Pull-in analysis of a MEMS device

Model definition

The model consists of two parallel square plates with certain thickness and are separated by vaccum gap. DC voltage is applied to the bottom plate while the top plate is grounded. The bottom plate is clamped and the top plate is attached to a spring of stiffness $K$ . The displacement of top plate is constrained to move only in the $Z$ -direction. The interaction between the top plate and attached spring is determined using a lumped model:

F_z = -K \cdot U_z

INTRO_pull-in-2D-model

Parameters

The following are the model parameters and these variables will be defined as shared expressions in Allsolve.

Length of the square plate, $L = 50 \, \, \mu m$
Height of the square plate, $H = 3 \, \, \mu m$
Gap between the two parallel square plates, $d = 1 \, \, \mu m$
Stiffness of the spring, $K = 10000 \,\, N/m$
Overlapping area between the two parallel plates, $A = L \times L \, \, m^2$

Geometric element	Size	Center point
Bottom plate	L $\times$ L $\times$ H	[0, 0, 0]
Top plate	L $\times$ L $\times$ H	[0, 0, H/2 + d + H/2]
Vaccum box	L $\times$ L $\times$ d	[0, 0, H/2 + d/2]

Output Results:

Plot of applied voltage vs resulting displacement.

Material Data

Vacuum for the gap between the parallel plates
- Electric permittivity in F/m: $\epsilon$ = $\epsilon_0$
Silicon dioxide for the top and bottom plate
- Youngs modulus in GPa: $E = 70$
- Poissons ratio, $\nu = 0.17$
- Electric permittivity in F/m: $\epsilon$ = $3.9\times\epsilon_0$

Note: $\epsilon_0$ = $\dfrac{1}{\mu_0 c^2}$ = $8.854 \times 10^{-12} \, F/m$

Boundary conditions

Bottom plate
- Electrode : v = $V_{dc}$
- Clamped : $[u_x, u_y, u_z]$ = $[0, 0, 0]$
Top plate
- Grounded : v = $0$
- in-plane clamp : $[u_x, u_y]$ = $[0, 0]$

Note: We will define a shared expression called Vdc in Allsolve and provide a temporary value. Later, this expression can be used to define a simulation sweep which takes a list of different positive voltage values.

Analytical solution

For the above defined model setup, the analytical solution to the pull-in voltage $V_p$ is given by the formula [1]:

V_p = \sqrt{\frac{8}{27}\frac{Kd^3}{\epsilon A}}

where,

$K$ is the spring stiffness in $N/m$ .
$d$ is the initial gap between the parallel plates in $m$ .
$\epsilon$ is the electric permittivity of the gap medium $F/m$ .
$A$ is the overlapping area between the parallel plates $m^2$ .

The corresponding displacement $u_p$ of the top plate at pull-in voltage is one-third of the initial gap between the plates.

x = \frac{1}{3} d

The pull-in voltage and the corresponding displacement based on the values defined in the Parameters section above:

V_p = 365.9 \, volts \\ u_p = 0.3333 \, \mu m

Step-by-step guide

Here you’ll find a step-by-step tutorial on how to simulate this in Quanscient Allsolve

Step 1 - Create geometry

Start with a new project:
Click on box icon under Create a geometry:
For now, click on Confirm model changes and move to the Properties tab, where we will use Shared expressions to define model parameters which can then be used in geometry creation and physics interaction.
In the Properties tab, click on the + icon next to Shared expressions. Provide the following settings as in the image and click on Apply to confirm.
Similarly, create all the following new Shared expressions with the settings shown in the image.
Go back to the model tab and click on the Edit model button and then on box under Geometry elements.
In the GEOMETRIES SETTINGS, modify its size to $L \times L \times H$ . Click on Apply to confirm the settings and then click on Not built to build the modified box. Click on Reset view to fit the geometry to the visualization window.
Now, we create the other parallel plate. Click on the + icon next to Geometry elements and select Translate.
Under the GEO OPERATIONS SETTINGS, click on + next to Target and select volume tag 1. Update the Translation in z-direction to $H/2 + d + H/2$ . Enable the Copy tag and set the Repeat count=1. Click on Apply to confirm the settings and then click on Not built to build the translated object.
To fill the gap between the parallel plates, create another box with the following settings. Click on Apply to confirm.
Click on Confirm model changes to finish model creation process.

