How to I add tolerance to an LTspice .lib electrical characteristic

Question

I am currently trying to figure out how to add tolerance to my LM4040, ZVP2160, and 2N3904 components.

I'm attempting a Monte Carlo analysis and use the {mc(value,tolerance)} for the value of my resistors, but obviously changing the value breaks the custom part. I'm wondering if there is a way to modify VTO = -1.5 to something like VTO = mc(-1.5,.01) for example.

Is it even possible to add tolerance to custom components in LTspice?

Answer 1

Im wondering if there is a way to modify VTO = -1.5 to something like VTO = mc(-1.5,.01) for example.

Yes, you can do this and it's pretty straightforward (especially using LTspice's ako keyword) if you only have one instance of each .model you want to use. The only thing you're missing in your statement are the curly braces around the mc() function.

However, an issue arises when you use multiple instances of the same .model. LTspice only evaluates the .model statement once per each simulation run. So if you had three MOSFETs, then all three would have identical VTOs for each run as shown below. Notice that all 3 plots are on top of each other.

If you need them independent of each other you have to do some more work. If you only have a few of the same device, you can manually define each with its own .model statement and unique name as shown below. Now they have their own unique VTOs.

But what if you have MANY instances and you need them to all be different? It would get pretty tedious crafting new .model statements for each instance. But we don't have to do that because there is a trick we can use which only takes a little bit of work upfront. If you know how LTspice works, .model statements are loaded/evaluated into the SPICE engine once on each run but each time you instantiate a .subckt (subcircuit) the netlist inside gets evaluated for each instance. We can use this fact to our advantage and embed our .model statement within a .subckt. The one disadvantage of doing this is the ako keyword breaks within a .subckt, so we have to copy/paste the entire .model statement manually and edit just the Vto= part.

The last part of this trick (which was done above) requires you adjusting the NMOS symbols to expect a .subckt instead of a .model. You do this by CTRL+rightclick-ing the symbol and changing the "Prefix" field from MN (or whatever it is for your device) to X. You can do this once and copy/paste that symbol anywhere you need that device on your schematic.

---

Lastly, you mentioned in the title of the question something about .lib files. You can use the .subckt trick within external .lib files as well. You just have to make sure that the .model keyword that you want to use is in between the .subckt and .ends statements. If it's outside that scope then it will only get evaluated once like normal and won't generate unique values for each instance.

Answer 2

I assume you've already familiarized yourself with the MonteCarlo.asc file in the educational subdirectory of LTspice. So I won't belabor those details.

What I'll do is grab up a schematic I have -- it's a circuit that once triggered by a manual switch will continue to power a circuit for a specified period of time. (\$R_{_\text{DEVICE}}\$ is the circuit being powered.)

It uses a MOSFET device as part of the circuit. So I've modified my schematic to perform a Monte Carlo on \$V_{_\text{TO}}\$ of the BSS123. Note that I constructed my own MODEL statement and included the VTO parameter there, using a 5% tolerance around the typical value of \$1.6\:\text{V}\$.

You can see just how much variation in the circuit timing would be due to even that small amount of variation.

Hopefully, this shows you how. If you are using .SUBCKT/.ENDS models, the same thing applies. But you can also include parameters into these that can then be used with specific parts within the sub-circuit. It all just works fine.

(I didn't use resistor or capacitor tolerances here. This is just to demonstrate how to modify active device parameters. Not to exhibit this circuit, in particular. It's just an example to make a point.)

The device parameters for the BSS123 exist in the standard library file. But they may just as well have come from any library file you might include. You will need to write your own model statement, of course. But the ako: allows you to pull in all the library parameters that you don't want to vary. So it's really easy to vary only the parameters you want to modify.

added

Here's an example. It includes two separate current sources that help to show what's going on (should be only integer currents.) Meanwhile, I've set up the two BJTs to grab up (possibly) two different models for the purposes of showing the behavior of a differential amplifier (long-tailed pair.) This produces different models (sometimes) for the two different BJTs. So it can be used to show a range of behaviors.