Gm is broadly used in analog design techniques. Gm can be noted or plotted very easily.
Finding out gm for hand calculations at a given operating point
Perform simple dc and transient analysis of a schematic comprising of a transistor of required W/L and applied Vds and Vgs. Now there are two ways to find out gm of the transistor at the specified operating point.
1. In Analog Design Environment (ADE) click Tools > Result Browser. In the browser window select do-to-dc and select for transistor from the list and see its gm from the list of given parameters.
2. In ADE click Results > Direct plot > Transient operating point. Now screen goes to the schematic. click on the transistor. window opens. scroll to see gm. gm/id is also mentioned as gmoverid. Various model parameters can also be seen by selecting Model Parameters from Dirent plot and select any device.
Plotting gm and gm/Id
Use the same circuit designed above with a transistor and suitable bias voltages.
By default spectre doesnt save the operating point of the devices to keep the psf file slim. however we can force spectre to save all the operating points. Follow the below steps to do this.
1. Make sure spectre is being used as the simulator.
2. create oppoint.scs from our favourite editor and save it in your cadence work directly. make sure you have write permission to this directory. In the oppoint.scs file write this
here N0 is the instance name of the NMOS transistor used in the schematic. We can find out more about command save from spectre user guide.
3. now click ADE -> options -> select waveform tools : AWD
4. now sweep Vgs of the transistor and hit netlist and run in ADE
5. go to the result browser as: ADE > tools > result browser, then, schematic->psf/ -> Run 1 -> DC to DC -> N0, this gives the DC operating points saved.
6. Right click Gm and get the gm plot
7. Add this file as a model library file just like what you usually do to setup Spectre. Make sure the path to oppoint.scs is correct. It is important to note that AWD was used as the waveform tool instead of wavescan.
8. Go to ADE and click menu session, then save script. A window will pop up and that is the first OCEAN script you are going to use. Please note that this ocean script file will be saved in your default cadence directory. From the script file, you can find out that all these setups you made
for simulation in here. OcnWaveformTool set the wave viewer to AWD. Command Simulator selects Spectre as the simulation engineer, so on and so forth.
You have to add few lines to this simple script file to save the DC operating point parameters you are interested in (copy this text exactly):
ocnPrint(?output “~/gmid.dat” ?numberNotation ‘scientific
Here, ?output means all data will be saved to a file called gmid.dat. You can modify the tag line “~/gmid.dat” in order to have the gmid.dat file saved any directory of your choice; otherwise the gmid.dat file will be saved in your root directory. getData selects the parameter you want to save.
9. Now you can load this file and run the simulation again from CIW window by typing:
10. Go to the root directory (or where ever you saved the file) and you can find “gmid.dat”. All the parameters you want, gm, Cgs, Id, Vdsat (Defined as vd) are saved here.
11. Plot the required curves using any scientific program like MATLAB.