IC's and PSpice models

Thread Starter

hunterage2000

Joined May 2, 2010
487
Anybody know of a database on the web that holds IC PSpice models? And if there is no model, how do you create one in Multisim. I know you can create one in Multisim but you have to choose a component type like diodes, bjts, fets etc. What if you need something like a MOSFET high end gate drive, would you need the IC's discrete component makeup?
 

MikeML

Joined Oct 2, 2009
5,444
You can also create a behavioral models which are things that act like the IC using VCVS and CCCS. Have you looked on TI's web site? They have models for a lot of stuff. Also look at the LTSpice Yahoo group. There is a large repository of contributed models there...
 

Papabravo

Joined Feb 24, 2006
16,502
Like many things on the web that information is distributed. Manufacturers are often the best source for SPICE models. To create your own models from just a datasheet is, in my experience, nearly impossible. It requires that you estimate model parameters which are not generally shown on datasheets, and it requires you to have detailed knowledge of the actual model itself. Just in MOSFETS there are at least three levels of model that provide increasingly more complex behavior.

Here is an example of the Gummel-Poon model of the bipolar transistor
http://en.wikipedia.org/wiki/Gummel–Poon_model

Here are some resources for MOSFETS
http://ecee.colorado.edu/~bart/book/book/chapter7/ch7_5.htm
http://www.cs.mun.ca/~paul/transistors/node3.html
http://www.csit-sun.pub.ro/courses/...lectures/winter/vlsi/vorlesung_pdf/chap04.pdf

I tried once upon a time and gave up. If you can wade through it: "You're a better man than I am..."
 

upopads2

Joined Sep 20, 2014
54
<snip> i used to have so many of those IC models...

So so <snip> many of those.

Edited by mod: expletives deleted.
 
Last edited by a moderator:

upopads2

Joined Sep 20, 2014
54
Like many things on the web that information is distributed. Manufacturers are often the best source for SPICE models. To create your own models from just a datasheet is, in my experience, nearly impossible. It requires that you estimate model parameters which are not generally shown on datasheets, and it requires you to have detailed knowledge of the actual model itself. Just in MOSFETS there are at least three levels of model that provide increasingly more complex behavior.

Here is an example of the Gummel-Poon model of the bipolar transistor
http://en.wikipedia.org/wiki/Gummel–Poon_model

Here are some resources for MOSFETS
http://ecee.colorado.edu/~bart/book/book/chapter7/ch7_5.htm
http://www.cs.mun.ca/~paul/transistors/node3.html
http://www.csit-sun.pub.ro/courses/...lectures/winter/vlsi/vorlesung_pdf/chap04.pdf

I tried once upon a time and gave up. If you can wade through it: "You're a better man than I am..."
Bro what I used to do was I would find something close and use that.
 

Papabravo

Joined Feb 24, 2006
16,502
But what precisely does 'close' mean in this context. You have the same problem as doing one from scratch. How do you verify that similar is close enough?
 

upopads2

Joined Sep 20, 2014
54
But what precisely does 'close' mean in this context. You have the same problem as doing one from scratch. How do you verify that similar is close enough?

YOU DO THE BEST YOU CAN WITH COMMERCIAL LT SPICE MODELS AND WHAT RESOURCES ARE AVAILABLE TO YOU AT THE TIME.
 

Papabravo

Joined Feb 24, 2006
16,502
YOU DO THE BEST YOU CAN WITH COMMERCIAL LT SPICE MODELS AND WHAT RESOURCES ARE AVAILABLE TO YOU AT THE TIME.
My point was that a false and misleading conclusion from a poor choice of simulation models is arguably worse than no conclusion at all. It is OK to use a generic transistor model in place of a specific model that you don't have. It would be a mistake substitute one model for another without some way of demonstrating how close they are to each other.
 

upopads2

Joined Sep 20, 2014
54
My point was that a false and misleading conclusion from a poor choice of simulation models is arguably worse than no conclusion at all. It is OK to use a generic transistor model in place of a specific model that you don't have. It would be a mistake substitute one model for another without some way of demonstrating how close they are to each other.
I 100% agree Papa, didn't mean to offend you if i did with my caps locks. We are both speaking in extreme generalities and I am a mess you can smell my insecurity there i suppose. But there was no anger directed towards you i hope you could see that... Anyways If I am looking for a 5 volt regulator that outputs 5 volts and another one does the same thing but has a slightly different package size...it may not matter depending on the design constraint. I had a situation in simulating one of these components from TI which did not have a model available, so I use the closest thing i can find to it...as long as its outputting the 5 volts to the op amp to provide functionality to the rest of the circuit its great. If its not, its hard to work from there and make changes.
 

WBahn

Joined Mar 31, 2012
26,398
Anybody know of a database on the web that holds IC PSpice models? And if there is no model, how do you create one in Multisim. I know you can create one in Multisim but you have to choose a component type like diodes, bjts, fets etc. What if you need something like a MOSFET high end gate drive, would you need the IC's discrete component makeup?
As others have pointed out, this is a hit and miss proposition and your best resource is the manufacturer's website or engineering support staff. Be forewarned that the models you get may not be faithful in all regards. I remember using a model I got from TI for a TL082 IC and one thing that was important for my design was total power consumption since my total power budget was 900uA for everything. The sim showed the opamp drawing hundreds of amps! After a lot of verifying that I wasn't doing anything stupid, I called TI and they informed me that their model was only concerned with getting the behavior close at the I/O pins and that the power pins simply did whatever they did and he wasn't surprised at all that it would show the kind of current I was seeing. Now, that was nearly two decades ago and PC-based simulation tools were certainly constrained by the limited processing power of the day. I hope (and expect) that they are generally much better today.

In coming up with your own models, or trying to use models from somewhat similar devices, you need to be very careful about how good is good enough (as Papabravo has been pointing out). It all depends on what you are trying to measure and how accurate you need your simulations to be. If you are looking for gross behavior, you may well be able to get acceptable results using a model for a roughly similar part. But if you are looking for fine details, such as bandwidth, or noise, or a thousand other things then it may not even be in the ballpark.

In designing ICs, the models have become extraordinarily complicated and even then it isn't nearly enough. When I was designing something using the IBM 130nm process about ten years ago the model for each transistor was actually a subcircuit containing over 300 devices, many of which were themselves Level 7 BSIM FET models. That was the level of complexity needed to get "good enough" sims to deal with short-channel effects in deep submicron geometries. I was just looking at the model files for the process I'm using now and even the simplest resistor is modeled as a subcircuit containing seven other resistors, each with a third order polynomial for the temperature effects as well as other factors for voltage-dependent nonlinearities. If I'm doing a sim in which none of that matters, then I can just use a fixed resistor model and get good enough results. But in many of the sims if I use the model for an N-diffusion resistor and in reality the device is a polysilicon resistor then I risk killing the design.
 
Top