Step 2 - Define material

Proceed to the Properties tab to define materials.
Click on the + icon next to Materials and select Vacuum from the list and click Confirm.
Click on Add volume under MATERIALS SETTINGS. Select the middle layer as the target volume from visualization window. Click on Apply. This applies the Vacuum material to the selected volume.
Click on the + icon next to Materials and select Silicon dioxide from the list and click Confirm.
Click on Add volume under MATERIALS SETTINGS. Select the top and bottom layers as the target volumes from visualization window. Click on Apply. This applies the Silicon dioxide material to the selected volumes.

Step 3 - Define the physics and apply boundary conditions

Proceed to the Physics tab to define physics and interactions.
Click on the + icon to add a new physics. Select Solid Mechanics.
To add the target volumes for solid mechanics physics, click on the Add volume under the PHYSICS SETTINGS and select bottom and top layers as shown. Click on Apply to confirm the settings.
Similarly, add the physics Electrostatics and Mesh deformation. The target volumes for these two physics are the whole geometry. If no target volumes are selected, then it defaults to the whole geometry. Therefore, it is not needed to select any target volumes for these two physics.
Now we shall add the interactions to each of the physics. Click on the + icon next to Solid Mechanics and select Clampfrom the list of Interactions. This boundary condition will constraint all components of the displacement vector in the targeted region to zero displacement: $u_x$ =0, $u_y$ =0, $u_z$ =0.
In the INTERACTIONS SETTINGS, click on Add region under Targets and choose volume.
Now, select the bottom plate as the target region and click on Apply to confirm the settings.
The top plate should be allowed to move only in the Z-direction and hence its displacement in the XY plane must be set to zero. This is can be achieved through the Constraint interaction.
Rename the interaction to in-plane clamp. Click on Add region under Targets, choose Volume and select the top plate from the visualization window. Set the $x$ and $y$ constraint value to 0. Disable the $z$ constraint so that it is considered as a degree of freedom and is solved for during the simulation run.
Select the Lump U/F as the next interaction in solid mechanics. We will use this to attach a spring to the top surface of the top plate via circuit coupling.
Click on Add surface in the INTERACTIONS SETTINGS.
From the visualization window, select the top surface of the top plate as the target region. Under Parameters, change the Actutation mode to Circuit coupling. Disable the $x$ and $y$ and set the $z$ component to lump.Fz - (-K*lump.Uz). Click on Apply to confirm the settings.
Now, we proceed to adding interactions for the Electrostatics physics. Click on the + icon next to Electrostatics. Select Constraint from the list of interactions.
Rename it as ground and click on Add region under Targets.
Choose volume as the region to add from the list.
From the visualization window, select the top plate as target volume. Set $0$ as the Constraint value and click on Apply to confirm the settings.
Similarly, add another Constraint interaction for the Electrostatics. Rename it as electrode and click on Add region under Targets. Choose volume as the region to add from the list. From the visualization window, select the bottom plate as target volume. Set Vdc as the Constraint value and click on Apply to confirm the settings.
The Solid mechanics and Electrostatics physics need to be coupled since the regions of solid mechanics experience forces due to electrostatics. This coupling is added by selecting Electric force interaction in Solid mechanics physics.
After clicking on Apply to confirm the coupling interaction, it can be observed that a corresponding Electric force interaction (text appeared as a lighter shade) gets added to the Electrostatics physics. This is only to indicate that the Electric force is a coupling interaction.
Now, we proceed to adding interactions for the Mesh deformation physics. The mesh motion of the top and bottom plates are constrained by the displacement field. Click on the + icon next to Mesh deformation. Select Constraint from the list of interactions.

Note: The voltage difference applied between parallel plates, results in the electrostatic force which pulls the top plate towards the bottom plate. This reduces the vacuum gap between the plates. Therefore, we need to allow for the mesh in the vacuum gap to deform due to displacement of the top plate. The Mesh deformation physics allows for such mesh motion.

