# How to model a Schottky diode based on datasheet?

I have a question about how to model a non-linear a Schottky diode based on available datasheet in ADS. Should I just assign Rs and Cj values from datasheet?

http://datasheet.octopart.com/DMK2790-G4D-Skyworks-Solutions-datasheet-23706700.pdf

The diode will be used as a switch. Could anyone help? Thanks

• The datasheet actually shows a model for the diode. Did you read the datasheet ?
– Mike
Feb 9 '18 at 20:40
• Yes I did and saw the parameters. I have trouble putting the model in ADS. Feb 9 '18 at 22:01

The spice model is in the datasheet:

It's a little confusing because they tell you to use these parameters:

R1 and LS, Csh are values for the circuit model, the rest are for the diode model.

You make a diode model like this:

General form: d[name] [anode] [cathode] [modelname]
.model ([modelname] d [parmtr1=x] [parmtr2=y] . . .)

Example: d1 1 2 mod1
.model mod1 d

Example2: D2 1 2 Da1N4004

.model Da1N4004 D (IS=18.8n RS=0 BV=400 IBV=5.00u CJO=30 M=0.333 N=2)

Draw the circuit up and plug in the other parameters for the diode model.

Here is another way to model a schottky diode if the above model does not sufficiently model all of the dynamics, you would need to take measurements of a real device and fit them to the model:

Edit: ADS does use spice models and the model format looks the same. You can also import models from spice into ADS.

• Thank you @laptop2d for the details. I am trying to simulate in ADS. Would it be similar? Feb 9 '18 at 22:15
• Sorry I forgot you were working in ADS, edited answer Feb 9 '18 at 23:00
• Thank you laptop2d! I did tried and imported the model to ADS. I am still playing around the parameters and see how they affect the diode as a switch. Especially for Td. Schottky didoes should have nearly 0 recovery time; Td in ps seems making sense. But I do not see it affecting the switch so far.. still figuring out. Feb 13 '18 at 15:00

I don't have ADS and have never had any experience with it. So one huge problem is that I can't tell what the Td parameter is. "Time delay" is the first thing that pops into my mind. But the value looks an awful lot to me like the saturation current, which is usually labeled as "Is" in the models. I'm offering the following only because it may help in some fashion as you try and get things working on your end.

My experiences are, today, mostly with LTSpice. For a device like this, I'd create a model using the .SUBCKT method. They show a diagram there. So that's what I'd try and follow. Something like this:

.SUBCKT DMK2790 1 2
D1 1 3 DMKDIODE 1
R1 3 4 3
L1 4 2 150p
C1 0 1 .02p
C2 0 2 .02p
.MODEL DMKDIODE D(N=1.05 Rs=4 CJO=0.05p Eg=0.82 XTI=2 FC=0.5 BV=4.0 IBV=1E-5 Is=1E-11 M=0.26)
.ENDS


You may note that I've changed the "Td" to "Is" in the diode model included above. But I honestly can't tell you if my guess is right or if ADS actually does use the Td parameter, instead. If so, just replace my "Is" with "Td" and see if that works for you.

As far as my sub-circuit model above goes, you should be able to see where I pulled values from the datasheet and placed them into the sub-circuit.

You can now use this sub-circuit in your own circuit, though. Try it out.

• Thank you @jonk !! I tried and it works pretty well. I think Td is time delay - same as transition time from ON-OFF(I am guessing). I also tried modifying Td to nanosec, by observing a time-domain plot, I don't see a obvious delay. Still need to figure out... but still, THANK YOU! Feb 13 '18 at 14:56