Photodiode SPICE models?
Phil Hobbs
I'm on a bit of a roll with TIA designs at the moment, but I've just
been using current sources with caps in parallel to model fully-depleted
photodiodes, and I need a better model to hack up.
The LTSPICE Yahoo group's files area is broken at the moment. Do any of
you have a decent PD model with 4 terminals (anode, cathode, and two to
represent the light input)?
Nonlinear capacitance would be a plus but isn't required.
(I've used SPICE more in the last two weeks than in my entire previous
career--I'm more of an algebra guy when it comes to circuit design, but
some things really need sims.)
Thanks
Phil Hobbs
--
Dr Philip C D Hobbs
Principal
ElectroOptical Innovations
55 Orchard Rd
Briarcliff Manor NY 10510
845-480-2058
hobbs at electrooptical dot net
http://electrooptical.net
Joerg
> Dear all:
>
> I'm on a bit of a roll with TIA designs at the moment, but I've just
> been using current sources with caps in parallel to model fully-depleted
> photodiodes, and I need a better model to hack up.
>
> The LTSPICE Yahoo group's files area is broken at the moment. Do any of
> you have a decent PD model with 4 terminals (anode, cathode, and two to
> represent the light input)?
>
> Nonlinear capacitance would be a plus but isn't required.
>
> (I've used SPICE more in the last two weeks than in my entire previous
> career--I'm more of an algebra guy when it comes to circuit design, but
> some things really need sims.)
>
Been there myself but ran out of time and did the design sans sims ...
rummaging in some old notes ... ah, here, in case you have library access:
Ravezzi L.; Dalla Betta G.-F.1; Stoppa D.; Simoni A., Microelectronics
Journal, Vol.31, No.4, April 2000, pp. 277-282, Elsevier.
Sorry, I wish I had it but I don't. But these are available online:
http://www.mos-ak.org/munich/posters/P09_MOS-AK_Senapati.pdf
http://www.nsti.org/publications/MSM/2001/pdf/302.pdf
Ecole Polytechnique in France has developed a model a couple years ago,
you might want to contact:
razvan.negru <at> polytechnique <dot> edu
Specialty stuff but may be helpful:
http://www.mdpi.com/1424-8220/8/10/6566/pdf
--
Regards, Joerg
http://www.analogconsultants.com/
"gmail" domain blocked because of excessive spam.
Use another domain or send PM.
Phil Hobbs
Thanks, Joerg. I'll do that.
Cheers
Yuri Belenky
> Dear all:
>
> I'm on a bit of a roll with TIA designs at the moment, but I've just
> been using current sources with caps in parallel to model fully-depleted
> photodiodes, and I need a better model to hack up.
>
> The LTSPICE Yahoo group's files area is broken at the moment. Do any of
> you have a decent PD model with 4 terminals (anode, cathode, and two to
> represent the light input)?
>
> Nonlinear capacitance would be a plus but isn't required.
>
> (I've used SPICE more in the last two weeks than in my entire previous
> career--I'm more of an algebra guy when it comes to circuit design, but
> some things really need sims.)
>
> Thanks
>
> Phil Hobbs
>
I've used this model several years ago (MRD500 photodiode):
--- model starts here ------------------------
* PSpice Model Editor - Version 10.5.0
*$
*******************************************************************************
* A = Anode
* C = Cathode
* P = (light)Power as voltage input
.SUBCKT MRD500 A C P PARAMS: Spec=1.0 Sensy=0.3894
* MRD500 from Motorola * RAP 7/97
DPD A C PhotoDet
RDUMMY P 0 1G
GPD C A TABLE {V(P)* Spec * Sensy} (0,0) (1,1)
.MODEL PhotoDet D IS=1.02p RS=10 N=0.841978 BV=100 IBV=1u
+ CJO=6.03p VJ=0.202968 M=0.146605 TT=1n ISR=17p
.ends
*$
--- end of model ------------------------------
Let me know if you need it as OrCAD library file.
Yuri.
Phil Hobbs
> Phil Hobbs wrote:
>> Dear all:
>>
>> I'm on a bit of a roll with TIA designs at the moment, but I've just
>> been using current sources with caps in parallel to model
>> fully-depleted photodiodes, and I need a better model to hack up.
>>
>> The LTSPICE Yahoo group's files area is broken at the moment. Do any
>> of you have a decent PD model with 4 terminals (anode, cathode, and
>> two to represent the light input)?
>>
>> Nonlinear capacitance would be a plus but isn't required.
