SWCADIII 555 model unrealistic?

T

Terry Pinnell

Guest
I'm trying out LT/SWCADIII. Is its NE555 model intended to be
realistic please? Both my breadboard test and my interpretation of the
data sheet seem to indicate that it's not. A simple astable with
supply voltage of 5.0V in practice gives pk-pk output of 3.7V, and
data sheet appears to predict 3.5V, yet SWCADIII simulates 5.0V. See
summary at
http://www.terrypin.dial.pipex.com/Images/555AstableSWCAD-3.gif

--
Terry Pinnell
Hobbyist, West Sussex, UK
 
Terry,
The 3.5V is specd at a load of 100 ma. What happens when you load it down
with a 35 Ohm resistor to ground? I don't think Linear makes 555s. So, you
don't know what model they are using.

Tam
"Terry Pinnell" <terrypin@dial.pipex.com> wrote in message
news:00n560pe2i9euk8muvqqiajbanrqjcvscs@4ax.com...
I'm trying out LT/SWCADIII. Is its NE555 model intended to be
realistic please? Both my breadboard test and my interpretation of the
data sheet seem to indicate that it's not. A simple astable with
supply voltage of 5.0V in practice gives pk-pk output of 3.7V, and
data sheet appears to predict 3.5V, yet SWCADIII simulates 5.0V. See
summary at
http://www.terrypin.dial.pipex.com/Images/555AstableSWCAD-3.gif

--
Terry Pinnell
Hobbyist, West Sussex, UK
Click to expand...
 
Terry,

I'm trying out LT/SWCADIII. Is its NE555 model intended to
be realistic please?
Click to expand...
There are two different 555's in LTspice/SwCADIII. The model
with the symbol is an idealized model. It doesn't represent
any particular 555 implementation. It just gives you idealized
behavior in the simulation and then it's up to you to find
a product that performs well enough to do the job.

The other 555 is a transistor implementation in the file
../examples/Educational/NE555.asc. That one works rather like
a bipolar 555. You can see all the little glitches while it
runs.

--Mike
 
On Thu, 25 Mar 2004 13:23:19 +0000, the renowned Terry Pinnell
<terrypin@dial.pipex.com> wrote:

I'm trying out LT/SWCADIII. Is its NE555 model intended to be
realistic please? Both my breadboard test and my interpretation of the
data sheet seem to indicate that it's not. A simple astable with
supply voltage of 5.0V in practice gives pk-pk output of 3.7V, and
data sheet appears to predict 3.5V, yet SWCADIII simulates 5.0V. See
summary at
Click to expand...
You shouldn't be using the curve for low drop since it's not
sinking any current. Also, 3.5V into 1K is about 3.5mA, not
10mA, so the curves predict an output voltage of about 3.65V p-p,
which is in close agreement with your measurement.

http://www.terrypin.dial.pipex.com/Images/555AstableSWCAD-3.gif
Click to expand...
Looks like it's a a simplified model.

Best regards,
Spehro Pefhany
--
"it's the network..." "The Journey is the reward"
speff@interlog.com Info for manufacturers: http://www.trexon.com
Embedded software/hardware/analog Info for designers: http://www.speff.com
 
"Tam/WB2TT" <t-tammaru@c0mca$t.net> wrote:

Terry,
The 3.5V is specd at a load of 100 ma.
Click to expand...
100 mA? I've used the 5 mA line, i.e. 5V across a 1k load. (My little
red circle on one graph was incorrectly positioned on the 10 mA line,
I see, but that doesn't affect the drop which is 1.4 V.)

What happens when you load it down
with a 35 Ohm resistor to ground?
Click to expand...
See above. Strictly the load should be 700 ohm, but 1k is close enough
in this context.

I don't think Linear makes 555s.
Click to expand...
Don't think that's relevant! What ECAD/Spice package supplier also
manufactures all the parts in their program's parts library?

So, you don't know what model they are using.
Click to expand...
True, but with the label 'NE555', I thought it was the NE555.
(Originally the biploar chip from Signetics, now Philips I think.)
Mike has advised it's actually an idealised model.


--
Terry Pinnell
Hobbyist, West Sussex, UK


Tam
"Terry Pinnell" <terrypin@dial.pipex.com> wrote in message
news:00n560pe2i9euk8muvqqiajbanrqjcvscs@4ax.com...
I'm trying out LT/SWCADIII. Is its NE555 model intended to be
realistic please? Both my breadboard test and my interpretation of the
data sheet seem to indicate that it's not. A simple astable with
supply voltage of 5.0V in practice gives pk-pk output of 3.7V, and
data sheet appears to predict 3.5V, yet SWCADIII simulates 5.0V. See
summary at
http://www.terrypin.dial.pipex.com/Images/555AstableSWCAD-3.gif

--
Terry Pinnell
Hobbyist, West Sussex, UK
Click to expand...
 
