Spectre Simulations

Spectre Simulations using CMOSP18 RF Models Mohammad Hekmat April 2005

Table of Contents: Spectre Simulations..........................................................................................................................1

TSMC Models................................................................................................................. 2 RF versus other models................................................................................................... 2 How to define an RF device ........................................................................................... 3 1-Setup your model path............................................................................................. 3 2-Modify the Netlist.................................................................................................... 5 3-Run the simulation................................................................................................... 7 4-An example.............................................................................................................. 7

Syntactical Conventions This document uses the same syntactical conventions as Cadence documentation. Menu commands and the fields in dialog boxes in the GUI are given in Arial italic font: File – Save An en dash (–) separates the menu name and the command name. Variables for which you are to substitute a value are given in Courier italic font: Filename, cellname File names and paths are given in Courier font: library.lib Copyright © 2005, Mohammad Hekmat – All Rights Reserved

1

Spectre simulations using CMOSP18 RF Models

TSMC Models TSMC provides three types of CMOSP18 device models for circuit simulations with Spectre. Each of these models is optimized for a certain application. Table 1 lists the name of the model definition files, their location, and their intended application. Model Name

Path1

log018.scs mm018.scs rf018.scs

$CAD/spectre445_logical/ $CAD/spectre445_mixed/ $CAD/t018mmsp001RF/

Application Logic Mixed-signal High Frequency (RF)

Table 1: Different models and their applications

Equivalent models are available for HSpice simulations in Cadence. Furthermore, TSMC also provides equivalent Mixed-signal and RF models for simulations within Agilent's ADS. You can expect to obtain the same simulation results using either tool (ADS or Cadence). Using the CMOSP18 RF models in the ADS graphical environment is straightforward since you simply select RF MOS transistors from the TSMC library. This is similar to the way the Logic and Mixed-signal models are used with Cadence’s Schematic Editor. However, this is not the case for the RF models in Cadence’s Schematic Editor, where CMC’s current setup does not provide graphical interface support for the RF models. This interface support can be created by modifying the CDF parameters of the instances in Cadence; however, here we assume that no configuration change in Cadence is possible. Instead, in this document, we describe an alternate and simple work-around to this problem. We assume that the user has chosen Spectre as the simulator for his circuit. A similar procedure can be followed for HSpice or SpectreS simulations.

RF versus other models All TSMC’s models use BSIM3v3.2 for device definition; however, the assigned model parameters are slightly different in different models because they are based on physical process measurements taken at different frequency ranges. Furthermore, the difference between the RF and mixed-signal models is more than just a difference in parameters. In RF models the basic transistor is replaced with a subcircuit composed of the intrinsic transistor surrounded by a few parasitic elements such as resistances and diodes2. These parasitic elements are mostly responsible for those effects that BSIM model does not take into account and can significantly affect simulation results. As an example, the simulated noise figure of a sample LNA using both mixed-signal and RF models is shown in Fig. 1. The considerable difference in the results comes from the contribution of gate, source, drain, and substrate parasitics that are absent in the Mixed-signal models. 1

Throughout this document $CAD is used instead of : /CMC/kits/cmosp18/models/spectre 2 For more details of this subcircuit see: TSMC 0.18um Mixed Signal 1P6M Salicide 1.8V/3.3V RF Spice Models, Document Number: T-018-MM-SP-001 Can be found in: /CMC/kits/cmosp18/doc/CMOSP18elecRFParams.pdf

2

Spectre simulations using CMOSP18 RF Models

(a)

(b) Figure 1 : Noise figure of a sample LNA using (a) mixed-signal, and (b) RF models

Another important point is that TSMC’s RF models are built based on measurements at frequencies up to 20GHz for transistors of 2.5µm length. As such, the gate width of RF transistors in the model is fixed to 2.5µm and cannot be changed. The user can modify the number of fingers but not the width. This is an important consideration in drawing the final layout of the circuit.

How to define an RF device 1-Setup your model path Draw the schematic of your circuit the same way as any other schematic in the Schematic Composer window of Cadence. Once the schematic view of your circuit is drawn and you

3

Spectre simulations using CMOSP18 RF Models are ready to simulate your circuit, use the following steps to define an RF model for your device: -In the ADE3 window choose Setup-Model Libraries. The Model Libraries Setup menu will open. In the Model Library File field add: /CMC/kits/cmosp18/models/spectre/t018mmsp001RF/rf018.scs

-In section part type: tt_rfmos4. -Click on Add button. Notice that clicking on OK will not add the model to the path. The final menu looks like Fig 2.

