Den fredag den 31. januar 2014 15.54.48 UTC+1 skrev Phil Hobbs:
> On 01/31/2014 03:47 AM, Lasse Langwadt Christensen wrote:
> 
> > Den fredag den 31. januar 2014 02.10.40 UTC+1 skrev Don Kuenz:
> 
> >> Lasse Langwadt Christensen <langwadt@fonz.dk> wrote:
> 
> >>
> 
> >>> Den torsdag den 30. januar 2014 20.44.39 UTC+1 skrev John Smith:
> 
> >>
> 
> >>
> 
> >>
> 
> >>>> Does annyone know whether any of the models on this page can ne used in
> 
> >>
> 
> >>>> LTSpice?
> 
> >>
> 
> >>>> http://www.onsemi.com/PowerSolutions/supportDoc.do?type=models&rpn=TIP31A
> 
> >>
> 
> >>
> 
> >>
> 
> >>> The easiest way (keeping everything in the same file), is to change
> 
> >>
> 
> >>> the name of the transistor to the models name Qtip31 and then add the
> 
> >>
> 
> >>> model as a spice directive on the schematic
> 
> >>
> 
> >>
> 
> >>
> 
> >> Interesting. Your method seems perfect for one-offs. Thank you for
> 
> >>
> 
> >> sharing. Another way is to add TIP31A as a component into LTSpice. This
> 
> >>
> 
> >> way the TIP31A always appears under
> 
> >>
> 
> >>    component
> 
> >>
> 
> >>      misc
> 
> >>
> 
> >>        TIP31A
> 
> >>
> 
> >>
> 
> >>
> 
> > snip
> 
> >
> 
> > the much simpler way is to add it to the file
> 
> >
> 
> > .....\LTC\LTspiceIV\lib\cmp\standard.bjt
> 
> >
> 
> >
> 
> > then it'll be in the list of transistor you can choose
> 
> >
> 
> >
> 
> > -Lasse
> 
> >
> 
> 
> 
> As long as you don't need to share the model with anybody.  For client 
> 
> work I generally cut'n'paste the model right into the .ASC file, and 
> 
> then hide the text.
> 

indeed, keeping every thing in a single file so it'll run anywhere makes 
life a lot easier when you have to share or run on multiple computers

would be nice with an option to embedded all the models in .asc file
automatically 

-Lasse

On 01/31/2014 03:47 AM, Lasse Langwadt Christensen wrote:
> Den fredag den 31. januar 2014 02.10.40 UTC+1 skrev Don Kuenz:
>> Lasse Langwadt Christensen <langwadt@fonz.dk> wrote:
>>
>>> Den torsdag den 30. januar 2014 20.44.39 UTC+1 skrev John Smith:
>>
>>
>>
>>>> Does annyone know whether any of the models on this page can ne used in
>>
>>>> LTSpice?
>>
>>>> http://www.onsemi.com/PowerSolutions/supportDoc.do?type=models&rpn=TIP31A
>>
>>
>>
>>> The easiest way (keeping everything in the same file), is to change
>>
>>> the name of the transistor to the models name Qtip31 and then add the
>>
>>> model as a spice directive on the schematic
>>
>>
>>
>> Interesting. Your method seems perfect for one-offs. Thank you for
>>
>> sharing. Another way is to add TIP31A as a component into LTSpice. This
>>
>> way the TIP31A always appears under
>>
>>    component
>>
>>      misc
>>
>>        TIP31A
>>
>>
>>
> snip
>
> the much simpler way is to add it to the file
>
> .....\LTC\LTspiceIV\lib\cmp\standard.bjt
>
>
> then it'll be in the list of transistor you can choose
>
>
> -Lasse
>

As long as you don't need to share the model with anybody.  For client 
work I generally cut'n'paste the model right into the .ASC file, and 
then hide the text.

