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 14th, 2005, 2:03am |
Title: SiMKit in Spectre Post by Sas on Jul 14th, 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 15th, 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 19th, 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 19th, 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:
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 20th, 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 20th, 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 21st, 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 21st, 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 22nd, 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 23rd, 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 |
The Designer's Guide Community Forum » Powered by YaBB 2.2.2! YaBB © 2000-2008. All Rights Reserved. |