class c rf amp with bfr93a

Hi to all.
I'm looking to make a small 433Mhz transmitter using bfr93's.
I want to have a oscillator , followed by a small class c amp , both
using bfr93.
Tho oscillator will be a standard Colpits oscillator , with a SAW
resonator.
I'd like to attach a class c amp (followed by filtering obviously) to
boost the power.
I've got a spice model for the BFR93 , from NXP.
What I want to know is will a simulation of this very non linear
application of the bfr93
provide any usefull results at all , or will I see total junk.
A LTSpice cct is attached , simulating a BFR93 as a class c amp.It's
not
a finished cct , so the component values are not final.I'd just like
to know if the results
that I get are realistic. If I built that cct , is that what I'd get.I
do realise that
I have not included any paracitics in the components yet.
Cheers
Rob

On 08/25/2010 06:12 AM, neddie wrote:
Hi to all.
I'm looking to make a small 433Mhz transmitter using bfr93's.
I want to have a oscillator , followed by a small class c amp , both
using bfr93.
Tho oscillator will be a standard Colpits oscillator , with a SAW
resonator.
I'd like to attach a class c amp (followed by filtering obviously) to
boost the power.
I've got a spice model for the BFR93 , from NXP.
What I want to know is will a simulation of this very non linear
application of the bfr93
provide any usefull results at all , or will I see total junk.
A LTSpice cct is attached , simulating a BFR93 as a class c amp.It's
not
a finished cct , so the component values are not final.I'd just like
to know if the results
that I get are realistic. If I built that cct , is that what I'd get.I
do realise that
I have not included any paracitics in the components yet.
Cheers
Rob

All I get when I try to read that file in LTSpice are tons-o-errors.

If the BRF93 is being marketed for service at UHF then the model should
work -- and there seem to be the right parasitic components in the model
to imply this. SPICE is all about nonlinear circuit analysis, so as
long as either you're not driving the transistor into saturation, or as
long as the model is taking storage effects into account, then the model
should be representative.

Whether you are correctly taking all of _your_ circuit parasitics into
account is your problem. I'm sure there are folks out there that can
model a circuit at that frequency and build it with confidence; I'm not
one of them.

Tim Wescott wrote:
[snip]

All I get when I try to read that file in LTSpice are tons-o-errors.


Yup. Rob, if you publish circuits that way make sure the models are in
it as well. It won't run on other people's PC unless they also have the
same model.


If the BRF93 is being marketed for service at UHF then the model should
work -- and there seem to be the right parasitic components in the model
to imply this. SPICE is all about nonlinear circuit analysis, so as
long as either you're not driving the transistor into saturation, or as
long as the model is taking storage effects into account, then the model
should be representative.

Whether you are correctly taking all of _your_ circuit parasitics into
account is your problem. I'm sure there are folks out there that can
model a circuit at that frequency and build it with confidence; I'm not
one of them.


You can drive it pretty hard but keep in mind that SPICE does not have a
*PHUT* function.
[snip]

On Wed, 25 Aug 2010 15:19:23 -0700, Joerg <invalid_at_invalid.invalid
wrote:

Tim Wescott wrote:
[snip]
All I get when I try to read that file in LTSpice are tons-o-errors.

Yup. Rob, if you publish circuits that way make sure the models are in
it as well. It won't run on other people's PC unless they also have the
same model.


If the BRF93 is being marketed for service at UHF then the model should
work -- and there seem to be the right parasitic components in the model
to imply this. SPICE is all about nonlinear circuit analysis, so as
long as either you're not driving the transistor into saturation, or as
long as the model is taking storage effects into account, then the model
should be representative.

Whether you are correctly taking all of _your_ circuit parasitics into
account is your problem. I'm sure there are folks out there that can
model a circuit at that frequency and build it with confidence; I'm not
one of them.

You can drive it pretty hard but keep in mind that SPICE does not have a
*PHUT* function.
[snip]

Of course it does... it's called a (*PHUT* Macro. I use them all
the time to monitor otherwise obscure failure mechanisms... like "hot
electron" effects in MOS device gates.

Jim Thompson wrote:
On Wed, 25 Aug 2010 15:19:23 -0700, Joerg <invalid_at_invalid.invalid
wrote:

Tim Wescott wrote:
[snip]
All I get when I try to read that file in LTSpice are tons-o-errors.

Yup. Rob, if you publish circuits that way make sure the models are in
it as well. It won't run on other people's PC unless they also have the
same model.


If the BRF93 is being marketed for service at UHF then the model should
work -- and there seem to be the right parasitic components in the model
to imply this. SPICE is all about nonlinear circuit analysis, so as
long as either you're not driving the transistor into saturation, or as
long as the model is taking storage effects into account, then the model
should be representative.

