Akis,
I was measuring a bjt that had a spice model created by Andy_C to see how a real world sample compare to a model that had been tweaked to better match the data sheet. From all that I've read on this forum, it seems that if you are using models in critical locations, you probably need to tweak the model to better match the data sheet.
Ken
we amateurs cannot maintain constant temperature test conditions with our cheap and quick jury rigged test procedures.
And that work is courageous, especially since you are messing with 10A currents!
I do not think the datasheet is correct either. It could easily be related to manufacturing : different batches, different factories, different companies - whatever reason there are great differences between datasheet and measurements. And on top of that it also appears the SPICE models are different.
Secondly it is not about "critical locations"; if you have a single stage single transistor amplifier, well, it is critical by definition. I spend considerable amount of time in SPICE trying to fine tune circuits and select the values of 80 resistors and 20 capacitors. If those calculations are out then even the topology of my circuit could be wrong.
For example I am measuring THD in the virtual world and biasing the various stages accordingly. If the model thinks there is a 50% hFE shift from Vce=3V to Vce=23V then it will show much higher THD, which simply is not there, because measurements show a shift of 1% not 50%.
This shortfall of the SPICE model has become more apparent in post-amp circuits where you do expect a swing of 20V, and has gone unnoticed in pre-amp circuits where the voltage swings are one ot two volts.
Why have others not noticed it? May be they have. May be they are all using hefty amounts of negative feedback and a VAS stage with an active load (as is the common practice) so that the Vce/hFE variations are the least of your worries.
But try to create a circuit with no negative feedback and ask it to amplify 20 times and swing 20V and see what THD the model will say you are getting.
Akis,
The Spice Simulation Sticky in this forum also covers this topic. I've started refining my models using Andy_C's techniques along with the Analog Services spread sheet. It is possible to tune the models to get them pretty close on things such as hFe. It's time consuming... but, less time consuming than physical testing, de-soldering, re-soldering, testing, rinse, repeat...
Ken
The Spice Simulation Sticky in this forum also covers this topic. I've started refining my models using Andy_C's techniques along with the Analog Services spread sheet. It is possible to tune the models to get them pretty close on things such as hFe. It's time consuming... but, less time consuming than physical testing, de-soldering, re-soldering, testing, rinse, repeat...
Ken
Dear gentlemen,
I need a reasonably accurate model of either 2SA1186 or 2SA1860. These are very good Sanken power transistors but Sanken does not provide the model AFAIK. Does anyone know where to get them? Or would anyone build one so that many people can benefit from these as the transistors have very good characteristics. I would build them if I know how but it would take some time before I get to that place.
Thanks
I need a reasonably accurate model of either 2SA1186 or 2SA1860. These are very good Sanken power transistors but Sanken does not provide the model AFAIK. Does anyone know where to get them? Or would anyone build one so that many people can benefit from these as the transistors have very good characteristics. I would build them if I know how but it would take some time before I get to that place.
Thanks
just my 2 cents, if the transistor data sheet (which is usually data taken from a large population to find "worse case average") and a spice simulation both show large variation in hfe with Vce than it probably exists and there may be something wrong with your testing. hfe varies exponentialy with temp so unless you keep it controlled I dont know how you can be sure of your data. hfe also varies with Ic and from individual transistor to transistor, so its best to design around it, and thats what most people do.
If Andy_C was still around he could set us all straight.
If Andy_C was still around he could set us all straight.
I use Cordell's models for the BC550C/560C. I believe they reflect the Fairchild parts. The ONSemi and NXP parts are a bit different.
CordellAudio.com - SPICE Models
The models reflect the "real thing" pretty well as far as I can tell. But BJT modeling is somewhat of an inexact art so far, and you just aren't going to get models that match reality in every aspect. Even if you did you would probably find them inconvenient because they would make simulation very slow.
CordellAudio.com - SPICE Models
The models reflect the "real thing" pretty well as far as I can tell. But BJT modeling is somewhat of an inexact art so far, and you just aren't going to get models that match reality in every aspect. Even if you did you would probably find them inconvenient because they would make simulation very slow.
I already use those and they work fine for lower rails. But they are limited in vce0, so that's why I need the 546/556, and all I could find are the B types.
Transistor characteristics tend to vary significantly from one manufacturing lot to another, so you should not expect any models to match specific parts you have on-hand with high precision. I recall finding some comments from Bob Cordell where he discussed his methods for developing models, the characteristics he tried to model, and the places where his models are different from manufacturers' published models. I believe it was either on his web site, or in a thread here on DIYAudio. That discussion may give you insight into the suitability of his (or any other) models for the simulations you want to perform.
