Zener Diode Model in HSpice

Hi,
Anyone can help me with a Zener Diode model in HSpice?
The voltage should be somewhere between 2.5-3.5 Volt with a maximum 15-20mA current.
Thanks

Just take a standard diode model (from a diode, which can stand the required current), and add/change the BV parameter for the necessary breakdown voltage, s. the corresponding page from the "HSPICE Elements and Device Models Manual®" below.

You can also download the models of zener diodes from manufacturers e.g.
https://www.onsemi.com/PowerSolutions/supportDoc.do?type=models&category=830

Keith.

Keith
The models in OnSemi site cant be used with HSpice i think, i downloaded 2 of them, but there are UnDefined parameters for HSpice in their models.

Ericl
I used one of the .models from PSpice:
.MODEL D1N4684 D
+ IS=80.21637E-9
+ N=2.80334
+ RS=3.412605e-002
+ CJO=135E-12
+ M=.5033
+ VJ=.75
+ ISR=4.2604E-6
+ NR=4.11012
+ BV=3.4781
+ IBV=49.004E-3
+ TT=150.49E-9

and i tried to change the BV voltage to 1 volt for example, but still i had 1.5volt on the output of the Zener diode and somehow the voltage was dependent to next stage of the circuit and was not fixed! so im confused how it works?

rvn176 said:

Keith
The models in OnSemi site cant be used with HSpice i think, i downloaded 2 of them, but there are UnDefined parameters for HSpice in their models.

Click to expand...

You need to make sure you only download the Pspice ones or the .lib ones, not the SP3 ones. I tried one and it seems fine but it is a it messy because it was defined as a subcircuit and so you need to be able to handle that.

I have quite a lot of discrete zener models such as BZX79 series, 1N4728 series, BZD23 series. Let me know what voltage you want and I can post it here. Here is an example:

.subckt BZX79-4V7 1 2
D1 1 2 D1
D2 2 3 D2
I1 1 3 0.9814
R1 1 3 4 TC1=-0.3566m
.model D1 D IS=9.19e-16 CJO=300p RS=0.57061 ISR=4.05e-08
.model D2 D IS=1.00e-15
.ends

Keith.

Keith
here is the model i downloaded + the **error** from HSpice, i think u have deleted some parameters in ur model:

.subckt bzx84c3v0lt1 2 1
**************************************
* model generated by modpex *
*copyright(c) symmetry design systems*
* all rights reserved *
* unpublished licensed software *
* contains proprietary information *
* which is the property of *
* symmetry or its licensors *
*commercial use or resale restricted *
* by symmetry license agreement *
**************************************
* model generated on mar 10, 06
* model format: pspice
* anode cathode
*node: 2 1
* forward section
d1 2 1 md1
.model md1 d is=5.21532e-16 n=1 xti=1 rs=0.5
+ cjo=4.5e-10 tt=1e-08
* leakage current
r 1 2 mdr 1.53846e+06
.model mdr res tc1=0 tc2=0
* breakdown

**error**: unknown model type: res

rz 2 3 14.6948
izg 4 3 0.24
r4 4 3 3500
d3 3 4 md3
.model md3 d is=2.5e-12 n=2.76529 xti=0 eg=0.1
d2 5 4 md2
.model md2 d is=2.5e-12 n=10.6468 xti=0 eg=0.1
ev1 1 5 6 0 1
ibv 0 6 0.001
rbv 6 0 mdrbv -1158.4
.model mdrbv res tc1=0.00196824
*-- pspice diode model default parameter
* values are assumed
*is=1e-14 rs=0 n=1 tt=0 cjo=0
*vj=1 m=0.5 eg=1.11 xti=3 fc=0.5
*kf=0 af=1 bv=inf ibv=1e-3 tnom=27

**error**: unknown model type: res

.ends bzx84c3v0lt1

I want to use this Zener diode for the required voltage in the gate of a CMOS in 0.5um (the transistor gonna work like a buffer).
The diode is connected to the supply voltage by a resistor. For first step a Zener diode with 2v voltage is ok, but as i said when i used the model i posted before, with different source resistors, the gate voltage which is connected to the diode, changes.
I dont know it was because of a wrong Zener model or the circuit itself?

The model I posted is complete, but not from the ON-Semi site - they are old Philips ones I think.

I am not sure why the one you downloaded doesn't work with Hspice, maybe it is Pspice syntax (my simulator is supposed to take either). Anyway, I would try removing the

.model mdr res tc1=0 tc2=0

and change the

r 1 2 mdr 1.53846e+06

to

r 1 2 1.53846e+06

It is only a resistor.

Keith.

rvn176 said:

Ericl
I used one of the .models from PSpice:
.MODEL D1N4684 D
+ IS=80.21637E-9
+ N=2.80334
+ RS=3.412605e-002
+ CJO=135E-12
+ M=.5033
+ VJ=.75
+ ISR=4.2604E-6
+ NR=4.11012
+ BV=3.4781
+ IBV=49.004E-3
+ TT=150.49E-9

and i tried to change the BV voltage to 1 volt for example, but still i had 1.5volt on the output of the Zener diode and somehow the voltage was dependent to next stage of the circuit and was not fixed! so im confused how it works?

Click to expand...

Zener diodes in the voltage range 2..5V do not show a sharp "knee" - unlike avalanche diodes with breakthrough voltages >≈ 6V. Hence their reverse voltage is rather dependent on the current. You picked one with a series resistance of RS=34mΩ (s. above), which adds another 340mV @ 10mA (e.g.). Of course you could change the RS parameter, but that's not realistic.

Anyway, you can't integrate such a zener into an IC design; no process will offer such a zener diode. You could instead use 1 or 2 (serial) standard diodes (or diode connected MOSFETs) operated in forward direction, but the knee won't be sharp either. Both methods must use constant current through the diode(s).

If you want a fixed voltage only for simulation purpose, just use a vdc source ;-)

Surely 34m ohms at 10mA is 340uV?

Anyway, I agree that if it is for an ASIC you need to use something available on the process!

Keith

keith1200rs said:

Surely 34m ohms at 10mA is 340uV?

Click to expand...

Of course, Keith and rvn, sorry!