Whether you are correctly taking all of _your_ circuit parasitics into
account is your problem. I'm sure there are folks out there that can
model a circuit at that frequency and build it with confidence; I'm not
one of them.

You can drive it pretty hard but keep in mind that SPICE does not have a
*PHUT* function.
[snip]

Of course it does... it's called a (*PHUT* Macro. I use them all
the time to monitor otherwise obscure failure mechanisms... like "hot
electron" effects in MOS device gates.


Sure you can write your own macros. But there are no native voltage
limits on device.

It's a classic pitfall in RF where many people think
small-signal most of the time or the professors taught that: Class A amp
with a resonant circuit or just a choke on the collector, works nicely
in SPICE, works nicely in real life. Then the engineer does something to
drop the input below cutoff for some reason, collector flies up, way
past abs max ... *WHADDABAM*

Tim Wescott wrote:
On 08/25/2010 06:12 AM, neddie wrote:
Hi to all.
I'm looking to make a small 433Mhz transmitter using bfr93's.
I want to have a oscillator , followed by a small class c amp , both
using bfr93.
Tho oscillator will be a standard Colpits oscillator , with a SAW
resonator.
I'd like to attach a class c amp (followed by filtering obviously) to
boost the power.
I've got a spice model for the BFR93 , from NXP.
What I want to know is will a simulation of this very non linear
application of the bfr93
provide any usefull results at all , or will I see total junk.
A LTSpice cct is attached  , simulating a BFR93 as a class c amp.It's
not
a finished cct , so the component values are not final.I'd just like
to know if the results
that I get are realistic. If I built that cct , is that what I'd get.I
do realise that
I have not included any paracitics in the components yet.
Cheers
Rob

All I get when I try to read that file in LTSpice are tons-o-errors.

Yup. Rob, if you publish circuits that way make sure the models are in
it as well. It won't run on other people's PC unless they also have the
same model.

If the BRF93 is being marketed for service at UHF then the model should
work -- and there seem to be the right parasitic components in the model
to imply this.  SPICE is all about nonlinear circuit analysis, so as
long as either you're not driving the transistor into saturation, or as
long as the model is taking storage effects into account, then the model
should be representative.

Whether you are correctly taking all of _your_ circuit parasitics into
account is your problem.  I'm sure there are folks out there that can
model a circuit at that frequency and build it with confidence; I'm not
one of them.

You can drive it pretty hard but keep in mind that SPICE does not have a
*PHUT* function. On the computer you can make a virtual kilovolt-level
amp with a BFR93 which then in practice will explode violently.

But yeah, one can simulate RF stuff and it tends to come out alright on
the circuit board.

--
Regards, Joerg

http://www.analogconsultants.com/

"gmail" domain blocked because of excessive spam.
Use another domain or send PM.

On Aug 26, 12:19 am, Joerg <inva...@invalid.invalid> wrote:
Tim Wescott wrote:
On 08/25/2010 06:12 AM, neddie wrote:
Hi to all.
I'm looking to make a small 433Mhz transmitter using bfr93's.
I want to have a oscillator , followed by a small class c amp , both
using bfr93.
Tho oscillator will be a standard Colpits oscillator , with a SAW
resonator.
I'd like to attach a class c amp (followed by filtering obviously) to
boost the power.
I've got a spice model for the BFR93 , from NXP.
What I want to know is will a simulation of this very non linear
application of the bfr93
provide any usefull results at all , or will I see total junk.
A LTSpice cct is attached , simulating a BFR93 as a class c amp.It's
not
a finished cct , so the component values are not final.I'd just like
to know if the results
that I get are realistic. If I built that cct , is that what I'd get.I
do realise that
I have not included any paracitics in the components yet.
Cheers
Rob
All I get when I try to read that file in LTSpice are tons-o-errors.
Yup. Rob, if you publish circuits that way make sure the models are in
it as well. It won't run on other people's PC unless they also have the
same model.

If the BRF93 is being marketed for service at UHF then the model should
work -- and there seem to be the right parasitic components in the model
to imply this. SPICE is all about nonlinear circuit analysis, so as
long as either you're not driving the transistor into saturation, or as
long as the model is taking storage effects into account, then the model
should be representative.
Whether you are correctly taking all of _your_ circuit parasitics into
account is your problem. I'm sure there are folks out there that can
model a circuit at that frequency and build it with confidence; I'm not
one of them.
You can drive it pretty hard but keep in mind that SPICE does not have a
*PHUT* function. On the computer you can make a virtual kilovolt-level
amp with a BFR93 which then in practice will explode violently.

But yeah, one can simulate RF stuff and it tends to come out alright on
the circuit board.

