The Cyber-Spy.Com Usenet Archive Feeds Directly
From The Open And Publicly Available Newsgroup
This Group And Thousands Of Others Are Available
On Most IS NNTP News Servers On Port 119.
Cyber-Spy.Com Is NOT Responsible For Any Topic,
Opinions Or Content Posted To This Or Any Other
Newsgroup. This Web Archive Of The Newsgroup And
Posts Are For Informational Purposes Only.
From: firstname.lastname@example.org (Paul Burridge)
Subject: Re: Transistor amplifiers v. frequency in SPICE
Date: 12 Jan 2003 04:53:20 -0800
NNTP-Posting-Date: 12 Jan 2003 12:53:20 GMT
Mike Monett wrote in message news:<3E20D1C8.166C@sneakemail.com>...
> Paul Burridge wrote:
> [... see original for CKT file]
> I have to admire your energy and persistence. SPICE is not easy to learn,
> and you are doing a good job of asking the right questions.
THanks, Mike. I can use all the encouragement I get!
> A couple of quick comments. Your SPICE should be able to plot the AC
> response curve instead of having to do each frequency manually. What
> version are you using?
I think the version is shown on the .ckt file I posted. However, I'll
the instruction line for the AC sweep and maybe from that you can see
> The emitter and collector resistors are way too high for the frequency
> response you are asking. MicroCap calculates the ft at 1.72MHz under
> these conditions. Here are some suggestions you might want to try:
> Change the resistors to the following values:
> R1 = 1k
> R8 = 1k
> R7 = 750
> R2 = 470
> Change C2 to 1uF.
> Now plot the frequency response. It should improve, but it still falls
> off rapidly.
Thanks for that. The reason for the high value resistors was that I
trying to keep Zin as high as possible, since the real signal source
I am modelling has a quite high Z. Yes, I know. Get myself a FET! :-)
> You should be able to find the operating point information in the
> printout, and it should indicate the transistor parameters such as
> collector, base and emitter current, and also the beta and ft. These are
> rough guides to how the transistor is functioning.
Indeed. I do use the DC .op function quite often and find it very
> Try changing to a higher frequency transistor like the MMBR941:
> .MODEL MMBR941 NPN(BF=110 VAF=80 VAR=8.0 RC=.54 RB=.08 RE=.009 IKF=35M
> + ISE=0.45E-14 TF=0.111E-10 TR=0.80E-09 ITF=0.20E-01 VTF=0.33E+01
> + CJC=0.074E-12 CJE=0.064E-12 XTI=3.0 NE=1.5 ISC=0.15E-14 EG=1.11
> + XTB=1.5 BR=2.86 VJC=0.75 VJE=0.75 IS=0.50E-15 MJC=0.33 MJE=0.33 XTF=4.0
> + IKR=0.35E-01 KF=0.1E-14 NC=1.7 FC=0.50 RBM=.06 IRB=0.50E-02 XCJC=0.5)
> Now you should see a flat frequency response past 1GHz. Don't believe it
> for a minute:)
Thanks for posting the model. If it's not in my library I'll add it.
> Add a 50 ohm resistor in series with the signal source. The frequency
> response falls off dramatically.
> Add a 5pF cap from the collector to ground to simulate stray trace and
> pin capacity. The frequency response falls even faster.
> Add a 1pf from the collector to the base. The frequency response falls
> faster still.
> These are simple ways to see how a circuit is working, and to get a
> feeling for the real-world effect of strays. It tells you for wideband
> circuits, you need low impedance which means high current.
Fascinating. Thanks for a valuable insight into the difference between
SPICEWORLD and the real world! BTW and on this subject, would I be
to assume that SPICE models take no account of component lead-length?
example, a real-world coupling capacitor has an optimal value with
impedance at the desired (radio)frequency due to the inductance of the
creating a series tuned circuit of sorts, whereas the SPICE capacitor
"perfect" and bigger (values)are always better and present less
> But first thing is to get SPICE to plot the AC response curves for you.
> Lets see if we can help!
Many thanks again. I'm always grateful for informed input to my
I'll establish the relevant instruction sequence and append it to this
Go Back To The Cyber-Spy.Com
Usenet Web Archive Index Of
The sci.electronics.design Newsgroup