Spice simulation - Page 50 - diyAudio
Go Back   Home > Forums > Design & Build > Software Tools

Software Tools SPICE, PCB CAD, speaker design and measurement software, calculators

Please consider donating to help us continue to serve you.

Ads on/off / Custom Title / More PMs / More album space / Advanced printing & mass image saving
Reply
 
Thread Tools Search this Thread
Old 6th February 2008, 02:53 PM   #491
syn08 is offline syn08  Canada
Account disabled at member's request
 
Join Date: Aug 2005
Location: Toronto
Default Re: Re: Japanese JFET models

Quote:
Originally posted by Onvinyl



Hi,
I have the same models. Your definition, however, is not reflected there, if I'm not completly off anything.
For the 2SK170, it is stated BETA= 59.86m, Vto=0.5024, and you said Idss 12mA. When processing BETA=Idss*Vto^2
I get BETA=12*(0.5024^2)
BETA=12*0.2524=3.028m
Or, vice versa, if BETA is correct, you'd get an Idss of 237mA. Gosh!
I hope I don't mis-interprete the mathematical chars...

The relation of the modeled values are close to BETA=Idss*(Vto*10), however...


Rüdiger

Sorry, it's a typo in my latest post! it should read Idss=BETA*Vto^2 as I've said in the previous posts. Now 60*(0.5)^2=12

Thanks for spotting this.
  Reply With Quote
Old 7th February 2008, 06:32 PM   #492
diyAudio Member
 
Onvinyl's Avatar
 
Join Date: Aug 2002
Location: Germany
Oops, I should have read your posts above

However, is it approprioate to leave anything but Vto and Idss unchanged in the model and hope for reasonability?

And, is there an obvious way to model thermal drift of the FET's parameters in LTSpice?

Rüdiger
__________________
"I can feel what's going on inside a piece of electronic equipment. I have a sense that I know what's going on inside the transistors." Robert Moog
  Reply With Quote
Old 7th February 2008, 07:17 PM   #493
diyAudio Member
 
EDDELARUE's Avatar
 
Join Date: Nov 2004
Location: Brasilia
Send a message via MSN to EDDELARUE Send a message via Skype™ to EDDELARUE
Hi syn08,

Besides Toshiba Jfets models, would you have acurate models for 2SK1058/2SJ162 Hitachi Output Mosfets family , and/or their 2SK216/2J79 drivers family for use in Pspice ?

  Reply With Quote
Old 7th February 2008, 09:04 PM   #494
syn08 is offline syn08  Canada
Account disabled at member's request
 
Join Date: Aug 2005
Location: Toronto
Quote:
Originally posted by Onvinyl
Oops, I should have read your posts above

However, is it approprioate to leave anything but Vto and Idss unchanged in the model and hope for reasonability?

And, is there an obvious way to model thermal drift of the FET's parameters in LTSpice?

Rüdiger
I have checked those models against the datasheets and they are pretty good.

I have to confess I see little reason why simulating the Blowtorch, even if John would disclose the schematics. For the bias points, you don't really need to simulate anything (a calculator and ten minutes are good enough). For the noise performance - the models have no provisons for that, other than the thermal noise. For the closed loop bandwidth - it doesn't really matter if you are using K170/J74 or 2N5458/2N5461.

What's left:

The impact of device matching on the DC and AC performance. That's what I was mostly using the above models for. Yes, for this purpose you may want to keep Vto constant, and calculate Beta for (say) Idss=6, 10, 16mA.

The loop gain (if there's any feedback). The high gain of the japanese devices will pay off and, of course, the distortions (as much as you trust your simulator for that).

Don't expect a simulator to disclose why the Blowtorch is so highly regarded. To me, as much as I know about, if there's anything technically outstanding in the Blowtorch amp it's not the design/schematic, but the implementation/construction. As Scott Wurcer posted elsewhere, a simulator won't tell a thing about the difference (ahem... if there is any) between Vishay and Roederstein resistors.

Spice models suck big time when it comes to thermal analysis. You don't have any better chance but to create your own device models at different temperatures (if you have data about).
  Reply With Quote
Old 7th February 2008, 09:11 PM   #495
syn08 is offline syn08  Canada
Account disabled at member's request
 
Join Date: Aug 2005
Location: Toronto
Quote:
Originally posted by EDDELARUE
Hi syn08,

Besides Toshiba Jfets models, would you have acurate models for 2SK1058/2SJ162 Hitachi Output Mosfets family , and/or their 2SK216/2J79 drivers family for use in Pspice ?