--
Regards, Joerg

http://www.analogconsultants.com/

"gmail" domain blocked because of excessive spam.
Use another domain or send PM.

Thanks for the help guys .Your answers have helped.
I don't plan on getting huge powers , say 20mW , but
keeping an eye on the max current and collector voltage may be
a good idea :0)
The data sheet does not have parameters for the voltage and currents
that I'm
looking to use , but I'm hoping that they will at least get me in to
the ballpark.
I'm hoping the sims will be accurate enough to guide me from there.
This RF stuff is tough!!
I tried to embed the spice model into the CCT , that is why it fails :
0(
This is the CCT.

Version 4
SHEET 1 1300 1580
WIRE 48 144 -256 144
WIRE -256 192 -256 144
WIRE 48 192 48 144
WIRE -256 304 -256 272
WIRE -240 304 -256 304
WIRE -80 304 -96 304
WIRE -16 304 -80 304
WIRE -256 320 -256 304
WIRE -368 368 -496 368
WIRE -320 368 -368 368
WIRE -80 368 -80 304
WIRE -16 368 -16 304
WIRE -496 480 -496 448
WIRE -368 480 -368 448
WIRE -368 480 -496 480
WIRE -256 480 -256 416
WIRE -256 480 -368 480
WIRE -80 480 -80 432
WIRE -80 480 -256 480
WIRE -16 480 -16 448
WIRE -16 480 -80 480
WIRE 48 480 48 272
WIRE 48 480 -16 480
WIRE -368 496 -368 480
FLAG -368 496 0
SYMBOL voltage -496 352 R0
WINDOW 3 -14 181 Left 0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR Value SINE(0 1 433.92Meg)
SYMATTR InstName V1
SYMBOL ind -272 176 R0
SYMATTR InstName L1
SYMATTR Value 470n
SYMBOL res -384 352 R0
SYMATTR InstName R1
SYMATTR Value 1k
SYMBOL voltage 48 176 R0
SYMATTR InstName V2
SYMATTR Value 6
SYMBOL npn2 -320 320 R0
SYMATTR InstName Q1
SYMATTR Value BFR93A
SYMATTR Prefix X
SYMBOL cap -176 288 R90
WINDOW 0 0 32 VBottom 0
WINDOW 3 32 32 VTop 0
SYMATTR InstName C1
SYMATTR Value 100n
SYMBOL res -32 352 R0
SYMATTR InstName R2
SYMATTR Value 200
SYMBOL ind -80 288 R90
WINDOW 0 5 56 VBottom 0
WINDOW 3 32 56 VTop 0
SYMATTR InstName L2
SYMATTR Value 50n
SYMBOL cap -96 368 R0
SYMATTR InstName C2
SYMATTR Value 2p
TEXT -64 1288 Left 0 !.tran 50n


This is the MODEL file , actually sub-cct.

* Filename: BFR93A_SPICE.PRM
* BFR93A SPICE MODEL
* PHILIPS SEMICONDUCTORS
* Date : September 1995
*
* PACKAGE : SOT23 DIE MODEL : BFR91A
* 1: COLLECTOR; 2: BASE; 3: EMITTER;
.SUBCKT BFR93A 1 2 3
Q1 6 5 7 7 BFR91A
* SOT23 parasitic model
Lb 4 5 .4n
Le 7 8 .83n
L1 2 4 .35n
L2 1 6 .17n
L3 3 8 .35n
Ccb 4 6 71f
Cbe 4 8 2f
Cce 6 8 71f
*
* PHILIPS SEMICONDUCTORS
Version: 1.0
* Filename: BFR91A.PRM Date: Feb
1992
*
.MODEL BFR91A NPN
+ IS = 1.32873E-015
+ BF = 1.02000E+002
+ NF = 1.00025E+000
+ VAF = 5.19033E+001
+ IKF = 8.15511E+000
+ ISE = 1.39029E-014
+ NE = 1.51292E+000
+ BR = 1.76953E+001
+ NR = 9.94038E-001
+ VAR = 3.28032E+000
+ IKR = 1.00000E+001
+ ISC = 1.04297E-015
+ NC = 1.18993E+000
+ RB = 1.00000E+001
+ IRB = 1.00000E-006
+ RBM = 1.00000E+001
+ RE = 7.63636E-001
+ RC = 9.00000E+000
+ EG = 1.11000E+000
+ XTI = 3.00000E+000
+ CJE = 2.03216E-012
+ VJE = 6.00000E-001
+ MJE = 2.90076E-001
+ TF = 6.55790E-012
+ XTF = 3.89752E+001
+ VTF = 1.09308E+001
+ ITF = 5.21078E-001
+ CJC = 1.00353E-012
+ VJC = 3.40808E-001
+ MJC = 1.94223E-001
.ENDS