Cheers

Phil Hobbs

-- 
Dr Philip C D Hobbs
Principal Consultant
ElectroOptical Innovations LLC
Optics, Electro-optics, Photonics, Analog Electronics

160 North State Road #203
Briarcliff Manor NY 10510

hobbs at electrooptical dot net
http://electrooptical.net

On 2014-01-29, Tim Wescott <tim@seemywebsite.really> wrote:
> On Wed, 29 Jan 2014 17:44:16 -0500, John Smith wrote:
>
>> "Lasse Langwadt Christensen" <langwadt@fonz.dk> wrote in message
>> news:0e3398dc-c4ba-4202-aa79-bf100371b4c7@googlegroups.com...
>>> Den onsdag den 29. januar 2014 22.27.39 UTC+1 skrev John Smith:
>>>> "Lasse Langwadt Christensen" <langwadt@fonz.dk> wrote in message
>>>>
>>>> news:b16e26e5-c5bd-4939-8836-d18278ed8ee2@googlegroups.com...
>>>>
>>>> Den onsdag den 29. januar 2014 20.53.09 UTC+1 skrev John Smith:
>>>>
>>>> > "Jan Panteltje" <pNaonStpealmtje@yahoo.com> wrote in message
>>>>
>>>>
>>>> >
>>>> > news:lcbgpa$am8$1@news.albasani.net...
>>>>
>>>>
>>>> >
>>>> > > On a sunny day (Wed, 29 Jan 2014 13:02:18 -0500) it happened "John
>>>>
>>>> > > Smith"
>>>>
>>>>
>>>> >
>>>> > > <invalid@invalid.invalid> wrote in <lcbfjq$i5p$1@dont-email.me>:
>>>>
>>>>
>>>> >
>>>>
>>>> > >
>>>>
>>>> >
>>>>
>>>> >
>>>>
>>>>
>>>> Thanks for going to that much effort Lasse but I've got started with
>>>> drawing
>>>>
>>>> the schematic myself in LT Spice and will compare it with yours when
>>>> I'm
>>>>
>>>> done figuring out which function key does what.
>>>>
>>>> How do I change a designator? i.e. change Q3 into Q4?
>>>>
>>>>
>>> right click on the designator
>> 
>> Aha, thanks, I was right clicking the component.
>> 
>> Is there no symbol for a variable resistor? Do I have to make it out of
>> two resistors?
>
> Or one, yes.  Your VR2 is really just one resistor that changes when you 
> turn a knob.  Usually in LTSpice (or any SPICE) such user input isn't 
> modeled -- it's up to you to enter the resistance that would be there.

Some do realtime interaction...  EWB, and the "circuit simulator" module in
GCompris would be two examples. I would not recommend the latter.

-- 
For a good time: install ntp

--- news://freenews.netfront.net/ - complaints: news@netfront.net ---

Den fredag den 31. januar 2014 02.10.40 UTC+1 skrev Don Kuenz:
> Lasse Langwadt Christensen <langwadt@fonz.dk> wrote:
> 
> > Den torsdag den 30. januar 2014 20.44.39 UTC+1 skrev John Smith:
> 
> 
> 
> >> Does annyone know whether any of the models on this page can ne used in
> 
> >> LTSpice?
> 
> >> http://www.onsemi.com/PowerSolutions/supportDoc.do?type=models&rpn=TIP31A
> 
> 
> 
> > The easiest way (keeping everything in the same file), is to change
> 
> > the name of the transistor to the models name Qtip31 and then add the
> 
> > model as a spice directive on the schematic
> 
> 
> 
> Interesting. Your method seems perfect for one-offs. Thank you for
> 
> sharing. Another way is to add TIP31A as a component into LTSpice. This
> 
> way the TIP31A always appears under
> 
>   component
> 
>     misc
> 
>       TIP31A
> 
> 
> 
snip

the much simpler way is to add it to the file

....\LTC\LTspiceIV\lib\cmp\standard.bjt


then it'll be in the list of transistor you can choose


-Lasse

>"I used that capacitor because I had it available, it's probaby between 30=
=20
and 40 years old. "

It might be better off as the main filter, though still overkill. The probl=
em is that it is going to take a while to charge and discharge, so you woul=
d want to have the input side also charge slowly. Then you are capable of d=
riving at subwoofer frequencies. If your source has a bass boost it'll eat =
all the power up in notime. I would let the low end response roll off at ma=
ybe 100 Hz. If you get a bigger speaker then modify it.=20

When I said jump out C2 the intent was to lower the DC voltage required at =
the base of Q1 so it wouldn't take forever to charge. Actually the way you =
have it is just fine and has the advantage of being less susceptable to cha=
nges in Vbe on Q1. More stable as the battery dies as well, I would say kee=
p it that way.=20

