The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Simulators >> Circuit Simulators >> SiMKit in Spectre
https://designers-guide.org/forum/YaBB.pl?num=1121331796

Message started by Sas on Jul 14^th, 2005, 2:03am

Title: SiMKit in Spectre
Post by Sas on Jul 14^th, 2005, 2:03am

Help!

I need to make the circuit using bjt from SiMKit (mextram model). I attached SiMKit to Spectre, Spectre can find it, but I have no idea how to find my bjt504 and place it on schematic.
Is anyone knows how to establish model for npn or pnp (if I want to use Gummel-Poon or others)? :-/

Title: Re: SiMKit in Spectre
Post by Andrew Beckett on Jul 15^th, 2005, 3:25am

Sounds like you need to either attend some training or read the analog design environment documentation.

Most of the time, processes come with a design kit, which has a set of symbols for the devices in that process, and some corresponding model files.

If so, consult the documentation for that design kit, and use the appropriate component.

If you only have the model files (i.e. a text file describing a particular bipolar type, which uses the underlying bjt504
model), then you can use the npn/pnp component from analogLib, and specify the name of the model (as defined in the model file) in the model field on the edit properties form.

Then in ADE, reference the model library (setup->model libraries).

If you don't have a model file, then you've got to create one. But that's not something you can just invent...

Andrew.

Title: Re: SiMKit in Spectre
Post by Geoffrey_Coram on Jul 19^th, 2005, 9:10am

Actually, for Mextram, the model has built-in defaults that correspond to some sort of NPN (the parameters anre't all zero).

So, you can place an npn symbol from the analogLib and then your model library file can just look like this:

model mynpn bjt504 type=n

Here's a whole netlist:

* test netlist
simulator lang=spectre

VB (b 0) vsource type=dc dc=0.5
VC (c 0) vsource type=dc dc=1
model mynpn bjt504 type=npn
Q1 (c b 0 0) mynpn

dc1 dc oppoint=screen

Title: Re: SiMKit in Spectre
Post by Andrew Beckett on Jul 19^th, 2005, 10:51am

Geoffrey,

In fact that's true of many models in spectre. I often throw together simple testcases with models such as:

Code:

model nch bsim3v3 type=n

but of course such a model is not exactly of practical use... which was my point in my previous reply in this thread.

Regards,

Andrew.

Title: Re: SiMKit in Spectre
Post by Geoffrey_Coram on Jul 20^th, 2005, 4:38am

Andrew -
Whether the defaults are reasonable or not has to do with the definition of the standard model, not with the simulator (Spectre or otherwise). BSIM3 and Mextram have "reasonable" defaults. On the other hand, Hicum does not -- all of the zero-bias capacitances (cjci0, cjei0, ...) and the external resistances (rbx, rcx, re) are zero by default.

As to whether this is useful: it's really not clear at all what Sas is trying to do; it might actually be a useful next step to get a simple Gummel plot using the default model, and then worry about getting the right model parameters.

-Geoffrey

Title: Re: SiMKit in Spectre
Post by Sas on Jul 20^th, 2005, 5:30am

Hello,
I want to specify my question. I want to use the bjt with mextram model in my desing. I installed SiMKit according the instructions of website. SPECTRE can see SiMKit (2.1.1). If I create netlist with bjt504t (with substrate and selfheating) and run it, there is no doubts that SPECTRE use bjt504t from SiMKit. BUT! I need to creat schematic with bjt (5 ports) and use mextram as model (parameters can be default). I can't get a way how to find components (in my case 5 port bjt) from SiMKit library and how to see the library components in that case. I have similar problem with phillib.

Why I can see analogLib and use components from there on my schemaitic and I can't see the same way SiMKit (or another philips library). :-[

Title: Re: SiMKit in Spectre
Post by Geoffrey_Coram on Jul 21^st, 2005, 6:26am

I don't think SimKit includes any symbols, it just includes the model code.

Title: Re: SiMKit in Spectre
Post by Sas on Jul 21^st, 2005, 7:40am

So basically I can't use it in schematic (if it has 5 input ports and npn suggests only 3!).

Title: Re: SiMKit in Spectre
Post by Geoffrey_Coram on Jul 22^nd, 2005, 12:52pm

Well, there might be a 5-terminal BJT ... I vaguely recall 3- and 4-terminal BJTs in PSpice. We have our own libraries with its own symbols here, specific to each manufacturing process (no BJTs in the CMOS library); so there must also be a way to create your own symbols. I haven't done it myself; you'll have to read the manual or take a class or something, though.

Title: Re: SiMKit in Spectre
Post by sheldon on Jul 23^rd, 2005, 6:02am

Greetings,

It is not a big deal to create 5 terminal bjt symbols, used
to do it for vertical pnp transistors with isolated collectors.
Bascially, just copied a four terminal symbol, added a
additional terminal, and updated the CDF. Since we had
a schematic underneath, ADE treated it like a subcircuit.
Not sure how ADE will handle 5-terminal primitives, you
may need to wrap the model in an in-line subcircuit.

Best Regards,

Art Schaldenbrand