neddie wrote:
On Aug 26, 12:19 am, Joerg <inva...@invalid.invalid> wrote:
Tim Wescott wrote:
On 08/25/2010 06:12 AM, neddie wrote:
Hi to all.
I'm looking to make a small 433Mhz transmitter using bfr93's.
I want to have a oscillator , followed by a small class c amp , both
using bfr93.
Tho oscillator will be a standard Colpits oscillator , with a SAW
resonator.
I'd like to attach a class c amp (followed by filtering obviously) to
boost the power.
I've got a spice model for the BFR93 , from NXP.
What I want to know is will a simulation of this very non linear
application of the bfr93
provide any usefull results at all , or will I see total junk.
A LTSpice cct is attached , simulating a BFR93 as a class c amp.It's
not
a finished cct , so the component values are not final.I'd just like
to know if the results
that I get are realistic. If I built that cct , is that what I'd get.I
do realise that
I have not included any paracitics in the components yet.
Cheers
Rob
All I get when I try to read that file in LTSpice are tons-o-errors.
Yup. Rob, if you publish circuits that way make sure the models are in
it as well. It won't run on other people's PC unless they also have the
same model.

If the BRF93 is being marketed for service at UHF then the model should
work -- and there seem to be the right parasitic components in the
model
to imply this. SPICE is all about nonlinear circuit analysis, so as
long as either you're not driving the transistor into saturation, or as
long as the model is taking storage effects into account, then the
model
should be representative.
Whether you are correctly taking all of _your_ circuit parasitics into
account is your problem. I'm sure there are folks out there that can
model a circuit at that frequency and build it with confidence; I'm not
one of them.
You can drive it pretty hard but keep in mind that SPICE does not have a
*PHUT* function. On the computer you can make a virtual kilovolt-level
amp with a BFR93 which then in practice will explode violently.

But yeah, one can simulate RF stuff and it tends to come out alright on
the circuit board.

--
Regards, Joerg

http://www.analogconsultants.com/

"gmail" domain blocked because of excessive spam.
Use another domain or send PM.

Thanks for the help guys .Your answers have helped.
I don't plan on getting huge powers , say 20mW , but
keeping an eye on the max current and collector voltage may be
a good idea :0)
The data sheet does not have parameters for the voltage and currents
that I'm
looking to use , but I'm hoping that they will at least get me in to
the ballpark.
I'm hoping the sims will be accurate enough to guide me from there.
This RF stuff is tough!!
I tried to embed the spice model into the CCT , that is why it fails :
0(
This is the CCT.

Version 4
SHEET 1 1300 1580
WIRE 48 144 -256 144
WIRE -256 192 -256 144
WIRE 48 192 48 144
WIRE -256 304 -256 272
WIRE -240 304 -256 304
WIRE -80 304 -96 304
WIRE -16 304 -80 304
WIRE -256 320 -256 304
WIRE -368 368 -496 368
WIRE -320 368 -368 368
WIRE -80 368 -80 304
WIRE -16 368 -16 304
WIRE -496 480 -496 448
WIRE -368 480 -368 448
WIRE -368 480 -496 480
WIRE -256 480 -256 416
WIRE -256 480 -368 480
WIRE -80 480 -80 432
WIRE -80 480 -256 480
WIRE -16 480 -16 448
WIRE -16 480 -80 480
WIRE 48 480 48 272
WIRE 48 480 -16 480
WIRE -368 496 -368 480
FLAG -368 496 0
SYMBOL voltage -496 352 R0
WINDOW 3 -14 181 Left 0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR Value SINE(0 1 433.92Meg)
SYMATTR InstName V1
SYMBOL ind -272 176 R0
SYMATTR InstName L1
SYMATTR Value 470n
SYMBOL res -384 352 R0
SYMATTR InstName R1
SYMATTR Value 1k
SYMBOL voltage 48 176 R0
SYMATTR InstName V2
SYMATTR Value 6
SYMBOL npn2 -320 320 R0
SYMATTR InstName Q1
SYMATTR Value BFR93A
SYMATTR Prefix X
SYMBOL cap -176 288 R90
WINDOW 0 0 32 VBottom 0
WINDOW 3 32 32 VTop 0
SYMATTR InstName C1
SYMATTR Value 100n
SYMBOL res -32 352 R0
SYMATTR InstName R2
SYMATTR Value 200
SYMBOL ind -80 288 R90
WINDOW 0 5 56 VBottom 0
WINDOW 3 32 56 VTop 0
SYMATTR InstName L2
SYMATTR Value 50n
SYMBOL cap -96 368 R0
SYMATTR InstName C2
SYMATTR Value 2p
TEXT -64 1288 Left 0 !.tran 50n


This is the MODEL file , actually sub-cct.