"Mike Engelhardt" <pmte@concentric.net> wrote:

Terry,

I'm trying out LT/SWCADIII. Is its NE555 model intended to
be realistic please?

There are two different 555's in LTspice/SwCADIII. The model
with the symbol is an idealized model. It doesn't represent
any particular 555 implementation. It just gives you idealized
behavior in the simulation and then it's up to you to find
a product that performs well enough to do the job.

The other 555 is a transistor implementation in the file
./examples/Educational/NE555.asc. That one works rather like
a bipolar 555. You can see all the little glitches while it
runs.

Thanks, Mike, I'll try that alternative.
Click to expand...

--
Terry Pinnell
Hobbyist, West Sussex, UK

>
 
Hi Terry,

Actually we are very lucky. LT used to provide this spice only
for use with their switching regulator chips. It was a very kindly
act of generosity that allows you to use it as a full featured spice
emulator... for free, no less.

LT was nice enough to provide models for all of their parts, and most
passives. Isn't it a little too much to ask of them that they give
you models for all of their competitor's parts too?

They are not your usual cad tool provider.

-Chuck Harris

Terry Pinnell wrote:

I don't think Linear makes 555s.


Don't think that's relevant! What ECAD/Spice package supplier also
manufactures all the parts in their program's parts library?
Click to expand...
 
"Terry Pinnell" <terrypin@dial.pipex.com> wrote in message
news:6m36609po4s5vltrk1tt77ous42a1ua956@4ax.com...
"Tam/WB2TT" <t-tammaru@c0mca$t.net> wrote:

Terry,
The 3.5V is specd at a load of 100 ma.

100 mA? I've used the 5 mA line, i.e. 5V across a 1k load. (My little
red circle on one graph was incorrectly positioned on the 10 mA line,
I see, but that doesn't affect the drop which is 1.4 V.)

I looked at 2 different data sheets, and see Vh at 100 ma. This is probably
Click to expand...
moot, because they seem to give you a functional, rather than a transistor
level model. The output consists of a double emitter follower. So, with any
load at all the output should be down 2 Vbe drops from Vcc

What happens when you load it down
with a 35 Ohm resistor to ground?

See above. Strictly the load should be 700 ohm, but 1k is close enough
in this context.

I don't think Linear makes 555s.

Don't think that's relevant! What ECAD/Spice package supplier also
manufactures all the parts in their program's parts library?

I don't know where you got your copy of the program from, but I downloaded
Click to expand...
mine from the LT web site. They are paying for it. The models for their
parts work.

So, you don't know what model they are using.

True, but with the label 'NE555', I thought it was the NE555.
(Originally the biploar chip from Signetics, now Philips I think.)
Mike has advised it's actually an idealised model.


--
Terry Pinnell
Hobbyist, West Sussex, UK


Tam
"Terry Pinnell" <terrypin@dial.pipex.com> wrote in message
news:00n560pe2i9euk8muvqqiajbanrqjcvscs@4ax.com...
I'm trying out LT/SWCADIII. Is its NE555 model intended to be
realistic please? Both my breadboard test and my interpretation of the
data sheet seem to indicate that it's not. A simple astable with
supply voltage of 5.0V in practice gives pk-pk output of 3.7V, and
data sheet appears to predict 3.5V, yet SWCADIII simulates 5.0V. See
summary at
http://www.terrypin.dial.pipex.com/Images/555AstableSWCAD-3.gif

--
Terry Pinnell
Hobbyist, West Sussex, UK
Click to expand...
 
On 25 Mar 2004 11:03:57 EST, "Mike Engelhardt" <pmte@concentric.net>
wrote:

Terry,

I'm trying out LT/SWCADIII. Is its NE555 model intended to
be realistic please?

There are two different 555's in LTspice/SwCADIII. The model
with the symbol is an idealized model. It doesn't represent
any particular 555 implementation. It just gives you idealized
behavior in the simulation and then it's up to you to find
a product that performs well enough to do the job.

The other 555 is a transistor implementation in the file
./examples/Educational/NE555.asc. That one works rather like
a bipolar 555. You can see all the little glitches while it
runs.

--Mike


Hello Mike,
Click to expand...
I would like to ask a few off topic questions, if I may. I am
a learner with SWCADIII. I am wearing my "L" plates. :)
My version is recently updated 2.09E and Free.
Thanks for that. Greatly appreciated.

Netlists that I have seen posted on the group say Version 4.
I can still see the circuits, after I click the little problem dialog
box that pops up and click to ignore the problems.