You almost don't really need R1 and C3, but they will help reduce the turno=
n transient. Let C3 charge slow. I don't feel like figuring the time consta=
nt right now, but you want it slower than C4 charges. (do lower that C4 val=
ue !) Other than that it is not critical.=20

On something like this, simplicity is wonderful. Remember what they used to=
 tell engineers - don't waste silicon. (eyeing D3 or D4 with an evil eye...=
)

Lasse Langwadt Christensen <langwadt@fonz.dk> wrote:
> Den torsdag den 30. januar 2014 20.44.39 UTC+1 skrev John Smith:

>> Does annyone know whether any of the models on this page can ne used in
>> LTSpice?
>> http://www.onsemi.com/PowerSolutions/supportDoc.do?type=models&rpn=TIP31A

> The easiest way (keeping everything in the same file), is to change
> the name of the transistor to the models name Qtip31 and then add the
> model as a spice directive on the schematic

Interesting. Your method seems perfect for one-offs. Thank you for
sharing. Another way is to add TIP31A as a component into LTSpice. This
way the TIP31A always appears under
  component
    misc
      TIP31A

The TIP31A.asc file shown below uses the TIP31A component.


------------------------------------------------------------------------
These lines go into C:\Program Files\LTC\LTspiceIV\lib\sub\TIP31A.sub
------------------------------------------------------------------------

*NPN silicon power transistor: TIP31A
SUBCKT TIP31A 1 2 3
**************  C B E
Q1 1 2 3 NMOD
MODEL NMOD NPN(IS=1e-09 BF=3656.16 NF=1.23899 VAF=10
+IKF=0.0333653 ISE=1e-08 NE=2.29374 BR=0.1
+NR=1.5 VAR=100 IKR=0.333653 ISC=1e-08
+NC=1.75728 RB=6.15083 IRB=100 RBM=0.00113049
+RE=0.0001 RC=0.0491489 XTB=50 XTI=1
+EG=1.05 CJE=3.26475e-10 VJE=0.446174 MJE=0.464221
+TF=2.06218e-09 XTF=15.0842 VTF=25.7317 ITF=0.001
+CJC=3.07593e-10 VJC=0.775484 MJC=0.476498 XCJC=0.750493
+FC=0.796407 CJS=0 VJS=0.75 MJS=0.5
+TR=9.57121e-06 PTF=0 KF=0 AF=1 )
ENDS TIP31A


------------------------------------------------------------------------
These lines go into C:\Program Files\LTC\LTspiceIV\lib\sym\Misc\TIP31A.asy
------------------------------------------------------------------------

Version 4
SymbolType CELL
LINE Normal 44 76 36 84
LINE Normal 64 96 44 76
LINE Normal 64 96 36 84
LINE Normal 40 80 16 64
LINE Normal 16 80 16 16
LINE Normal 16 32 64 0
LINE Normal 16 48 0 48
WINDOW 0 56 32 Left 0
WINDOW 3 56 68 Left 0
SYMATTR Value TIP31A
SYMATTR Prefix X
SYMATTR Description Bipolar NPN transistor
SYMATTR SpiceModel TIP31A
SYMATTR ModelFile TIP31A.sub
PIN 64 0 NONE 0
PINATTR PinName C
PINATTR SpiceOrder 1
PIN 0 48 NONE 0
PINATTR PinName B
PINATTR SpiceOrder 2
PIN 64 96 NONE 0
PINATTR PinName E
PINATTR SpiceOrder 3