* Filename: BFR93A_SPICE.PRM
* BFR93A SPICE MODEL
* PHILIPS SEMICONDUCTORS
* Date : September 1995
*
* PACKAGE : SOT23 DIE MODEL : BFR91A
* 1: COLLECTOR; 2: BASE; 3: EMITTER;
.SUBCKT BFR93A 1 2 3
Q1 6 5 7 7 BFR91A
* SOT23 parasitic model
Lb 4 5 .4n
Le 7 8 .83n
L1 2 4 .35n
L2 1 6 .17n
L3 3 8 .35n
Ccb 4 6 71f
Cbe 4 8 2f
Cce 6 8 71f
*
* PHILIPS SEMICONDUCTORS
Version: 1.0
* Filename: BFR91A.PRM Date: Feb
1992
*
.MODEL BFR91A NPN
+ IS = 1.32873E-015
+ BF = 1.02000E+002
+ NF = 1.00025E+000
+ VAF = 5.19033E+001
+ IKF = 8.15511E+000
+ ISE = 1.39029E-014
+ NE = 1.51292E+000
+ BR = 1.76953E+001
+ NR = 9.94038E-001
+ VAR = 3.28032E+000
+ IKR = 1.00000E+001
+ ISC = 1.04297E-015
+ NC = 1.18993E+000
+ RB = 1.00000E+001
+ IRB = 1.00000E-006
+ RBM = 1.00000E+001
+ RE = 7.63636E-001
+ RC = 9.00000E+000
+ EG = 1.11000E+000
+ XTI = 3.00000E+000
+ CJE = 2.03216E-012
+ VJE = 6.00000E-001
+ MJE = 2.90076E-001
+ TF = 6.55790E-012
+ XTF = 3.89752E+001
+ VTF = 1.09308E+001
+ ITF = 5.21078E-001
+ CJC = 1.00353E-012
+ VJC = 3.40808E-001
+ MJC = 1.94223E-001
.ENDS

Sorry Rob, this one errors, says "Too few nodes, version 1.0". Whatever
that means.

--
Regards, Joerg

http://www.analogconsultants.com/

"gmail" domain blocked because of excessive spam.
Use another domain or send PM.

"Joerg" <invalid_at_invalid.invalid> schrieb im Newsbeitrag
news:8dqrcfFcnhU1_at_mid.individual.net...
neddie wrote:
On Aug 26, 12:19 am, Joerg <inva...@invalid.invalid> wrote:
Tim Wescott wrote:
On 08/25/2010 06:12 AM, neddie wrote:
Hi to all.
I'm looking to make a small 433Mhz transmitter using bfr93's.
I want to have a oscillator , followed by a small class c amp , both
using bfr93.
Tho oscillator will be a standard Colpits oscillator , with a SAW
resonator.
I'd like to attach a class c amp (followed by filtering obviously) to
boost the power.
I've got a spice model for the BFR93 , from NXP.
What I want to know is will a simulation of this very non linear
application of the bfr93
provide any usefull results at all , or will I see total junk.
A LTSpice cct is attached , simulating a BFR93 as a class c amp.It's
not
a finished cct , so the component values are not final.I'd just like
to know if the results
that I get are realistic. If I built that cct , is that what I'd get.I
do realise that
I have not included any paracitics in the components yet.
Cheers
Rob
All I get when I try to read that file in LTSpice are tons-o-errors.
Yup. Rob, if you publish circuits that way make sure the models are in
it as well. It won't run on other people's PC unless they also have the
same model.

If the BRF93 is being marketed for service at UHF then the model should
work -- and there seem to be the right parasitic components in the
model
to imply this. SPICE is all about nonlinear circuit analysis, so as
long as either you're not driving the transistor into saturation, or as
long as the model is taking storage effects into account, then the
model
should be representative.
Whether you are correctly taking all of _your_ circuit parasitics into
account is your problem. I'm sure there are folks out there that can
model a circuit at that frequency and build it with confidence; I'm not
one of them.
You can drive it pretty hard but keep in mind that SPICE does not have a
*PHUT* function. On the computer you can make a virtual kilovolt-level
amp with a BFR93 which then in practice will explode violently.

But yeah, one can simulate RF stuff and it tends to come out alright on
the circuit board.

--
Regards, Joerg

http://www.analogconsultants.com/

"gmail" domain blocked because of excessive spam.
Use another domain or send PM.
Thanks for the help guys .Your answers have helped.
I don't plan on getting huge powers , say 20mW , but
keeping an eye on the max current and collector voltage may be
a good idea :0)
The data sheet does not have parameters for the voltage and currents
that I'm
looking to use , but I'm hoping that they will at least get me in to
the ballpark.
I'm hoping the sims will be accurate enough to guide me from there.
This RF stuff is tough!!
I tried to embed the spice model into the CCT , that is why it fails :
0(
This is the CCT.

