Cadence Virtuoso Simulation of a pixel

Transcription

1 MEMS AND MICROSENSORS 2018/2019 Cadence Virtuoso Simulation of a pixel 11/12/2018 Giorgio Mussi giorgio.mussi@polimi.it Introduction In this lab, we will use Cadence Virtuoso to simulate a sub-array of 4 pixels of a 3T CMOS image sensor. We will learn how to launch Cadence Virtuoso, how to use the Schematic Editor to add instances in our circuit, and how to use the Analog Design Environment (ADE) to run simulations. We will first place the components from scratch, using the Schematic Editor. Then, we will open a preconfigured schematic and we will use the ADE to simulate it. The pre-configured schematic contains 4 pixels that belong to 4 different rows of the same column of a CMOS image sensor used for 25-fps video acquisition. The readout method is based on the rolling shutter architecture. With the help of the ADE, we will be able to evaluate: the full-well charge (the maximum photocurrent), and its limitation due to DC voltage drops; the non-linearity related with the depletion capacitance of the photodiode; timing issues related with the readout of a matrix of pixel. Used models will be ideal: unfortunately, we do not have access to a Process Design Kit (PDK). Hence, some simulation details will be inaccurate due to the non-accurate modelization of the devices. In addition, the lack of the PDK does not allow us to layout our pixel, as there s no layout associated with our ideal components.

2 Environment Setup Linux Environment Setup As first step, you need to start the Linux environment where Cadence Virtuoso tools are installed. Open virtualdesktop in your web browser: and log in with your Polimi account. Open NX Client, and wait until the Linux environment opens. Once the environment is ready, you will be able to launch Cadence Virtuoso.

3 Library Import Before starting to use the software, you need to import a library required for simulations. The library is a compressed file that contains the model of the transistor. You need to extract it in the proper folder. Open Firefox (in Linux, not in Windows), browse to ftp://ftp.elet.polimi.it/outgoing/giacomo.langfelder/mems_and_microsensors_fem_modes_videos/e18/. Click on MEMIS16.tar, to download the file. Save it (do not open it) in your Download folder. Move the downloaded file into your Home folder (/data/home/guest0xxx).

4 Open the Linux terminal: Applications > System Tools > Terminal. Type tar -xvf MEMIS16.tar and press enter. The file is now extracted. Check your Home folder. You should now find a folder named MEMIS16. Cadence Virtuoso Launch Now you can launch Cadence Virtuoso. Open the Terminal, type virtuoso.sh and press ENTER. Cadence Virtuoso should start. The opened window is called CIW (Command Interpreter Window). Close What s New tab.

5 Now you need to add the imported library (MEMIS16) to Cadence Virtuoso. Open the Library Manager, the tool where you can manage your designs: from the CIW, Tools > Library Manager. The Library Manager window will appear.

6 From the Library Manager, Edit > Library Path. A Read Only File pop-up appears, press OK. Add the library: in the Library Path Editor window, Edit > Add Library. Browse through your Home folder (/data/home/guest0xxx), using the drop-down menu.

7 Select MEMIS16 Library and press OK. A new library, in blue, will appear in the Library Path Editor.

8 Save the library definition list. From the Library Path Editor, File > Save As. In the Files To Save section, click on BROWSE Change the path to your Home. You can find it on the left-most side of the window. Press SAVE, then OK.

9 You should now find the MEMIS16 library as the first entry in the Library column of the Library Manager. You are ready to use Cadence Virtuoso.

10 Schematic Entry We are ready to design our pixel. To open a new schematic cell, from the Library Manager, first click on MEMIS16, then go to File > New > Cell View. The library is MEMIS16. Name the cell pixel. Check that schematic type is chosen. Every time a license pop-up appears, click Always. The Schematic Editor is now open.

11 You can use ftp://ftp.elet.polimi.it/outgoing/paolo.minotti/mems_and_microsensors/e19/cadence-seshortcuts.pdf as a reference for schematic entry shortcuts! As first instance, place the photodiode. Press I (keyboard shortcut), then browse to ahdllib > diode_sch. Click CLOSE. Set the parameters of the diode as shown. area is the area of the photodiode: name it as L*L, assuming a square photodiode, whose side is L. is is the dark current density. cjo is the depletion capacitance density.