------------------------------------------------------------------------
These lines go into TIP31A.asc
------------------------------------------------------------------------
Version 4
SHEET 1 880 680
WIRE 240 32 48 32
WIRE 400 32 240 32
WIRE 400 64 400 32
WIRE 48 80 48 32
WIRE 240 80 240 32
WIRE 400 160 400 144
WIRE 240 256 240 160
WIRE 320 256 240 256
WIRE 240 320 240 256
WIRE -80 368 -208 368
WIRE 48 368 48 160
WIRE 48 368 -16 368
WIRE 176 368 48 368
WIRE -208 400 -208 368
WIRE -208 528 -208 480
WIRE 240 528 240 416
FLAG 400 160 0
FLAG 240 528 0
FLAG -208 528 0
SYMBOL voltage 400 48 R0
WINDOW 123 0 0 Left 2
WINDOW 39 0 0 Left 2
SYMATTR InstName V1
SYMATTR Value 10V
SYMBOL res 224 64 R0
SYMATTR InstName R1
SYMATTR Value 1K
SYMBOL res 32 64 R0
SYMATTR InstName R2
SYMATTR Value 580K
SYMBOL cap -16 352 R90
WINDOW 0 0 32 VBottom 2
WINDOW 3 32 32 VTop 2
SYMATTR InstName C1
SYMATTR Value 1\xc2\xb5
SYMBOL cap 384 240 R90
WINDOW 0 0 32 VBottom 2
WINDOW 3 32 32 VTop 2
SYMATTR InstName C2
SYMATTR Value 1\xc2\xb5
SYMBOL Misc\\signal -208 384 R0
WINDOW 123 0 0 Left 2
WINDOW 39 0 0 Left 2
SYMATTR InstName V2
SYMATTR Value SINE(0 25mV 1K)
SYMBOL Misc\\TIP31A 176 320 R0
SYMATTR InstName Q1
TEXT -232 104 Left 2 !.tran 10ms


--
      __
   __/  \
  /  \__/
  \__/    Don Kuenz
  /  \__
  \__/  \
     \__/

><jurb6006@gmail.com> wrote in message 
>news:6dd0fb77-9e22-45e2-bd59->e0a86be273a4@googlegroups.com...
>I haven't put my two cents in yet but here it is :
>
>First of all, C4 should be nowhere near 4700 uF. You are not driving a 12" 
>woofer with it. Look
>at those good old stereo console pieces of junk, they got by with as low as 
>like 220 uF. Since
>it isn't in the feedback loop anyway, forget about phase shift, it means 
>nothing.

Thanks for your comments.
I used that capacitor because I had it available, it's probaby between 30 
and 40 years old.

>
>Next, you are not submitting this thing for evaluation by the IHF (are the 
>even still around ?)
>or Hifi magazine (same question) so you can totally eliminate Q2 and just 
>send the feedback (DC
>and AC) straight to the emitter of Q1. I would suggeast lower values for 
>the voltage divider to
>yield a lower impedance, off the top of my head use 4.7K for R7 and 470 for 
>R5. Eliminate C2 of
>course or the thing won't work.

Before I saw your post I experimented with removing Q2 as follows:
www.pdelectronics.ca/sed/amp2014jan28/amp2014jan28_5.zip
Quick View:
www.pdelectronics.ca/sed/amp2014jan28/amp2014jan28_5.jpg

I adjusted the component values for what seemed to be reasonable DC 
operating conditions with correct center voltage and same voltage gain. The 
bode plot looks reasonable over the audio range, unity gain frequency is now 
about 1MHz.

I haven't looked in the time domain yet to see if there are any other 
issues.

I was going to ask if there was any good reason to keep Q2.

Old Guy

>
>That will set your feedback at about 1/10th of the center voltage at R10 
>and 11. With your
>voltage divider there, make the voltage at the base of Q1 about that, just 
>add schoch for the
>drain of Q1. It really doesn't have to be all that accurate. Accuracy comes 
>later.
>
>Increase R1 and C3 to charge slowly and reduce the turnon transient. 
>Whatever the voltage
>divider feeding the base of Q1, figure the bottom resistor against the 
>input coupling cap to
>give the desired lower frequency limit, there is no reason to be concerned 
>about anything below
>100 Hz unless your speakers are going to reproduce it. If they are, that 
>can be done later.
>(you might want heftier transistors and a realer battery at that point) 
><tech jargon there...

>Now that the thing is designed like a bean counter would, then you and the 
>kid can go through
>the refinements. Draw out the scematic and show him the diff pair, 
>different values for some
>caps, in fact make it so shitty at first that some minor improvements can 
>make an audible
>difference. Maybe even jump out R13 in the beginning to demonstrate 
>crossover distortion.

>That's what I would do. You know even what was called hifi a long time ago 
>didn't use
>differential pairs at the input usually. It worked well enough. But realize 
>the other thing I
>am saying is maybe make it so there is room for improvement. (of course I 
>was known as the mad
>modifier back in the day, nothing was stock)

>Slide the pennies under the door if I am asleep.