Version 4
SHEET 1 1300 1580
WIRE 48 144 -256 144
WIRE -256 192 -256 144
WIRE 48 192 48 144
WIRE -256 304 -256 272
WIRE -240 304 -256 304
WIRE -80 304 -96 304
WIRE -16 304 -80 304
WIRE -256 320 -256 304
WIRE -368 368 -496 368
WIRE -320 368 -368 368
WIRE -80 368 -80 304
WIRE -16 368 -16 304
WIRE -496 480 -496 448
WIRE -368 480 -368 448
WIRE -368 480 -496 480
WIRE -256 480 -256 416
WIRE -256 480 -368 480
WIRE -80 480 -80 432
WIRE -80 480 -256 480
WIRE -16 480 -16 448
WIRE -16 480 -80 480
WIRE 48 480 48 272
WIRE 48 480 -16 480
WIRE -368 496 -368 480
FLAG -368 496 0
SYMBOL voltage -496 352 R0
WINDOW 3 -14 181 Left 0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR Value SINE(0 1 433.92Meg)
SYMATTR InstName V1
SYMBOL ind -272 176 R0
SYMATTR InstName L1
SYMATTR Value 470n
SYMBOL res -384 352 R0
SYMATTR InstName R1
SYMATTR Value 1k
SYMBOL voltage 48 176 R0
SYMATTR InstName V2
SYMATTR Value 6
SYMBOL npn2 -320 320 R0
SYMATTR InstName Q1
SYMATTR Value BFR93A
SYMATTR Prefix X
SYMBOL cap -176 288 R90
WINDOW 0 0 32 VBottom 0
WINDOW 3 32 32 VTop 0
SYMATTR InstName C1
SYMATTR Value 100n
SYMBOL res -32 352 R0
SYMATTR InstName R2
SYMATTR Value 200
SYMBOL ind -80 288 R90
WINDOW 0 5 56 VBottom 0
WINDOW 3 32 56 VTop 0
SYMATTR InstName L2
SYMATTR Value 50n
SYMBOL cap -96 368 R0
SYMATTR InstName C2
SYMATTR Value 2p
TEXT -64 1288 Left 0 !.tran 50n


This is the MODEL file , actually sub-cct.

* Filename: BFR93A_SPICE.PRM
* BFR93A SPICE MODEL
* PHILIPS SEMICONDUCTORS
* Date : September 1995
*
* PACKAGE : SOT23 DIE MODEL : BFR91A
* 1: COLLECTOR; 2: BASE; 3: EMITTER;
.SUBCKT BFR93A 1 2 3
Q1 6 5 7 7 BFR91A
* SOT23 parasitic model
Lb 4 5 .4n
Le 7 8 .83n
L1 2 4 .35n
L2 1 6 .17n
L3 3 8 .35n
Ccb 4 6 71f
Cbe 4 8 2f
Cce 6 8 71f
*
* PHILIPS SEMICONDUCTORS
Version: 1.0
* Filename: BFR91A.PRM Date: Feb
1992
*
.MODEL BFR91A NPN
+ IS = 1.32873E-015
+ BF = 1.02000E+002
+ NF = 1.00025E+000
+ VAF = 5.19033E+001
+ IKF = 8.15511E+000
+ ISE = 1.39029E-014
+ NE = 1.51292E+000
+ BR = 1.76953E+001
+ NR = 9.94038E-001
+ VAR = 3.28032E+000
+ IKR = 1.00000E+001
+ ISC = 1.04297E-015
+ NC = 1.18993E+000
+ RB = 1.00000E+001
+ IRB = 1.00000E-006
+ RBM = 1.00000E+001
+ RE = 7.63636E-001
+ RC = 9.00000E+000
+ EG = 1.11000E+000
+ XTI = 3.00000E+000
+ CJE = 2.03216E-012
+ VJE = 6.00000E-001
+ MJE = 2.90076E-001
+ TF = 6.55790E-012
+ XTF = 3.89752E+001
+ VTF = 1.09308E+001
+ ITF = 5.21078E-001
+ CJC = 1.00353E-012
+ VJC = 3.40808E-001
+ MJC = 1.94223E-001
.ENDS
Sorry Rob, this one errors, says "Too few nodes, version 1.0". Whatever
that means.

--
Regards, Joerg

http://www.analogconsultants.com/

"gmail" domain blocked because of excessive spam.
Use another domain or send PM.