I don't think SPICE models any kind of breakdown (or other non-ideal behavior at high Vce) in the standard "Transistor" devices. Or, if it does, the breakdown is modeled using parameters that are seldom, if ever, published in manufacturers' models.
The attached file contains various SPICE models I have collected for the BC54x and BC55x families. Pick a few examples and study how the model parameters change for the various voltage ratings, and for the various Hfe ranges. That should give you enough information to make intelligent modifications to models for similar devices (e.g., the BC546B, or the BC547C) so they more closely match your BC546C. Then verify your changes by running simulations and comparing results to Data Sheet curves.
Dale
For almost every transistor, there are more bad models than good models. Most of the bad models come from simulator libraries and vendor libraries (no exceptions as far as I can tell, except maybe NXP/Phillips). It seems like someone committed lots and lots of fraud in selling bogus models to manufacturers, and bizarrely, the manufacturers don't seem to care. Maybe it's a sore spot?
So I suggest if someone shows you a known working model, check that out first. The problematic models are often really easy to spot. The Cordell models were created by hand and for that reason alone should be reasonable, if not for your specific batch, then for the batches Cordell had access to (Fairchild), and if you're that picky, you'll need a new model for every new project anyway. Yes, I checked the Early voltage parameters and they are close enough for me. Even I don't rely on individual transistor parameters THAT much. If it's that critical you should probably have a prototype working alongside the simulation.
Also, if one parameter is bogus, it's very likely there are other bogus parameters, so the whole model should probably be pruned and scrutinized. That's the point where I seriously consider ditching the model and starting from scratch, because the model is probably a scrambled clone of another model (yes, the standard libraries are full of these), and totally worthless.
So I suggest if someone shows you a known working model, check that out first. The problematic models are often really easy to spot. The Cordell models were created by hand and for that reason alone should be reasonable, if not for your specific batch, then for the batches Cordell had access to (Fairchild), and if you're that picky, you'll need a new model for every new project anyway. Yes, I checked the Early voltage parameters and they are close enough for me. Even I don't rely on individual transistor parameters THAT much. If it's that critical you should probably have a prototype working alongside the simulation.
Also, if one parameter is bogus, it's very likely there are other bogus parameters, so the whole model should probably be pruned and scrutinized. That's the point where I seriously consider ditching the model and starting from scratch, because the model is probably a scrambled clone of another model (yes, the standard libraries are full of these), and totally worthless.
Look at this one in Simetrix
*From Philips SC04 "Small signal transistors 1991"
* Base spreading parameters (RB,IRB,RBM) estimated. TR derived using BCY58 data
.model BC547C npn ( IS=7.59E-15 VAF=19.3 BF=500 IKF=0.0710 NE=1.3808
+ ISE=7.477E-15 IKR=0.03 ISC=2.00E-13 NC=1.2 NR=1 BR=5 RC=0.25 CJC=6.33E-12
+ FC=0.5 MJC=0.33 VJC=0.65 CJE=1.25E-11 MJE=0.55 VJE=0.65 TF=4.12E-10
+ ITF=0.4 VTF=3 XTF=12.5 RB=100 IRB=0.0001 RBM=10 RE=0.5 TR=1.50E-07)
The Early voltage is only 19.3 V and the simulator has Ic rising from 4.2 mA to 13 mA for 10 uA base current as Vce is ramped up to 50V
I cannot find a usable curve in a datasheet to estimate the true value, but I don't believe it's this horrible
*From Philips SC04 "Small signal transistors 1991"
* Base spreading parameters (RB,IRB,RBM) estimated. TR derived using BCY58 data
.model BC547C npn ( IS=7.59E-15 VAF=19.3 BF=500 IKF=0.0710 NE=1.3808
+ ISE=7.477E-15 IKR=0.03 ISC=2.00E-13 NC=1.2 NR=1 BR=5 RC=0.25 CJC=6.33E-12
+ FC=0.5 MJC=0.33 VJC=0.65 CJE=1.25E-11 MJE=0.55 VJE=0.65 TF=4.12E-10
+ ITF=0.4 VTF=3 XTF=12.5 RB=100 IRB=0.0001 RBM=10 RE=0.5 TR=1.50E-07)
The Early voltage is only 19.3 V and the simulator has Ic rising from 4.2 mA to 13 mA for 10 uA base current as Vce is ramped up to 50V
I cannot find a usable curve in a datasheet to estimate the true value, but I don't believe it's this horrible
- Status
- This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.