>>
>> (I've used SPICE more in the last two weeks than in my entire previous
>> career--I'm more of an algebra guy when it comes to circuit design,
>> but some things really need sims.)
>>
>> Thanks
>>
>> Phil Hobbs
>>
>
> I've used this model several years ago (MRD500 photodiode):
>
> --- model starts here ------------------------
>
> * PSpice Model Editor - Version 10.5.0
>
> *$
> *******************************************************************************
>
> * A = Anode
> * C = Cathode
> * P = (light)Power as voltage input
> * MRD500 from Motorola * RAP 7/97
> DPD A C PhotoDet
> RDUMMY P 0 1G
> GPD C A TABLE {V(P)* Spec * Sensy} (0,0) (1,1)
> + CJO=6.03p VJ=0.202968 M=0.146605 TT=1n ISR=17p
> *$
>
> --- end of model ------------------------------
>
> Let me know if you need it as OrCAD library file.
>
> Yuri.
A couple of people have sent models (Thanks, guys), but there is one
remaining puzzle: shot noise. I'd have thought that the .asc file below
would generate exactly the shot noise of Iphoto--diodes have full shot
noise, so connecting it to a DC current source should turn D1 into a
full shot noise current source, which ought to get picked off via the
infinite capacitor into the 0V source, and so into the behavioural
current source at the output.
However, it doesn't do anything of the sort--it's all over the map.
Different diodes and diode-connected transistors give all sorts of
different values.
Any ideas what's going on? One possible clue is that any resistance at
all in series with V2 reduces the noise enormously.
Jim Thompson
Phil,
Unfortunately, transient and DC simulations won't/don't show noise.
A .AC analysis should show noise. I don't know the set-ups for
LTspice.
.MODEL PhotoDet is likely lacking in noise coefficients, so it's
defaulting to who knows what.
...Jim Thompson
--
| James E.Thompson, CTO | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona 85048 Skype: Contacts Only | |
| Voice:(480)460-2350 Fax: Available upon request | Brass Rat |
| E-mail Icon at http://www.analog-innovations.com | 1962 |
"Somebody had to build the ceiling...
before Michelangelo could go to work."
- John Ratzenberger
http://analog-innovations.com/SED/Somebody_had_to_build_the_ceiling.pdf
Phil Hobbs
> defaulting to who knows what.
>
> ...Jim Thompson
Jim,
Thanks. I should have been clearer I expect--I'm trying to do a .noise
simulation, and I see the diode noise but it's anywhere from 1% to 75%
of the correct shot noise value depending on the device and the value of
Iphoto. Replacing the diode with a 1N5817 gets nearly the right answer
at 1 mA but is hopelessly low at 1 uA. Using a diode-connected BFT25A
(B-C shorted) gives results about 10 dB too low at all photocurrents.
I saw this exact technique recommended in a paper. There's obviously
something I'm doing wrong, but I don't know what it is.
Cheers
Phil Hobbs
> Jim Thompson wrote:
>> On Wed, 28 Oct 2009 12:40:25 -0400, Phil Hobbs
>> <pcdhSpamM...@electrooptical.net> wrote:
>>
>>> Yuri Belenky wrote:
>>>> Phil Hobbs wrote:
>>>>> Dear all:
>>>>>
>>>>> I'm on a bit of a roll with TIA designs at the moment, but I've
>>>>> just been using current sources with caps in parallel to model
>>>>> fully-depleted photodiodes, and I need a better model to hack up.
>>>>>
>>>>> The LTSPICE Yahoo group's files area is broken at the moment. Do
>>>>> any of you have a decent PD model with 4 terminals (anode, cathode,
>>>>> and two to represent the light input)?
>>>>>
>>>>> Nonlinear capacitance would be a plus but isn't required.
>>>>>
>>>>> (I've used SPICE more in the last two weeks than in my entire
>>>>> previous career--I'm more of an algebra guy when it comes to
>>>>> circuit design, but some things really need sims.)
>>>>>
>>>>> Thanks
>>>>>
>>>>> Phil Hobbs
>>>>>
Ah, I see where the confusion arose--I'm not using Yuri's circuit, but
the one I attached. Here it is again inline.
Still weird.