Hello Rob,

There was a missing "*" at the beginning of two comment lines.
Below is the corrected version.
You can add the model text as a SPICE-directive to your schematic or
save it in an extra file. In the ladder case you have to include the model
file.

Helmut Sennewald wrote:
"Joerg" <invalid_at_invalid.invalid> schrieb im Newsbeitrag
news:8dqrcfFcnhU1_at_mid.individual.net...
neddie wrote:
On Aug 26, 12:19 am, Joerg <inva...@invalid.invalid> wrote:
Tim Wescott wrote:
On 08/25/2010 06:12 AM, neddie wrote:
Hi to all.
I'm looking to make a small 433Mhz transmitter using bfr93's.
I want to have a oscillator , followed by a small class c amp , both
using bfr93.
Tho oscillator will be a standard Colpits oscillator , with a SAW
resonator.
I'd like to attach a class c amp (followed by filtering obviously) to
boost the power.
I've got a spice model for the BFR93 , from NXP.
What I want to know is will a simulation of this very non linear
application of the bfr93
provide any usefull results at all , or will I see total junk.
A LTSpice cct is attached , simulating a BFR93 as a class c amp.It's
not
a finished cct , so the component values are not final.I'd just like
to know if the results
that I get are realistic. If I built that cct , is that what I'd get.I
do realise that
I have not included any paracitics in the components yet.
Cheers
Rob
All I get when I try to read that file in LTSpice are tons-o-errors.
Yup. Rob, if you publish circuits that way make sure the models are in
it as well. It won't run on other people's PC unless they also have the
same model.

If the BRF93 is being marketed for service at UHF then the model should
work -- and there seem to be the right parasitic components in the
model
to imply this. SPICE is all about nonlinear circuit analysis, so as
long as either you're not driving the transistor into saturation, or as
long as the model is taking storage effects into account, then the
model
should be representative.
Whether you are correctly taking all of _your_ circuit parasitics into
account is your problem. I'm sure there are folks out there that can
model a circuit at that frequency and build it with confidence; I'm not
one of them.
You can drive it pretty hard but keep in mind that SPICE does not have a
*PHUT* function. On the computer you can make a virtual kilovolt-level
amp with a BFR93 which then in practice will explode violently.

But yeah, one can simulate RF stuff and it tends to come out alright on
the circuit board.

--
Regards, Joerg

http://www.analogconsultants.com/

"gmail" domain blocked because of excessive spam.
Use another domain or send PM.
Thanks for the help guys .Your answers have helped.
I don't plan on getting huge powers , say 20mW , but
keeping an eye on the max current and collector voltage may be
a good idea :0)
The data sheet does not have parameters for the voltage and currents
that I'm
looking to use , but I'm hoping that they will at least get me in to
the ballpark.
I'm hoping the sims will be accurate enough to guide me from there.
This RF stuff is tough!!
I tried to embed the spice model into the CCT , that is why it fails :
0(

Sorry Rob, this one errors, says "Too few nodes, version 1.0". Whatever
that means.

--
Regards, Joerg

http://www.analogconsultants.com/

"gmail" domain blocked because of excessive spam.
Use another domain or send PM.

Hello Rob,

There was a missing "*" at the beginning of two comment lines.
Below is the corrected version.
You can add the model text as a SPICE-directive to your schematic or
save it in an extra file. In the ladder case you have to include the model
file.


Yep. Thanks, Helmut, that made it run. Rob: The BFR93 isn't a very happy
camper for class C. Connect the source with a 1000pF, add a resistor in
the 7K range from base to 6V, and 10ohms or so in the emitter. Then you
can drive it with 100mV and get similar output but much cleaner. Just
watch for DC runaway if you build it. Of course now it ain't really
class C anymore.

On Fri, 27 Aug 2010 17:07:10 -0700, Joerg wrote:

Helmut Sennewald wrote:
"Joerg" <invalid_at_invalid.invalid> schrieb im Newsbeitrag
news:8dqrcfFcnhU1_at_mid.individual.net...
neddie wrote:
On Aug 26, 12:19 am, Joerg <inva...@invalid.invalid> wrote:
Tim Wescott wrote:
On 08/25/2010 06:12 AM, neddie wrote:
Hi to all.
I'm looking to make a small 433Mhz transmitter using bfr93's.
I want to have a oscillator , followed by a small class c amp , both
using bfr93.
Tho oscillator will be a standard Colpits oscillator , with a SAW
resonator.
I'd like to attach a class c amp (followed by filtering obviously) to
boost the power.
I've got a spice model for the BFR93 , from NXP.
What I want to know is will a simulation of this very non linear
application of the bfr93
provide any usefull results at all , or will I see total junk.
A LTSpice cct is attached , simulating a BFR93 as a class c amp.It's
not
a finished cct , so the component values are not final.I'd just like
to know if the results
that I get are realistic. If I built that cct , is that what I'd get.I
do realise that
I have not included any paracitics in the components yet.
Cheers
Rob
All I get when I try to read that file in LTSpice are tons-o-errors.
Yup. Rob, if you publish circuits that way make sure the models are in
it as well. It won't run on other people's PC unless they also have the
same model.