Figure 2 : Setting the model path

Note that you do not need to include the top line i.e. the path to mixed-signal models is not necessary; however, having both models in your path enables you to use different models for different parts of your circuit e.g. you can use RF models for critical parts of your design and mixed-signal models for the rest. Nonetheless, remember that RF models are not in general as accurate as mixed-signal models unless you are specifically looking for RF performance and as discussed before, the use of these models imposes some limitations on the width of the transistors in your design. An alternative way to setup your model libraries is to manually modify the model library definition file icfspectre.init. This file is located by default in the $CAD/ directory where you are not allowed to modify it. In order to modify the file, copy icfspectre.init to a folder in your home directory, and then modify it by simply adding the following line: 3 4

ADE stands for Analog Design Environment, previously known as Analog Artist. Other process corners can be used by replacing tt_rfmos with ss_rfmos, ff_rfmos, etc.

4

Spectre simulations using CMOSP18 RF Models

include "$CAD/t018mmsp001RF/rf018.scs" section=tt_rfmos

Then, go back to the Model Library Setup, and in the Model Library File field add: $PATH$/icfspectre.init.

Either of these two methods will include the RF library to your models path.

2-Modify the Netlist So far your model path is set up for RF models, but still Spectre will not simulate the circuit correctly. So, the final step is to generate and edit the netlist of your circuit. Since the netlist is a text file you can edit it using any text editor e.g. emacs. If you do not know the path to the netlist, run the simulation once and choose Simulation/Netlist/Display in the ADE window5. A new window will pop up and the current netlist will be shown. The path is shown in the top window bar. It should be similar to the following path: $Simulation-Directory/spectre/schematic/netlist/input.scs

Note that although this file contains netlist information it is NOT the netlist file you need to modify. This input.scs file is created every time you simulate your circuit by combining information from the netlist file, and the simulation control and analysis statements that result from your selections in the GUI. Note that in contrast, the standalone netlist file, which contains only information about the electrical components and their connections, is generated/updated only if you choose the Simulation/netlist and run or Simulation/Netlist/Create or recreate in the ADE. The actual netlist that we need to modify is located in the same directory and its name is netlist: $Simulation-Directory/spectre/schematic/netlist/netlist

Before simulating the circuit, Cadence’s ADE prepares the netlist of the schematic view drawn in Schematic Composer Window. The parameters assigned by the user in the object properties dialogue box appear in the netlist as instance parameters. It is the task of ADE to compose the appropriate netlist based on the schematic symbols i.e. whenever an instance of an NMOS transistor is used in the circuit; the ADE will automatically add the proper device definition to the netlist (the proper format is chosen based on library definitions and the model path). However, the current version of CMOSP18 libraries available from CMC does not support this feature for RF models; therefore, it is the designer’s task to edit the netlist so that the correct model definition is used. If you do not change the netlist manually the simulation will most probably be done without issuing any error messages; however, the results will not be correct because some device parameters are missing for the simulation. To understand why and how the parameters should be changed, here is the heading of the subcircuit definition in the rf018.scs file: 5