I wish... Unfortunately, the 2SK1058/2SJ162 datasheets are very, very poor so there's little to extract from there. So, until I'll get a curve tracer and a 1MHz (max) LCR meter with bias and HPIB, both sometimes later this year, use the following. They are horrible, but more than nothing...

.SUBCKT 2SK1058 10 20 40
* TERMINALS: D G S
* Hitachi 160 Volt 7 Amp .171 ohm N-Channel Power MOSFET 08-06-1993
M1 1 2 3 3 DMOS L=1U W=1U
RD 100 1 80.4M
RS 30 3 5.28M
RG 20 2 21.4
CGS 2 3 410P
EGD 12 0 2 1 1
VFB 14 0 0
FFB 2 1 VFB 1
CGD 13 14 128P
R1 13 0 1
D1 12 13 DLIM
DDG 15 14 DCGD
R2 12 15 1
D2 15 0 DLIM
DSD 3 100 DSUB
LS 30 40 7.5N
LD 10 100 4N
.MODEL DMOS NMOS (LEVEL=3 THETA=85M VMAX=163K ETA=2.2M VTO=.5 KP=.999)
.MODEL DCGD D (CJO=128P VJ=.6 M=.68)
.MODEL DSUB D (IS=29N N=1.5 RS=61.4M BV=160 CJO=802P VJ=.8 M=.42 TT=252N)
.MODEL DLIM D (IS=100U)
.ENDS

.SUBCKT 2SJ162 10 20 40
* TERMINALS: D G S
* Hitachi 160 Volt 7 Amp .171 ohm P-Channel Power MOSFET 08-06-1993
M1 1 2 3 3 DMOS L=1U W=1U
RD 100 1 110.4M
RS 30 3 25.28M
RG 20 2 17.4
CGS 2 3 760P
EGD 12 0 1 2 1
VFB 14 0 0
FFB 1 2 VFB 1
CGD 13 14 467P
R1 13 0 1
D1 12 13 DLIM
DDG 15 14 DCGD
R2 12 15 1
D2 15 0 DLIM
DSD 100 3 DSUB
LS 30 40 7.5N
LD 10 100 4N
.MODEL DMOS PMOS (LEVEL=3 THETA=90M VMAX=183K ETA=6.5M VTO=-.5 KP=1.109)
.MODEL DCGD D (CJO=467P VJ=.6 M=.68)
.MODEL DSUB D (IS=29N N=1.5 RS=61.4M BV=160 CJO=900P VJ=.8 M=.42 TT=252N)
.MODEL DLIM D (IS=100U)
.ENDS
  Reply With Quote
Old 7th February 2008, 09:41 PM   #496
diyAudio Member
 
EDDELARUE's Avatar
 
Join Date: Nov 2004
Location: Brasilia
Send a message via MSN to EDDELARUE Send a message via Skype™ to EDDELARUE
Hi syn08,
thanks for models. I´ll try use them.
  Reply With Quote
Old 8th February 2008, 05:14 PM   #497
diyAudio Member
 
jackinnj's Avatar
 
Join Date: Apr 2002
Location: Llanddewi Brefi, NJ
Quote:
Originally posted by gootee
We also need to get some magazines, like EDN et al, to write articles that could help convince the manufacturers that having spice models (and good spice models, at that) might _INCREASE SALES_ of their components.
3 years ago EDN had a design note in which the TL431 was used and the compensation network explicitly described -- the authors were two guys from Texas Instruments -- and had built a model for the TL431 --

It wasn't the model which TI has on its website -- the TI model correctly factors in the tempco of the device but is absent the reactive components.

I don't think that TI ever fixed the problem even though I talked to them and pointed out the incongruity. The ubiquitous TL431 costs about a nickel.
  Reply With Quote
Old 8th February 2008, 05:36 PM   #498
diyAudio Member
 
aparatusonitus's Avatar
 
Join Date: Jan 2004
Location: Split, Croatia
Quote:
Originally posted by jackinnj
3 years ago EDN had a design note in which the TL431 was used and the compensation network explicitly described -- the authors were two guys from Texas Instruments -- and had built a model for the TL431 --
Is it this one? Note that I named it TL431EDN just to know from where I got this particular model for TL431.

