time with his family and friends.