Den torsdag den 30. januar 2014 20.44.39 UTC+1 skrev John Smith:
> "Kevin McMurtrie" <mcmurtrie@pixelmemory.us> wrote in message=20
>=20
> news:mcmurtrie-934B9C.22562129012014@c-61-68-245-199.per.connect.net.au..=
.
>=20
> > In article <lcbfjq$i5p$1@dont-email.me>,
>=20
> > "John Smith" <invalid@invalid.invalid> wrote:
>=20
> >
>=20
> >> The radio kit hasn't arrived yet (Thread of 18th Jan. Probably due to
>=20
> >> weather conditions here in Ontario) so I thought I'd try my hand at=20
>=20
> >> making
>=20
> >> my own audio amplifier kit.
>=20
> >>
>=20
> >> The requirements were as follows:
>=20
> >> 1. Must use components I already have. I couldn't find any 1N4148 but =
did
>=20
> >> find packets of 1N4001 so that's what I used. Also I could only find o=
ne
>=20
> >> resistor under 1 ohm so another is made from two in parallel.
>=20
> >> 2. Must be simple enough to fit on one piece of breadboard but not be =
a
>=20
> >> trivial design.
>=20
> >> 3. Must deliver enough power to make an 8 ohm speaker cone move visibl=
y.
>=20
> >> 4. Must run from a single 9V battery.
>=20
> >> 5. Must be quick to design with minimal calculation.
>=20
> >> 6. Any soldering must be done in advance of taking it into a school an=
d
>=20
> >> getting a little guy to build it.
>=20
> >> 7. Doesn't need high voltage gain as it will be driven from an ipod so=
 I
>=20
> >> designed for a gain of about 10.
>=20
> >> 8. Low distortion is not essential as long as there's no obvious issue=
=20
>=20
> >> below
>=20
> >> clipping level.
>=20
> >>
>=20
> >> With those requirements in mind I got a piece of paper out and drew th=
is:
>=20
> >> www.pdelectronics.ca/sed/amp2014jan28/schematic.jpg
>=20
> >> Then I did the layout:
>=20
> >> www.pdelectronics.ca/sed/amp2014jan28/layout.jpg
>=20
> >> Then I built and tested it:
>=20
> >> www.pdelectronics.ca/sed/amp2014jan28/built.jpg
>=20
> >> Actually there was much overlap between those three things.
>=20
> >>
>=20
> >> I set VR2 to zero resistance and measured an idle current of 60mA, so =
I
>=20
> >> didn't adjust VR2.
>=20
> >> I then connected a signal source from a computer, adjusted VR1 and the
>=20
> >> requirements seemed to have been met.
>=20
> >>
>=20
> >> I'm aware that there are people here who can comment on my amplifier=
=20
>=20
> >> design
>=20
> >> skills, or lack of them, and maybe some component values can be tweake=
d=20
>=20
> >> for
>=20
> >> better performance.
>=20
> >>
>=20
> >> Are there any free tools available which can run a simulation of this
>=20
> >> circuit?
>=20
> >> What is the lower and upper 3dB bandwidth?
>=20
> >> Is my wild guess at a value for C6 reasonable?
>=20
> >>
>=20
> >> Old Guy
>=20
> >
>=20
> > Your power filter of R8 and C3 is definitely not right.  The voltage
>=20
> > difference between the two circuit halves is going to modulate TR4 via
>=20
> > R3.  It will thump during power-on and probably motor-boat when the
>=20
> > battery is low.  The only thing that needs filtering is the voltage
>=20
> > divider on your input.  Everything else is running in constant current
>=20
> > mode and is fine with unregulated voltage.
>=20
> >
>=20
> > I don't know what current is flowing through TR3, but it should be
>=20
> > adjusted so that C6 charges and discharges symmetrically.  Sometimes yo=
u
>=20
> > can put a long wire on the input and adjust the current until you stop
>=20
> > hearing AM radio stations :)
>=20
> >
>=20
> > Unless it's there to be educational, replace whole constant current
>=20
> > regulator around TR3 with a simple resistor.  You only have +/- 0.4V of
>=20
> > input swing to reach full modulation.  The current through a resistor
>=20
> > should be close enough.
>=20
>=20
>=20
> Many thanks for your comments. I moved the power filter to the input volt=
age=20
>=20
> divider. 330uF is probably overkill. I've also given the battery a 2 ohm=
=20
>=20
> internal resistance.
>=20
>=20
>=20
> TR3 was mostly intended to be educational but for the present circuit I h=
ave=20
>=20
> replaced TR3 with a 4.7k resistor. The LTspice model says that the curren=
t=20
>=20
> in the resistor is 0.82 mA.
>=20
>=20
>=20
> Can I use the LTspice model to find out whether C6 is charging and=20
>=20
> discharging symetrically?
>=20