*Reference3 Pin Order: A, K, Ref
*TL431 model from EDN magazine: March 15,1990, page 180-181
*Programmable Precision Reference pkg:TO-92 2,3,1. pkg_DIP8 6,1,8
*Connections
* Anode
* | Cathode
* | | Reference
* | | |
.SUBCKT TL431EDN 3 2 1
*
*Reference input stage
Q1 3 1 10 QINPUT
RIN 10 2 500K
*
*Internal reference voltage
VR 20 2 DC 1.7791
RVR 20 2 1G
*
*Pole/Zero modeling
GM 0 30 10 20 1
RGM 30 0 1MEG
*Pole/Zeros: Pole 1= RGM & CP2, 10KHz
* Pole 2= RP2 & CP2, 60KHz
* Pole 3= CP1 & RZ1, 500KHz
*
CP1 30 40 15.9P
RZ1 40 0 20K
RP2 30 50 10MEG
CP2 50 0 0.265P
*Gain stage voltage clamp
DC 0 30 DCLAMP
*
*Output stage
GO 3 2 50 0 2.5U
DR 2 3 DNOM
*
.MODEL DNOM D(IS=100E-15 RS=7)
.MODEL DCLAMP D(IS=0.1)
.MODEL QINPUT NPN (BF=1 VAF=11.15)
.ENDS TL431EDN
__________________
Non é mai abbastanza...
  Reply With Quote
Old 8th February 2008, 06:59 PM   #499
syn08 is offline syn08  Canada
Account disabled at member's request
 
Join Date: Aug 2005
Location: Toronto
Quote:
Originally posted by aparatusonitus


Is it this one? Note that I named it TL431EDN just to know from where I got this particular model for TL431.


Yep, that's it.

The following model for the same circuit covers all of the temperature coefficient, AC gain, stability with capacitive loads (a big issue with TL431, and the reason why I prefer LM4041) noise and output impedance.

.SUBCKT TL431 A K R
Q1 3 2 1 0 NPN1 2.70
Q2 2 2 A 0 NPN1 1
R1 1 A 800 TC=0.00035
R2 4 2 2.4k
R3 4 3 7.2k
R4 5 4 3.28k
Q3 6 3 A 0 NPN1 1
R5 7 6 4k
Q4 10 5 7 0 NPN1 1
Q5 K R 5 0 NPN1 1
R6 2 12 1k
Q6 11 12 A 0 NPN1 0.2
Q9 K 11 13 0 NPN1 2
Q10 K 14 A 0 NPN1 10
R10 14 A 10k
R9 13 14 150
R7 K 8 800
Q7 10 10 8 0 PNP1 1
Q8 11 10 9 0 PNP1 1
D2 A K D1
D1 A 11 D3
R8 K 9 800
C1 K 11 20p
C2 6 3 20p
D3 11 R D2
.MODEL NPN1 NPN(Is=0.8e-14 BF=100 VAF=100 TF=0.5e-9 RB=50 IKF=10m KF=1e-16 AF=1 RE=10)
.MODEL PNP1 PNP(Is=1e-14 BF=50 VAF=50 TF=1e-8 IKF=2m KF=1e-16 AF=1)
.MODEL D1 D(Is=1e-13 Rs=10 CJO=20p)
.MODEL D2 D(Is=1e-13 Rs=10 CJO=2p BV=5 IBV=10u)
.MODEL D3 D(Is=1e-13 Rs=10 CJO=2p )
.ENDS TL431
  Reply With Quote
Old 27th February 2008, 12:17 AM   #500
fotios is offline fotios  Greece
diyAudio Member
 
fotios's Avatar
 
Join Date: Feb 2007
Location: Δραμα - North Greece
Quote:
Originally posted by john curl
Spice emulations? I don't need no stinking Spice emulations! (think bandito icon)
Count me in with Bob Pease on this one. ;-)
I just measure them in REAL-TIME with capacitors and a square wave generator, as I learned to do at my mentor's side, 40 years ago.
Hi John Curl