So, am I missing anything important by clicking "ignore"?
Is version 4 free also, or what? Where do I get it?

Here in Sydney the only place I found to buy the LT
switcher ICs was RS Components. That mob are too
expensive and they did not have many LT components,
only about half a dozen.
I asked LT who the Australian agents for parts were
but LT didn't reply to my e-mail. So here, we have you,
the designer offering help to people which is great,
a free program which is also great, but no assortment
of LT switcher parts to play with in this part of the world.
What rotten luck, eh!

Regards,
John Crighton
Sydney
 
John,

Netlists that I have seen posted on the group say
Version 4. I can still see the circuits, after
I click the little problem dialog box that pops
up and click to ignore the problems.

So, am I missing anything important by clicking
"ignore"? Is version 4 free also, or what?
Where do I get it?
Click to expand...
Usually those errors are due to either line wrap
from the Usenet News Service or sometimes a missing
symbol. BTW, the text that starts with "Version 4"
and needs to be saved in .asc files are just called
schematics, not netlists. LTspice uses an ASCII
format for schematics so that they can be e-mailed
about, posted, viewed, etc. as open files. That
"Version 4" refers to the file version, not the
program version. The up-to-date, unlimited version
of LTspice is indeed freely availible from the web.
BTW, there's an an independent users' group at
http://groups.yahoo.com/group/LTspice that you might
like to follow.

Here in Sydney the only place I found to buy the LT
switcher ICs was RS Components. That mob are too
expensive and they did not have many LT components,
only about half a dozen.
I asked LT who the Australian agents for parts were
but LT didn't reply to my e-mail. So here, we have
you, the designer offering help to people which is
great, a free program which is also great, but no
assortment of LT switcher parts to play with in this
part of the world. What rotten luck, eh!
Click to expand...
Send some e-mail to Linear's web site asking about a
local rep/distributor for you. You can buy direct from
Linear's web, too, I think. It must be possible to buy
everything Linear sells in Australia. The Pacific rim
is a non-trivial fraction of Linear's business.

--Mike
 
On Thu, 25 Mar 2004 22:52:57 GMT, john_c@tpg.com.au (John Crighton) wrote:

(snip)

Here in Sydney the only place I found to buy the LT
switcher ICs was RS Components. That mob are too
expensive and they did not have many LT components,
only about half a dozen.
I asked LT who the Australian agents for parts were
but LT didn't reply to my e-mail.
Click to expand...
Arrow Australia (regrettably)
 
In article <40635853.10688006@News.individual.net>,
John Crighton <john_c@tpg.com.au> wrote:
[...]
expensive and they did not have many LT components,
only about half a dozen.
I asked LT who the Australian agents for parts were
but LT didn't reply to my e-mail. So here, we have you,
the designer offering help to people which is great,
a free program which is also great, but no assortment
of LT switcher parts to play with in this part of the world.
What rotten luck, eh!
Click to expand...
Move to the US and buy the LT parts from Digikey.

--
--
kensmith@rahul.net forging knowledge
 
On Fri, 26 Mar 2004 03:55:32 +0000 (UTC), kensmith@violet.rahul.net (Ken Smith)
wrote:

In article <40635853.10688006@News.individual.net>,
John Crighton <john_c@tpg.com.au> wrote:
[...]
expensive and they did not have many LT components,
only about half a dozen.
I asked LT who the Australian agents for parts were
but LT didn't reply to my e-mail. So here, we have you,
the designer offering help to people which is great,
a free program which is also great, but no assortment
of LT switcher parts to play with in this part of the world.
What rotten luck, eh!

Move to the US and buy the LT parts from Digikey.
Click to expand...
If he wants more than a handful, that'll be the cheaper option :-(
 
Chuck Harris wrote:
Hi Terry,

Actually we are very lucky. LT used to provide this spice only
for use with their switching regulator chips. It was a very kindly
act of generosity that allows you to use it as a full featured spice
emulator... for free, no less.
Click to expand...
Complete Nonsense. It was not an act of kindness or generosity in any
way whatsoever. It was a sound, well thought out business decision. As
Mike has already pointed out, it has probably led to millions of dollars
of increased sales for LT components.

No one dose nought for nought in this universe. Companies simply don't
do things to be nice. http://www.anasoft.co.uk/replicators/index.html

Kevin Aylward
salesEXTRACT@anasoft.co.uk
http://www.anasoft.co.uk
SuperSpice, a very affordable Mixed-Mode
Windows Simulator with Schematic Capture,
Waveform Display, FFT's and Filter Design.

"quotes with no meaning, are meaningless" - Kevin Aylward.
 
"Mike Engelhardt" <pmte@concentric.net> wrote:

Terry,

I'm trying out LT/SWCADIII. Is its NE555 model intended to
be realistic please?