if you hover over the component you get the amp meter


>=20
>=20
> The current circuit is here:
>=20
> http://www.pdelectronics.ca/sed/amp2014jan28/amp2014jan28_4.zip
>=20
> Quick view here:
>=20
> http://www.pdelectronics.ca/sed/amp2014jan28/amp2014jan28_4.jpg
>=20
>=20
>=20
> I've also added an equivalent circuit for a loudspeaker which came from=
=20
>=20
> here:
>=20
> http://sound.westhost.com/tsp.htm
>=20
> I've no idea how close that is to my real loudspeaker but it may be close=
r=20
>=20
> than an 8 ohm resistor.
>=20
>=20
>=20
> A bode plot of V(input)/V(output) from 5Hz to 3MHz shows the expected 20d=
B=20
>=20
> voltage gain.
>=20
> The gain and phase are fairly flat over the audio range but the unity gai=
n=20
>=20
> frequency appears to be about 2.3 MHz. Is there any advantage in reducing=
=20
>=20
> that for an audio amplifier? Apart from reducing the potential for=20
>=20
> amplification of AM radio signals?
>=20
>=20
>=20
> Does annyone know whether any of the models on this page can ne used in=
=20
>=20
> LTSpice?
>=20
> http://www.onsemi.com/PowerSolutions/supportDoc.do?type=3Dmodels&rpn=3DTI=
P31A
>=20
>=20
>=20
> Old Guy

The easiest way (keeping everything in the same file), is to change the nam=
e of the transistor to the models name Qtip31 and then add the model as a s=
pice directive on the schematic

Version 4
SHEET 1 1728 680
WIRE 560 -64 256 -64
WIRE 256 0 256 -64
WIRE 256 112 256 80
WIRE 560 112 560 -64
WIRE 496 160 256 160
WIRE 256 208 256 160
WIRE 560 224 560 208
WIRE 256 336 256 288
WIRE 560 336 560 304
FLAG 256 112 0
FLAG 256 336 0
FLAG 560 336 0
SYMBOL voltage 256 -16 R0
WINDOW 123 0 0 Left 2
WINDOW 39 0 0 Left 2
SYMATTR InstName V1
SYMATTR Value 12
SYMBOL npn3 496 112 R0
SYMATTR InstName Q1
SYMATTR Value Qtip31
SYMBOL voltage 256 192 R0
WINDOW 123 0 0 Left 2
WINDOW 39 0 0 Left 2
WINDOW 3 -485 52 Left 2
SYMATTR InstName V2
SYMATTR Value PULSE(0 1.7 1m 500m 500m 10m 20m 1)
SYMBOL res 544 208 R0
SYMATTR InstName R1
SYMATTR Value 1
TEXT 64 312 Left 2 !.tran 1
TEXT 904 -120 Left 2 !.MODEL Qtip31 npn\n+IS=3D1e-09 BF=3D3656.16 NF=3D1.23=
899 VAF=3D10\n+IKF=3D0.0333653 ISE=3D1e-08 NE=3D2.29374 BR=3D0.1\n+NR=3D1.5=
 VAR=3D100 IKR=3D0.333653 ISC=3D1e-08\n+NC=3D1.75728 RB=3D6.15083 IRB=3D100=
 RBM=3D0.00113049\n+RE=3D0.0001 RC=3D0.0491489 XTB=3D50 XTI=3D1\n+EG=3D1.05=
 CJE=3D3.26475e-10 VJE=3D0.446174 MJE=3D0.464221\n+TF=3D2.06218e-09 XTF=3D1=
5.0842 VTF=3D25.7317 ITF=3D0.001\n+CJC=3D3.07593e-10 VJC=3D0.775484 MJC=3D0=
.476498 XCJC=3D0.750493\n+FC=3D0.796407 CJS=3D0 VJS=3D0.75 MJS=3D0.5\n+TR=
=3D9.57121e-06 PTF=3D0 KF=3D0 AF=3D1


-Lasse
=20