LTSpice Modelling of BJT question - Page 1
Forum section: electronics / projects

author: HackedFridgeMagnet
author_rank: Super Contributor
timestamp: June 09, 2012, 03:02:28 am
content: HiI am having a bit of trouble modelling a transistor in LTSpice.The model that I transferred into LTSpice doesn't behave like an NPN should.I tried as both a Subckt and as a standard bjt.the manufacturers model isCode:************************************************************* PBSS4560PA** NXP Semiconductors** Low VCEsat NPN BISS transistor* IC = 6 A* VCEO = 60 V* hFE = typ. 325 @ 2V/2A**** Package: SOT 1061** Package Pin 1: Base* Package Pin 2: Emitter* Package Pin 3: Collector*** Extraction date (week/year): 20/2009* Simulator: Spice 3************************************************************#.SUBCKT PBSS4560PA 1 2 3*Q1 1 2 3 PBSS4560PAD1 2 1 DIODE** Diode D1 is dedicated to improve modeling of reversemode* operation and does not reflect a physical device.*.MODEL PBSS4560PA NPN+ IS = 1.437E-012+ NF = 0.956+ ISE = 5.283E-014+ NE = 1.354+ BF = 513+ IKF = 3.03+ VAF = 17.1+ NR = 0.9558+ ISC = 2.905E-016+ NC = 0.9863+ BR = 141.1+ IKR = 12.81+ VAR = 18+ RB = 9.55+ IRB = 0.0007+ RBM = 1.9+ RE = 0.01754+ RC = 0.02693+ XTB = 0+ EG = 1.11+ XTI = 3+ CJE = 7.404E-010+ VJE = 0.7269+ MJE = 0.3563+ TF = 9.5E-010+ XTF = 5+ VTF = 1+ ITF = 2+ PTF = 0+ CJC = 7.17E-011+ VJC = 0.045+ MJC = 0.2+ XCJC = 1+ TR = 6E-009+ CJS = 0+ VJS = 0.75+ MJS = 0.333+ FC = 0.98.MODEL DIODE D+ IS = 1.513E-013+ N = 1.001+ BV = 1000+ IBV = 0.001+ RS = 430.5+ CJO = 0+ VJ = 1+ M = 0.5+ FC = 0+ TT = 0+ EG = 1.11+ XTI = 3.ENDS*This model seemed to oscillate so I then tried to use a simpler model from format models in the Standard.bjt fileI tried to convert the PBSS4560PA into LTSpice without the extra components as:Code:.model PBSS4560PA NPN(IS=1.437E-012 NF=0.956 ISE=5.283E-014 NE=1.354 BF=513 IKF=3.03 VAF=17.1 NR=0.9558 ISC=2.905E-016 NC=0.9863 BR=141.1 IKR=12.81 VAR=18 RB=9.55 IRB=1.00E-06 RBM=1.9 RE=0.01754 RC=0.02693 XTB=0 EG=1.11 XTI=3 CJE=7.404E-010 VJE=0.7269 MJE=0.3563 TF=9.5E-010 XTF=5 VTF=1 ITF=2 PTF=0 CJC=7.17E-011 VJC=0.045 MJC=0.2 XCJC=1 TR=6E-009 CJS=0 VJS=0.75 MJS=0.333 FC=0.98 Vceo=60 Icrating=5 mfg=NXPThis_model_is_fail)as an example the BC547C is (from standard.bjt):Code:.model BC547C NPN(IS=4.679E-14 NF=1.01 ISE=2.642E-15 NE=1.581 BF=458.7 IKF=0.1371 VAF=52.64 NR=1.019 ISC=2.337E-14 NC=1.164 BR=11.57 IKR=0.1144 VAR=364.5 RB=1 IRB=1.00E-06 RBM=1 RE=0.2598 RC=1 XTB=0 EG=1.11 XTI=3 CJE=1.229E-11 VJE=0.5591 MJE=0.3385 TF=4.689E-10 XTF=160 VTF=2.828 ITF=0.8842 PTF=0 CJC=4.42E-12 VJC=0.1994 MJC=0.2782 XCJC=0.6193 TR=1.00E-32 CJS=0 VJS=0.75 MJS=0.333 FC=0.7936 Vceo=45 Icrating=100m mfg=Philips)I also tried to make a hybrid model to find the problematic parameters.Code:.model PBSS4560PAHybrid NPN(IS=1.437E-012 NF=0.956 ISE=5.283E-014 NE=1.354 BF=513 IKF=3.03 VAF=17.1 NR=0.9558 ISC=2.905E-016 NR=0.9558 BR=11.57 IKR=12.81 VAR=18 RB=9.55 IRB=1.00E-06 RBM=1.9 RE=0.01754 RC=0.02693 XTB=0 EG=1.11 XTI=3 CJE=7.404E-010 VJE=0.7269 MJE=0.3563 TF=9.5E-010 XTF=5 VTF=1 ITF=2 PTF=0 CJC=4.42E-12 VJC=0.1994 MJC=0.2782 XCJC=0.6193 TR=6E-009 CJS=0 VJS=0.75 MJS=0.333 FC=0.98 Vceo=60 Icrating=5 mfg=NXP)You can see the waveforms in the picture and or try the models.BR seems to be the killer (Ideal maximum reverse BETA) I guess it must be dependant on using a subckt type model.But other parameters also have bad effects. on about page 68 of the model parameter explanations.Would somebody be able to suggest the best way to approach this, as I want a decent model that is as least as complex as the BC547C, but behaves mostly as the PBSS4560PA will actually behave.So to reiterate, I want to get a model of the PBSS4560PA and the complementry PBSS5560PA as well, so If somebody can tell me either what my mistakes are and/or how best to approach these kind of modelling issues, it would be appreciated.ps.Heres a link to what might be explanations of the parametershttp://www.google.com.au/url?sa=t&rct=j&q=true-hspice%20device%20models%20reference%20manual&source=web&cd=4&ved=0CFUQFjAD&url=http%3A%2F%2Fwww.ece.neu.edu%2Fcourses%2Feece7353%2F2012sp%2FHspice%2FHspice_Quick_Reference.pdf&ei=e7fST_jKOu2QiAewwbXsAg&usg=AFQjCNH7wUgTu11WNYXPoVrIu2NmaTuORw&cad=rja

