Setting parameters in SPICE models

Question

I was trying to run some simulations on 45nm technology MOS transistors in Spice. I had a few beginner level questions regarding these models.

1. If a library says it is for 45nm process node, shouldn't the length and width of MOS be specified in lib itself ?
2. Although I can set the required values from schematic itself, How will I know if I am entering practical values, like drain and source area and perimeters. I believe if I enter W and L in nano meter scale and leave drain perimeter and area as it is, then I will get some impractical results.
3. Is there any way to get default values of these parameters ? and do I need to know about all the parameters written in library ? as most of them don't make sense to me.
4. I am unable to find values of gamma and lambda in downloaded spice model

Thanks

Answer 1

1. If a library says it is for 45nm process node, shouldn't the length and width of MOS be specified in lib itself ?

It means that transistors below a gate length of 45nm are not realizable. If you choose to make larger devices, the model will be chosen automatically (called binning).

---

2. Although I can set the required values from schematic itself, How will I know if I am entering practical values, like drain and source area and perimeters. I believe if I enter W and L in nano meter scale and leave drain perimeter and area as it is, then I will get some impractical results.

That is called circuit design. Correct dimensions are chosen by the designer not the simulator.(Addendum-point-2. The circuit designer chooses a W/L to realize specifications for each device. The layout designer (who is often, but not always, the same person) does the layout for the devices. Then a post-layout extraction is performed and a simulation is run with actual drain/source areas as well as other parasitics included in the netlist. The results from schematic simulation should match the results from the post-layout simulation.)

---

3. Is there any way to get default values of these parameters ? and do I need to know about all the parameters written in library ? as most of them don't make sense to me.

An analog designer has to worry about aspect ratio (W/L) of each of the transistor in the circuit. Indeed it is the only thing any designer has control over.

A digital designer often uses libraries that provide digital primitives and are made available with the design kit. The designer of such libraries are analog designers themselves.

---

4. I am unable to find values of gamma and lambda in downloaded spice model

Trying to relate level 1,2,3 models with BSIM4 models is a non-trivial exercise. At this point, it seems that you are not conversant with design flows for your kit's ecosystem.

(EDIT-2-Addendum on pt4) Spice modeling of on-chip devices is an area of research in itself. In the 70s when VLSI was in its infancy and SPICE had just been introduced, the process nodes were at 10um and the device modeling was done with few parameters. Each of the parameters had a well-understood physical meaning. Fast forward half a century, a BSIM model can have upwards of 200 parameters depending on the level and these are basically a result of fitting copious amounts of measured data using a computer. The complex higher order effects can't be described using any physical model. In other words, not all these parameters have a physical meaning anymore. You can find more information from publications at this Berkeley web page.

Answer 2

1. The "45 nm" value is the minimum gate length. The minimum gate width will be determined by the process design rules. You are free to create transistors larger in length and/or width. So, no, the W and L should not be in the model file.

2. You determine the source/drain area and perimeter from looking at the physical layout of the transistors. If you don't have a layout then you can estimate the area and perimeter using the W value for each transistor, and assuming that the other dimension of the source/drain is the minimum active area width with a contact in it. This is usually specified as the minimum contact size plus the minimum overlap of active area around a contact.

3. You may be able to get nominal or approximate values from the foundry that will build your chips. Generally the model parameters are supplied by the foundry and you need to trust that they are correct. The foundry might give you some limitations on the use of those models, such as a maximum W or L, but you will need to ask.

4. Modern SPICE models are much more sophisticated than the simple models we learn about in school, so you may not see a single model parameter corresponding to lambda or gamma. These will be calculated individually for each transistor based on its W, L, and possibly temperature. If you want to estimate lambda or transconductance for hand calculations then you can run simulations for a specific transistor size to get them.