Needs BJT for simulation in Cadence

cadence schematic pnp beta

I need NPN and PNP to simulate a small circuit in cadence
So I am searching for BJT models for simulation

In analoglib, there are pnp and npn transistors, and I've added them in my schematic and runned simulation. But the simulation was not sussessful and it shows error messege "Q1 is an instance of an undefined model npn"

In general, is it possible to use the NPN and PNP models from analoglib for simulation?

Or there is something wrong with my cadence installation or settings?

bjt pnp npn circuit

Your BJT model depends on the technology you are using.

If your process is AMI the foundry does not provide BJT models for the parasitic devices so you'll have to fabricate them, characterize them and then build your own models.

If your process is TSMC the DO provide the models for both vertical and lateral BJTs but you need to attach the model to your simulation (just as you usually do it for MOSFETs).

If you don't have any process, but you just want to... I don't know... randomly simulate a BJT just creat a simplified model using a Text editor and specify the value for Is (saturation current), Bf (Forward current gain) and n (The Vthermal correction factor) and then attach your model to the simulation

MAKE SURE THAT: your model name has exactly the same name given in the virtuoso component.

If you have any further questions just let me know,

diemilio

design bipolar transistors cadence

diemilio said:

. randomly simulate a BJT just creat a simplified model using a Text editor and specify the value for Is (saturation current), Bf (Forward current gain) and n (The Vthermal correction factor) and then attach your model to the simulation

Click to expand...

This sounds very interesting, but I've never done this by myself before.

could you please explain me more details or give me an example, how does a model file look like and how can I attach this self-written model file to cadence?

thanks

undefined model of pnp

Hello katrin,

I'm gonna try to explain the steps one by one.

First Instance your BJT in the virtuoso schematic window (you can take it from the analoglib if you want), then go to the element's properties and notice that there is a property called "Model Name"... this is going to be the name you are going to give to your model (obviously). For that property you can specify whatever you want... let's say for example vpbjt (to denote that it is a vertical PNP BJT). Once you're done putting together the rest of your circuit yo need to start ADE to simulate your circuit. Before you can simulate though, yo need a model for your device, so open a blank text file and write:

.MODEL vpbjt PNP ( LEVEL = 1
+ Bf = 10 Is = 1e-17 n = 1)

Then close and save the file with whatever name you want (try using .m extension to denote that is a model file)

This file creates a model for an PNP called vpbjt with a Beta of 10, Is of 1e-17 and n of 1.

Once you're done with this go back to ADE and from the top menu select:

setup --> Model Libraries...

Find the file you just created and add it to the list. Once you're done, press OK and you're good to go.

Hope this helps,

diemilio

an undefined model pnp+cadence

thanks very much, it worked!

But by the way, could you please give me some example of more complicated and accurate model file? or could I find it somewhere in the Internet?

I've just used the simple model file which you wrote. But the circuit I built has convergence problem with the simulation, but it can be because of the circuit itself.

npn model name cadence

As I told you before these models depend on your foundry so there's no use on taking a random model for simulation. If your circuit is not going to be fabricated and you just want to do some conceptual simulations, then the model I gave you is good enough.

Now, if you want the model just to play around with it I can give you one I found searching the web but... first, it's an HSPICE model, so if you're using spectre it won't work, and second... I have NO idea for what technology that model is so it will be very very difficult to figure out the dependency of each parameter with respect to the device's dimensions.

regards,

diemilio

how to simulate a circuit in cadence

Hello evryone, these days I'm also simulating a circuit with npn and pnp necessary. The software I used is Cadence and the language is spectre. I wonder if the model file gave above was in SPICE. How could I use it in spectre?
Thanks in advance for any help.
Best regards,jqjqjq

Hi diemilio,

Do you know what is the format if I want to create a pnp model for spectre?

Thanks,
Mario

diemilio said:

As I told you before these models depend on your foundry so there's no use on taking a random model for simulation. If your circuit is not going to be fabricated and you just want to do some conceptual simulations, then the model I gave you is good enough.

Click to expand...

not sure if that's entirely true. In my case, I don't have a particular process tech in mind but I am interested in seeing what second-order effects will do to my circuit, since it is of an experimental nature. I am just exploring ideas working with bipolar devices in extremely low current regimes (1nA). Can't simulate that with a level 1 spice model.

Anyone have a non-HSPICE model? I am using spectre...

You have to give the analogLib npn or pnp a model name property.
Then you have to force the Spectre include-chain to read in a
file that establishes that model. Either by messing with PDK init
files, or explicitly in the Setup > Model Libraries file list.

I have taken vendor PSPICE models and with a little fiddling
they work fine attached to analogLib instances.

solis365 said:

Anyone have a non-HSPICE model? I am using spectre...

Click to expand...

Find here several pnp models!

erikl said:

Find here several pnp models!

Click to expand...

Thanks, I will put those to good use.

What about complimentary NPNs? does anybody have them? my circuit needs both, unfortunately.

solis365 said:

What about complimentary NPNs? does anybody have them?

Click to expand...

Sure; a lot of people have them. But the process-dedicated models are mostly confidential. It would be easier to help you if you'd tell more exactly what you need. Which process size, lateral or vertical, dedicated or parasitic?

If you don't know, I'd suggest to use the open source VBIC99 model (Vertical Bipolar Inter-Company model from Motorola), a level 9 BJT model; you'll find it on Internet.

There are many example model files in Cadence installation directory..

erikl said:

Sure; a lot of people have them. But the process-dedicated models are mostly confidential. It would be easier to help you if you'd tell more exactly what you need. Which process size, lateral or vertical, dedicated or parasitic?

If you don't know, I'd suggest to use the open source VBIC99 model (Vertical Bipolar Inter-Company model from Motorola), a level 9 BJT model; you'll find it on Internet.

Click to expand...

Thanks, I'll definitely search that. (EDIT: searched, I need to get model parameter VALUES that are realistic that model the effects I am concerned about [see below]...)

I don't care about process size or vertical/horizontal, to be honest I don't know much about bipolar design, which is why I want to work with it. For the project I am mostly concerned with the current gain of the BJT at single nanoamp levels; one key aspect of the project is a current source capable of outputting 1nA. This is a very low frequency application, and must be low noise. I am not really sure what device properties I should be looking at for a project of this type.

I will also need high current (10s of mA) capability of the process, which I am sure will just require larger devices. This is not going to be a particularly area-restricted design. Other important features are low offset voltage for amplifiers, low drift, etc.

also there will be no digital parts of this project, strictly precision analog. so, filters, opamps, current mirrors, etc. digital can be off-chip or integrated with a bicmos process. This is more of an experimental proof of concept design