12 Once all the parameters are correctly entered, click Hide. You can use either scientific or engineering notation. The engineering suffix should be placed right after the number, with no space. Hence, 10u is 10 micro and 20K is 20 thousands. If you enter a number with decimals, e.g. 0.5, always double check that between the 0 and the 5 there is a dot and not a comma. If you don t write a number as an entry, but you use a variable, e.g. L, you can defer to the simulator (ADE) the choice of the value of that parameter. Before placing the instance in your schematic (by just clicking with the left button of your mouse), press R twice, so that you rotate it, thus having the cathode above the anode. Place instances not too close one each other; this will make the visualization of your schematic easier. While placing an instance, if you press F3, a pop-up appears; you can change the properties of the instance you are adding, e.g., you can change the orientation, you can flip it If you want to stop a command from being active, press Esc. If you want to change the properties of an instance, click on it, then press Q. The model of this photodiode includes the depletion capacitance non-linearity.

13 Place the photocurrent generator, a current source: press I, then browse to analoglib > idc. Put iph1 as DC current. When you enter a value, do not write the unit (m, V, A ): it will be updated automatically.

14 Place the supply voltage source: press I, analoglib > vdc. Insert 3 as DC voltage. Place the reset signal generator: press I, analoglib > vpulse. Insert the parameters as below. tfr is the inverse of the frame rate: how often are we taking a picture, i.e. how often are you resetting the pixels? tdelay is the reset delay. Assuming a rolling shutter readout technique, this is the first pixel that will be reset, i.e. delay is 0. If you have more than one pixel on the same column, the second one will have a 1*tdelay delay, the third one will have a 2*tdelay delay, and so on treset is the reset time interval, during which the reset transistor is kept closed.

15 Place the three transistors, with minimum size, 350 nm: press I, MEMIS16 > mos_level2. Insert the parameters as below. Place three of them: reset switch, source follower, row-selection switch. Rotate them as shown.

16 Place two capacitors: press I, analoglib > cap. You need to place two capacitors, because the model of the MOS transistor in MEMIS16 library does not include parasitic capacitances. You need to add a capacitor from the integration node to ground, and a capacitor from the gate to the source. Use CT as the value of the capacitance to ground, and 10a as the value of the gate-source capacitance. Place the row-selection voltage signal. You can copy the reset generator, as their properties will be similar. Click on the reset voltage source, press C, click to select the reference point for copy, then click to select the destination point for copy. Place the vpulse instance below the gate of the row-selection transistor. Select the just-added vpulse instance, press Q. Change its parameters as below. You need to change the delay time, i.e. when we want to readout this pixel: you need to wait treset, then tint (the integration time), then 0*tdelay as this is the first pixel that will be read out. If you have other pixels in the column, they will have a constantly increasing delay time. treadout is the readout time, i.e. the time the row-selection switch is closed.

17 Place the DC current source that will bias the source follower when the row-selection switch is closed: press I, analoglib > idc, and use 2u as DC current. Finally, below everything, we can place the ground instance, that defines the zero-volt potential: press I, analoglib > gnd. Now you need to properly connect all the instances. Follow the diagram below. You should connect the instances through wires (shortcut W), and connect the proper terminals together. If you want to start a wire, press W. If you want to stop placing wires, press Esc. If you want to suddenly end a wire, double tap the left mouse button. Remember to connect the bulk of the transistors with the source. In this lab, body effect is not simulated, but if you leave the bulk un-connected, any simulation will fail. The final schematic is shown in the next page.

18

19 Simulation For sake of simplicity, we will simulate a pre-configured schematic, so that we are sure that everything is set up properly. Always Check and save your design before running any simulation. From the Library Manager, select the 4pix cell in MEMIS16 library, and open the schematic view.

20 The schematic will open. In blue you find the net labels. They are used both for connecting terminals, without the need to connect them with a schematic wire, and for simulation outputs referencing. You will find 4 pixels. Imagine that they that belong to the same column of a CMOS image sensor.