If the BRF93 is being marketed for service at UHF then the model should
work -- and there seem to be the right parasitic components in the
model
to imply this. SPICE is all about nonlinear circuit analysis, so as
long as either you're not driving the transistor into saturation, or as
long as the model is taking storage effects into account, then the
model
should be representative.
Whether you are correctly taking all of _your_ circuit parasitics into
account is your problem. I'm sure there are folks out there that can
model a circuit at that frequency and build it with confidence; I'm not
one of them.
You can drive it pretty hard but keep in mind that SPICE does not have a
*PHUT* function. On the computer you can make a virtual kilovolt-level
amp with a BFR93 which then in practice will explode violently.

But yeah, one can simulate RF stuff and it tends to come out alright on
the circuit board.

--
Regards, Joerg

http://www.analogconsultants.com/

"gmail" domain blocked because of excessive spam.
Use another domain or send PM.
Thanks for the help guys .Your answers have helped.
I don't plan on getting huge powers , say 20mW , but
keeping an eye on the max current and collector voltage may be
a good idea :0)
The data sheet does not have parameters for the voltage and currents
that I'm
looking to use , but I'm hoping that they will at least get me in to
the ballpark.
I'm hoping the sims will be accurate enough to guide me from there.
This RF stuff is tough!!
I tried to embed the spice model into the CCT , that is why it fails :
0(

Circuit snipped

Sorry Rob, this one errors, says "Too few nodes, version 1.0". Whatever
that means.

--
Regards, Joerg

http://www.analogconsultants.com/

"gmail" domain blocked because of excessive spam.
Use another domain or send PM.
Hello Rob,

There was a missing "*" at the beginning of two comment lines.
Below is the corrected version.
You can add the model text as a SPICE-directive to your schematic or
save it in an extra file. In the ladder case you have to include the model
file.

Yep. Thanks, Helmut, that made it run. Rob: The BFR93 isn't a very happy
camper for class C. Connect the source with a 1000pF, add a resistor in
the 7K range from base to 6V, and 10ohms or so in the emitter. Then you
can drive it with 100mV and get similar output but much cleaner. Just
watch for DC runaway if you build it. Of course now it ain't really
class C anymore.

I managed to salvage the originally posted circuit. A lot of playing got
it going class C, about 50mW output into Rob's 200 ohm load (why 200
ohm?). FFT shows second harmonic -20dB, higher orders decreasing like they
should. I had to rehash Rob's coupling network to step up 200 ohms to
about 700 at the collector. That resulted in some stupidly small
capacitance values, like 0.18pF, in order to get a decent Q of about 10.
It needs a couple of volts RMS from a 50 ohm source to drive it.
Dissipation in the BFR93A is around 25mW. As you say, not a happy camper
for Class C.

I'll maybe have a play with simulating transmission line coupling,
(microstrip?). That might appeal to your parsimonious nature <grin>.

So unless you I misunderstand you drive at 80mW to get 50mW out? I'd do
that with three resistors instead of a BFR93A ... <duck and run

I'll maybe have a play with simulating transmission line coupling,
(microstrip?). That might appeal to your parsimonious nature <grin>.


And I'd think about replacing the BFR93A since it is over 10c a pop. A
BFS17A can be had for 3c less. Ok, a bit less than half the ft but that
ought to do here. Maybe a grounded base architecture.

Sunday's exercise might be to compare the (Philips) model's S-parameters
against Philips' data sheet values. Wanna bet they don't match?

Shame LTSpice won't do polar plots. Since it does impedance and
S-params, it really ought to.

On Sat, 28 Aug 2010 14:34:24 -0700, Fred Abse wrote:

Sunday's exercise might be to compare the (Philips) model's S-parameters
against Philips' data sheet values. Wanna bet they don't match?

Pretty close match, apart from S22, which doesn't show the pronounced kink
shown in the datasheet.

Shame LTSpice won't do polar plots. Since it does impedance and
S-params, it really ought to.

Found a way round that. Set LTSpice to do ASCII rawfiles, run, edit two or
three LT-specific lines out of the rawfile, and load it into Berkeley
Spice 3f4's Nutmeg, then plot polar and Smith from there.
Much easier than trying to get LTSpice netlists to run in 3f4.

I still think the facility should be in LTSpice, though.