Example image

Click on Add region under Targets. Choose volume as the region to add from the list.
From the visualization window, select the top and bottom plates as target volumes. Set the Constraint value = compx(u), compy(u), compz(u) and click on Apply to confirm the settings.
Since this lumped analysis is pseudo-1D, we add a new constraint in the vacuum region such that the mesh motion occurs only in the Z-direction. Click on the + icon next to Mesh deformation. Select Constraint from the list of interactions and rename it as in-plane constraint. Set the $x$ , $y$ constraint value to 0 and disable the $z$ constraint so that it is considered as a degree of freedom and is solved for during the simulation run.
Due to the mesh motion, the electric potential field $v$ must be solved for on the deformed mesh. This is achieved by adding Large displacement interaction in the Electrostatics physics. Click on Apply to confirm.

Note: The Large displacement interaction is generic and versatile. A prior Mesh deformation physics must be added to use Large displacement interaction. This interaction can then be added to any other physics, thereby evaluating the solution of the corresponding field variables on the deformed mesh configuration. However, note that in Solid mechanics physics, the Large displacement interaction indicates geometric nonlinearity.

Example image

The Electric force in Solid mechanics must as well be evaluated on the deformed mesh configuration. Therefore, under this physics we also add Large displacment interaction and click on Apply to confirm. This interaction inadvertently considers geometric nonlinearity in Solid mechanics. We will later see how this can be changed from nonlinear to linear without affecting the electric force.

Step 4 - Meshing the geometry

Proceed to the Simulations tab and add click on + icon next to the Meshes to add a new mesh.
Under the MESH SETTINGS, click on Mesh quality to view the dropdown menu and change the selection from Default to Expert Settings.
Continuing in the MESH SETTINGS, change the Used Mesher to Basic and set the Scale factor = 0.75.
Under the same settings, scroll down to the Mesh extrusion. Click on + icon next to it. Keep the Overlap mode to Prevent. Select all the volumes as the target regions and provide the sublayers count as shown in the image below. Click on Apply & mesh to confirm the mesh settings and generate the mesh.
Once the mesh status changes to Success scroll down to Mesh results under MESH SETTINGS and click on Show preview to see the generated mesh.

Step 5 - Apply simulation settings

Click on + icon next to the Simulations to add a simulation.
Under the SIMULATIONS SETTINGS, in the Analysis Type select Steady state and keep the remaining default settings and click on Apply button to confirm the settings.
Click on Mesh under Simulation 1 and select Mesh 1 to set this mesh for the current simulation.
Click on + icon next to Inputs under Simulation 1. Now select Vdc under Sweeps. This allows us to run a simulation sweep over different values of Vdc.
In OUTPUTS SETTINGS of Vdc sweep, provide a linspace expression as in the image below. This overides the previously given value for Vdc and creates a list of $73$ elements for simulation sweep starting from $5V$ to $365V$ with an increment of $5V$ . The theoritical pull-in voltage was $365.9V$ , hence, a closer but lesser voltage than this is set as the maximum value in the sweep. Click on Apply to confirm.
Click on + icon next to Outputs under Simulation 1. Now select Custom under Value outputs. Rename it as max displacement in um and provide the Output expression as shown. Click on Apply to confirm.
The solid mechanics physics considers geometric nonlinearity due to the Large displacement interaction. It is sufficient to consider geometric linearity for this simulation. To make this change, click on the Script under Simulation 1 and click on Scripting mode.
Click on the Yes button to enable the scripting mode.
In the scripting interface, scroll down to # Solid mechanics and modify the corresponding formulation as shown in the highlighted line of code.
Now click on Simulation 1 and then on Run Simulation button. The simulation status changes from Not run to Running and after completion to Success.

Step 5 - Post-processing of the simulation results

Once the simulation status changes to Success, click on Plotting under Results. Set the Input (x) in X axis to Vdc. For the Value (y) in Y axis, choose max displacement in um.

Note: To visualize the plot, It is not necessary to wait until all the jobs of the simulation sweep are completed. You can already do so after starting the simulation run. Although, wait until at least one of the job is completed so that the output data is available for selection in the Y-axis.The plot gets updated dynamically as when a simulation job has successfully completed the simulation.

Example image

Clicking on Summary opens a new dialog box which contains the tabular data of the voltage sweep. This data can also exported as csv file by clicking on the Export CSV button.

References

[1] Kaajakari, V. MEMS Tutorial: Pull-in voltage in electrostatic microactuators, 1-2. https://www.kaajakari.net/~ville/research/tutorials/pull_in_tutorial.pdf