21 Using the right button of the mouse, you can zoom on the pixel at the bottom, which is basically the same structure you designed in the Schematic Entry section.

22 Analog Design Environment Setup You can launch the Analog Design Environment, and load a pre-configured simulation state. From the Schematic Editor, Launch > ADE L. An empty ADE appears.

23 Load the pre-configured simulation state: from ADE window, Session > Load State. A window appears. In Load State Option (upper section of the window), select Cellview, then press OK.

24 The ADE window is now populated. Three different tabs are present: Design Variables, Analyses, Outputs. Design Variables In this tab you can easily change the parameters of your circuit before running any simulation. E.g., you can change the photocurrent of the first pixel (iph1), or you can change the size of the photodiode (L). fr Frame Rate [Hz] tdelay Delay time between subsequent rows (with a rolling shutter readout) treset Reset duration treadout Readout duration CT Parasitic capacitance between the integration node and ground L Size of each photodiode, so that Area = L^2 tint Integration time iph1 Photocurrent of PIX1 iph2 Photocurrent of PIX2 iph3 Photocurrent of PIX3 iph4 Photocurrent of PIX4 tfr Frame Period [s]; tfr = 1/fr Analyses In this tab you can choose the type of simulation. In our case, we will run (i) a DC simulation, that will compute the DC voltages and the DC operating points of the circuit, and (ii) a TRAN simulation, that computes the response of the circuit as function of time. Outputs In this tab you can choose which variables/parameters/expression will be automatically evaluated/plotted after running any simulation. You can select them by selecting the corresponding Plot tickbox.

25 Run & Analysis Single-pixel analysis Tick all pixel1-related outputs. Press Play Button, on the right side of the ADE, to run the simulation.

26 Selected outputs are displayed in a graph. If you want to zoom in xy mode, use the right mouse button. If you want to zoom in x (horizontal) mode, press X, then use the right mouse button. If you want to zoom in y (vertical) mode, press Y, then use the right mouse button.

27 From ADE window, Results > Annotate > DC Node Voltages. Then, Results > Annotate > DC Operating Points. In the Schematic Editor, all terminals will have their DC (bias) voltage annotated. Which is the value of the DC voltage at the integration node (PIX1)? Which is the value of the DC voltage at the source of the source follower (OUT1)? Note that DC voltage of SEL1 was set to 3 V.

28 Maximum photocurrent You can set up a parametric sweep on iph1, e.g. from 1 aa, to 1 pa, to evaluate the maximum photocurrent. Tick PIX1 and OUT1. From ADE window, Tools > Parametric Analysis. Parametric Analysis window appears. In Add Variable box, select iph1. As start point, type 1a. As End Point, type 1p. As Total Steps, type 7. Press Play (in Parametric Analysis, not in ADE). The outputs are displayed in a graph. Size and/or adjust the window for better visualization. After running a parametric sweep, click on the + icon on the left-most side of the waveform window to browse through the different sweeps.

29 As expected, the higher the photocurrent, the higher the slope. For iph = 1 pa, the pixel is saturated. Note that the integration time was set to 15 ms. Saturation should be avoided within 15 ms, not 40 ms (40 ms = 1 / 25 Hz = 1 / 25 fps). Re-run the simulation, now from 40 fa, up to 400 fa. Which is the maximum photocurrent? It is enough to look at PIX1 to evaluate it? Which is the maximum voltage variation of the integration node?

30 Non-linearity We can run a parametric analysis on CT, to evaluate non-linearity effects. Tick PIX1 and OUT1. Set iph1 to 60f. Open the Parametric Analysis tool. In Add Variable box, select CT. As start point, type 1a. As End Point, type 10f. As Total Steps, type 6. Does the gain change when you change the parasitic capacitance value? Does the linearity of the photocurrent integration increase?

31 Timing & matrix readout Set iph1 to 10f. In ADE, tick all the outputs. Press Play in ADE window, to run the simulation.

32 Layout Here, some examples of a pixel layout. 64x64 matrix

33 High-density matrix