Cheers
Phil
--------- ShotNoiseGen.asc -------------------
Version 4
SHEET 1 880 732
WIRE 80 32 16 32
WIRE 160 32 80 32
WIRE 400 32 288 32
WIRE 16 48 16 32
WIRE 160 48 160 32
WIRE 80 64 80 32
WIRE 400 64 400 32
WIRE 288 96 288 32
WIRE 160 128 160 112
WIRE 16 160 16 128
WIRE 80 160 80 128
WIRE 288 208 288 176
WIRE 400 208 400 144
WIRE 400 208 288 208
FLAG 16 160 0
FLAG 400 32 Output
FLAG 80 160 0
FLAG 160 208 0
FLAG 288 208 0
SYMBOL res 384 48 R0
SYMATTR InstName R1
SYMATTR Value 10k
SYMBOL current 16 128 R180
WINDOW 0 24 88 Left 0
WINDOW 3 24 0 Left 0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName I1
SYMATTR Value {Iphoto}
SYMBOL voltage 160 112 R0
WINDOW 123 0 0 Left 0
WINDOW 39 24 118 Left 0
SYMATTR SpiceLine Rser=0
SYMATTR InstName V2
SYMATTR Value 0
SYMBOL cap 144 48 R0
SYMATTR InstName C2
SYMATTR Value 1G
SYMATTR SpiceLine Rser=1f Lser=1f Rpar=1T
SYMBOL bi2 288 176 M180
WINDOW 0 24 88 Left 0
WINDOW 3 24 0 Left 0
SYMATTR InstName B2
SYMATTR Value I=Iphoto+I(V2)
SYMBOL diode 64 64 R0
SYMATTR InstName D1
SYMATTR Value Dshot
TEXT -216 128 Left 0 !.param Iphoto=1m
TEXT -216 160 Left 0 !.noise V(Output) I1 dec 10 1 1g
TEXT -200 104 Left 0 !.model Dshot D()
George Herold
<pcdhSpamMeSensel...@electrooptical.net> wrote:
> Yuri Belenky wrote:
> > Phil Hobbs wrote:
> >> Dear all:
>
> >> I'm on a bit of a roll with TIA designs at the moment, but I've just
> >> been using current sources with caps in parallel to model
> >> fully-depleted photodiodes, and I need a better model to hack up.
>
> >> The LTSPICE Yahoo group's files area is broken at the moment. Do any
> >> of you have a decent PD model with 4 terminals (anode, cathode, and
> >> two to represent the light input)?
>
> >> Nonlinear capacitance would be a plus but isn't required.
>
> >> (I've used SPICE more in the last two weeks than in my entire previous
> >> career--I'm more of an algebra guy when it comes to circuit design,
> >> but some things really need sims.)
>
> >> Thanks
>
> >> Phil Hobbs
>
> > I've used this model several years ago (MRD500 photodiode):
>
> > --- model starts here ------------------------
>
> > * PSpice Model Editor - Version 10.5.0
>
> > *$
>
> - Show quoted text -
Phil, this is most likely a stupid idea, but does model have the
correct source impedance for the 'diode as shot noise source'. R = kT/
(eI)
(I loved the 'link' that I clicked on an it loaded the whole
schematic.. cute)
George H.
Phil Hobbs
>><snip>
>
> Phil, this is most likely a stupid idea, but does model have the
> correct source impedance for the 'diode as shot noise source'. R = kT/
> (eI)
Hmm. That's an interesting point...perhaps the diode models aren't
implemented the way I thought, with the shot noise being a current
source internally.
>
> (I loved the 'link' that I clicked on an it loaded the whole
> schematic.. cute)
LTSpice rides again--flat ASCII schematic files. Go, Mike!
Cheers
Phil Hobbs
Okay, I solved the problem. There's something weird about the diode
model in LTSPice--it really really doesn't like zero impedance loads.
I've attached a hacked-up version of the SFH2400 model from the LTSpice
group on Yahoo, with switchable shot noise--it takes a parameter called
ShotNoiseOn (default=1) which does what you'd expect.
It uses a balanced pair of diodes and forms the shot noise contribution
by summing their terminal voltages and multiplying by
I_dc/(sqrt(2)*(25.8 mV)). This makes sure that only the uncorrelated
part (i.e. noise) winds up in the output. Single-ended voltage versions
cause signal feedthrough as well.
Cheers
Phil Hobbs
George Herold
> 1KViewDownload
>
> sfh2400_shotnoise_hy.asc
> 4KViewDownload- Hide quoted text -
>
> - Show quoted text -
Excellent! Now you've got something with the correct impedance. I
was 'burned' by the diode impedance when I first tried to measure the
shot noise from a diode. I biased it with a battery and large
resistor and fed the bottom end into a TIA opamp. NO noise??? (well
except for opamp and resistor noise.) I had to add a capacitor to
allow for a low impedance path for the shot noise.
Funny, how you usually have to screw something up before you really
learn it.
George H.