Maybe my -so many time delayed- post appears in the eyes of some PC software management experts a little funny, because as i have seen already the subject have inclined from your first thought, the expression of your thougt and the mean of your thought.
First i have to declare -with each modesty that become in a declaration so i ask the forgiveness of anyone thinks that i am arrogant - that i am also an expert in any kind of CAD software. For my job, i use for 9 years the medium quality CAD-CAE "EDWin" of Visionics which is a complete suite from schematic drawing to spice-thermal-electromagnetic analyser. I have also the high value "Altium" from the time which named "Protel" but the EDWin appeared from the begining to suit better in my demands of work. The spice simulator of EDWin works just fine and i think it is not of lower value of any other software simulator. Moreover it has an open spice model library so we can write the parameters of any model we want. I remembered before 6 years when i asked from Motorola the model of two transistors, they answered to me-for my luck was a Greek fellow worked at Motorola-that they don't have the models, but the fellow he linked me in two university databases, and i remembered that the one was the Berkeley university from which i got the models finally. For 3 hours i filed the parameters in the library of the EDSpice simulator.
After little time passed, i discovered finally that, for my amplifier model the simulator gave -in any kind of input signal- a wonderfull flat response from 0 to 1MHz! Fantastic! Something goes wrong i thinked. I tried for 1 week with each trick to destroy this incretible beauty waveform, but nothing changed. I tried a demo amplifier circuit which included in the software -something like the Leach with the double LTP in input- and this time indeed the simulator indicated a fall of response of this amplifier around 100KHz. Also an obvious distortion TIM & THD. My amplifier circuit-a version of it i published the schematic in this forum before few months-was a prototype based a little in the D.Self propositions, in my knoweledge of the circuits of different P.A. amplifiers produced in your country, and in some experiments that i made for some years. My circuit was very advanced-CCS in each stage eliminating bootstraps, Current mirrors, tripple darlington output of course full complementary, shared resistors in conjuction with local feedback resistors in the output devices, large capacitor in the AC coupled feedback ground node, etc- and after the carefully inspection of the demo circuit i discovered that it was a purposely shoddy circuit to show the effectiveness of spice simulator. From then i use the simulator only in cases of computing the static currents with two voltage markers accross each resistor (that means via the voltage drop, there is not any practical way to measure directly the current) and this gives only by 80-90% correct results and only up to 120Volt split supply (from this point and above the precision drops abraptly!). Also the simulator can compute with relativelly good precision the output power for given loads, so we can margin the values of the summing network resistors of the VI limitter of output devices. That is all. Everything furthermore it is most for academic discusion. And the reason IMHO it is that; the simulator it supposes the models of all the devices active or passive as ideal! And in real world the things are absolutelly different! Of course i suppose that the spice simulator can show its value, but only if someone has the courage to measure separately and in two different (to place a margin in variations) ambient conditions each of the endless parameters (many of which need instruments found only in nuclear physics laboratories) of each device and fill the long list of the spice model of device. I think for a big circuit 1 month it is enough without sleep.
I close my lengthy post, by say that; As many measurements (such as THD+noise, frequency response etc) are for consumer purposes only, something that it is also the spice simulation i.e. for students. For combatant designers and constructors the clearest way of estimation it is the square wave in input from a good generator of 10MHz (in other words with very small rise time), a dummy load in output (clear resistive) and a DSO. From the shape of square in output you can estimate: 1)From the rise time the bandwidth of the project 2)From the shape of the duty portions of square all the types of distortion and noise 3)From the shape of tilt line (concave or straight) of the duty portion in very low frequencies (under 100Hz) the good or bad coupling of all local and of whole the feedback loop 4)From the amount of tilt again in the low frequencies the force of power supply, the low output impedance (if there is need for more output devices) and finally the tight control in bass reproduction (such the damping? Factor? What is this? It is eatable?).

With Respect
Fotios Anagnostou
  Reply With Quote

Reply


Hide this!Advertise here!
Thread Tools Search this Thread
Search this Thread:

Advanced Search

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are Off
Refbacks are Off


Similar Threads
Thread Thread Starter Forum Replies Last Post
Need help with Spice simulation overmind Everything Else 4 23rd December 2002 04:58 PM


New To Site? Need Help?

All times are GMT. The time now is 03:04 PM.


vBulletin Optimisation provided by vB Optimise (Pro) - vBulletin Mods & Addons Copyright © 2014 DragonByte Technologies Ltd.
Copyright ©1999-2014 diyAudio

Content Relevant URLs by vBSEO 3.3.2