Or if you just want to create the netlist use: Simulation/Netlist/Create

5

Spectre simulations using CMOSP18 RF Models

subckt nmos_rf ( D G S B ) parameters lr=18.e-08 nr=12.8e+01

As can be seen this subcircuit has four nodes and two parameters that should be set by the user. The four terminals of the transistor require no change by the user, but the other two parameters namely nr and lr should be adjusted. nr is the number of fingers and lr is the length of the MOS device. Note that for a mixed-signal model there are a couple of parameters such as the area and periphery of diffusion regions and so on; however, in RF library, all these values will be automatically set by the TSMC model and are assigned internally in the subcircuit definition of the RF model and need not be set by the user. In order to correct the netlist, remove all parameters of the MOS devices except the terminal connections and add two parameters: ‘nr’ and ‘lr’. As an example the netlist of the LNA simulated in Fig. 1 before and after modification is shown here: Original Netlist Prepared by Cadence: // Library name: LNA // Cell name: LNA_CMC1 // View name: schematic PORT0 (net9 0) port r=50 num=1 dc=600m type=sine PORT1 (net3 0) port r=50 num=2 type=sine C1 (net17 net5) capacitor c=10.1p C0 (net17 net3) capacitor c=1u V0 (net5 0) vsource dc=1.8 type=dc L2 (net17 net5) inductor l=1n L1 (net9 net13) inductor l=38n L0 (net16 0) inductor l=450.00p M0 (net21 net13 net16 0) nch w=2.5u l=180.00n as=0.48u*(2.5u) \ ad=0.48u*(2.5u) ps=0.96u+2*(2.5u) pd=0.96u+2*(2.5u) \ nrd=0.27u/(2.5u) nrs=0.27u/(2.5u) m=60 region=triode M1 (net17 net5 net21 0) nch w=2.5u l=180.00n as=0.48u*(2.5u) \ ad=0.48u*(2.5u) ps=0.96u+2*(2.5u) pd=0.96u+2*(2.5u) \ nrd=0.27u/(2.5u) nrs=0.27u/(2.5u) m=60 region=triode ----------------------------------------------------------------------Modified Netlist of the LNA: // Library name: LNA // Cell name: LNA_CMC1 // View name: schematic PORT0 (net9 0) port r=50 num=1 dc=600.0m type=sine PORT1 (net3 0) port r=50 num=2 type=sine C1 (net17 net5) capacitor c=10.1p C0 (net17 net3) capacitor c=1u V0 (net5 0) vsource dc=1.8 type=dc L2 (net17 net5) inductor l=1n L1 (net9 net13) inductor l=38n L0 (net16 0) inductor l=450.00p M1 (net17 net5 net21 0) nmos_rf lr=180.00n nr=60 M0 (net21 net13 net16 0) nmos_rf lr=180.00n nr=60

Note that the only difference is in MOS definition part.

6

Spectre simulations using CMOSP18 RF Models

3-Run the simulation There are two options in the simulation menu of Analog Environment. One is “Run” and the other one is “Netlist and Run”. The latter generates netlist prior to simulation. After performing the netlist modification the “Run” option should be used in Spectre otherwise the new netlist will overwrite the one you have already edited. To make sure that the correct netlist is being used choose Simulation/Netlist/Display in ADE window and inspect the input.scs for changes you have made. Note that after the simulation, you might get some warning messages in your output log regarding the length and width of the transistors, these messages can be ignored.

4-An example As an example of the procedure described, we will use the netlist given in this document and compose a schematic for a sample LNA. Create the following schematic6.

Figure 3: The schematic of the sample LNA

6

For further information about how to create new cellviews and schematics refer to other tutorials available on CMC’s website e.g. Tutorial on schematic entry and digital simulation at: http://cmc.ca/prod_serv/education/training/

7

Spectre simulations using CMOSP18 RF Models

The list of elements and their corresponding libraries is given in Table 2. For any parameter not given in this table use default values. Part L0 L1 L2 C0 C1 Port0

Library analogLib analogLib analogLib analogLib analogLib analogLib

Instance name ind ind ind cap cap port

Port1

analogLib

port

V0 M0

analogLib cmosp18

vdc nfet

M1

cmosp18

nfet

Value 450pH 38nH 1nH 1uF 10.1pF Resistance=50 Ohms Port number=1 DC voltage= 600mV Resistance=50 Ohms Port number=2 1.8v Multiplier=60 Width=2.5um Multiplier=60 Width=2.5um

Table 2: Value of parameters for te sample LNA

In the ADE window choose Spectre as simulator (You do not need to change anything, usually, the default simulator is Spectre). Choose SP analysis and make sure to enable noise analysis. Set the frequency range to 1-2GHz. Once you enable noise analysis you have to select output and input ports. Select Port1 and Port0 for output and input ports, respectively. Click OK and run the simulation. Once the simulation is complete, in the ADE window choose Results/Direct Plot/ Main Form. The direct plot form will open. In this form choose NF and dB10 and finally click on plot. Fig. 2a will be shown in the Waveform window of Cadence. Modify the netlist created by Cadence following the steps shown in this document. Resimulate the circuit after setting model paths (As described before, do not use Netlist and Run just Run). This time you will see Fig. 2b in the waveform window. Both original and modified versions of the netlist are given in the previous section. As a final note, one might think what happens if one simply changes the model name for the NMOS transistor to nmos_rf and set the model paths to RF libraries without modifying the parameters in the netlist. Obviously, as you have understood throughout this document, the simulation results will not be correct. However, Spectre simulates your circuit even though the parameters are not correct. You will get a couple of warning messages stating that Spectre has ignored anything that it could not understand. A sample result is shown in Fig. 4, which is obviously wrong.

8

Spectre simulations using CMOSP18 RF Models

Figure 4: A sample simulation result that can occur due to ignoring some of the design parameters

9