author: amspire
author_rank: Super Contributor
timestamp: June 09, 2012, 03:37:10 am
content: I am not sure I see any oscillation. Can you point them out?The small peak on the BC547C is not an oscillation - that is just the effect of the base-collector capacitance.The last transistor with the red trace has massive collector-base leakage current, so one or two parameters have to be way out.Two numbers seem crazy. The BR reverse gain of 141, and even worse, the VJC of 0.045. Should be much bigger - the number looks ridiculous. Perhaps it was meant to be 0.45 V instead of 0.045 V.To check a model, start duplicating curves in the data sheet. If they do not match, the model is no good.Richard.

author: HackedFridgeMagnet
author_rank: Super Contributor
timestamp: June 09, 2012, 06:06:51 am
content: Initially I put the whole .subckt model into my switched mode circuit. I did not keep a copy of that attempt. That was the circuit that oscillated.Then I decided to just rip the transistor part out of the .subckt model of the PBSS4560PA provided by NXP.I knew this may be flawed thinking but I thought that it might give my a good approximation. It didn't.QuoteThat seems like a good way to do it.I just wonder why the model seems so wrong. I will have a go at duplicating the curves.

author: HackedFridgeMagnet
author_rank: Super Contributor
timestamp: June 09, 2012, 08:21:25 am
content: Here is a forward gain characteristicIt doesn't look very accurate but it doesn't look out of order either.This model is the NXP model with only the BR=141.1 changed to 14.1, not that this would effect the hfe characteristic anyway.Viewers will have to scroll right to see the current scale.Code:.model PBSS4560PAHybrid NPN(IS=1.437E-012 NF=0.956 ISE=5.283E-014 NE=1.354 BF=513 IKF=3.03 VAF=17.1 NR=0.9558 ISC=2.905E-016 NC=0.9863 BR=14.1 IKR=12.81 VAR=18 RB=9.55 IRB=1.00E-06 RBM=1.9 RE=0.01754 RC=0.02693 XTB=0 EG=1.11 XTI=3 CJE=7.404E-010 VJE=0.7269 MJE=0.3563 TF=9.5E-010 XTF=5 VTF=1 ITF=2 PTF=0 CJC=7.17E-011 VJC=0.045 MJC=0.2 XCJC=1 TR=6E-009 CJS=0 VJS=0.75 MJS=0.333 FC=0.98 Vceo=60 Icrating=5 mfg=NXP)

author: HackedFridgeMagnet
author_rank: Super Contributor
timestamp: June 10, 2012, 12:57:36 pm
content: Ok I think I found the problem (after reading the data sheet).The transistor in question is not the type of transistor I am looking for. I guess I should have read the data sheet instead of just seeing what I wanted to see.It is known as a Low Vce Saturation transistor, to be used as the pass transistor, in a high/medium current application.All I wanted was a fairly normal, high gain, relatively fast, switching transistor, but I got these instead.But it's purpose in my circuit is to stay out of deep into saturation.My only excuse is I bought these at the tail end of an order after midnight.So the model is probably ok, and it tells me not to use this transistor.http://www.nxp.com/documents/application_note/AN10360.pdfI will look for something else.

author: amspire
author_rank: Super Contributor
timestamp: June 10, 2012, 01:51:52 pm
content: Quote from: HackedFridgeMagnet on June 10, 2012, 12:57:36 pmThat probably is no problem with that transistor you selected if the data sheet curves look OK. There is usually nothing wrong with low Vce saturation transistors.It is the case though that Spice models vary hugely in accuracy. Some model are great. Some are made by people who do not understand the parameters properly. That seemed a very odd model to me. The switching speed in LTSpice looked much slower then I would expect. but I did not investigate.Just about to shut down my PC for the night, but I can take a second look tomorrow if you want me to.Richard.