There are two different 555's in LTspice/SwCADIII. The model
with the symbol is an idealized model. It doesn't represent
any particular 555 implementation. It just gives you idealized
behavior in the simulation and then it's up to you to find
a product that performs well enough to do the job.

The other 555 is a transistor implementation in the file
./examples/Educational/NE555.asc. That one works rather like
a bipolar 555. You can see all the little glitches while it
runs.
Click to expand...
OK, that certainly looks complex enough to be realistic! But how do I
set about using it in practice please, just as if it was another 555
model?

In CircuitMaker I'm familiar with making a new model by choosing an
appropriate symbol (such as an 8-pin DIP IC rectangle), adding
internal circuitry (such as your detailed 555 model), and saving as a
new part. Is there an equivalent approach in SWCADIII please?

--
Terry Pinnell
Hobbyist, West Sussex, UK
 
I read in sci.electronics.design that Kevin Aylward <kevindotaylwardEXTR
ACT@anasoft.co.uk> wrote (in <ASQ8c.18$t22.16@newsfep3-gui.server.ntli.n
et>) about 'SWCADIII 555 model unrealistic?', on Fri, 26 Mar 2004:

No one dose nought for nought in this universe.
Click to expand...
Maybe not for ever, but SuperSpice was free for a long while during
initial development.
--
Regards, John Woodgate, OOO - Own Opinions Only.
The good news is that nothing is compulsory.
The bad news is that everything is prohibited.
http://www.jmwa.demon.co.uk Also see http://www.isce.org.uk
 
Spehro Pefhany <speffSNIP@interlogDOTyou.knowwhat> wrote:

On Thu, 25 Mar 2004 13:23:19 +0000, the renowned Terry Pinnell
terrypin@dial.pipex.com> wrote:

I'm trying out LT/SWCADIII. Is its NE555 model intended to be
realistic please? Both my breadboard test and my interpretation of the
data sheet seem to indicate that it's not. A simple astable with
supply voltage of 5.0V in practice gives pk-pk output of 3.7V, and
data sheet appears to predict 3.5V, yet SWCADIII simulates 5.0V. See
summary at

You shouldn't be using the curve for low drop since it's not
sinking any current. Also, 3.5V into 1K is about 3.5mA, not
10mA, so the curves predict an output voltage of about 3.65V p-p,
which is in close agreement with your measurement.
Click to expand...
That was my point: data sheet prediction plus my measurement
contradict SWCADIII simulation. Mike has now answered with a No; it's
not meant to be realistic. (See also my earlier post re minor error re
5mS v 10 mA line; immaterial in context though.)

http://www.terrypin.dial.pipex.com/Images/555AstableSWCAD-3.gif

Looks like it's a simplified model.
Click to expand...
Indeed, as per Mike's reply.

Mike: I suggest a name change. 'NE555' is misleading. (That's the
Signetics, now Philips chip. How about something like '555' or
'555Ideal'?

Best regards,
Spehro Pefhany
Click to expand...
 
Kevin Aylward wrote:
Chuck Harris wrote:

Hi Terry,

Actually we are very lucky. LT used to provide this spice only
for use with their switching regulator chips. It was a very kindly
act of generosity that allows you to use it as a full featured spice
emulator... for free, no less.


Complete Nonsense. It was not an act of kindness or generosity in any
way whatsoever. It was a sound, well thought out business decision. As
Mike has already pointed out, it has probably led to millions of dollars
of increased sales for LT components.

No one dose nought for nought in this universe. Companies simply don't
do things to be nice. http://www.anasoft.co.uk/replicators/index.html
Click to expand...
Perhaps, but they could have done like Actel, Xilinx, Altera, Microchip,
.... and charged large bucks for the tools that were necessary to use
their chips.

Or, they could do like you, and charge big bucks for a half-fast
simulator.

-Chuck Harris
 
"Chuck Harris" <cfharris@erols.com> wrote in message
news:40643356$0$3053$61fed72c@news.rcn.com...
Kevin Aylward wrote:
Chuck Harris wrote:

Hi Terry,

Actually we are very lucky. LT used to provide this spice only
for use with their switching regulator chips. It was a very kindly
act of generosity that allows you to use it as a full featured spice
emulator... for free, no less.


Complete Nonsense. It was not an act of kindness or generosity in any
way whatsoever. It was a sound, well thought out business decision. As
Mike has already pointed out, it has probably led to millions of dollars
of increased sales for LT components.

No one dose nought for nought in this universe. Companies simply don't
do things to be nice. http://www.anasoft.co.uk/replicators/index.html

Perhaps, but they could have done like Actel, Xilinx, Altera, Microchip,
... and charged large bucks for the tools that were necessary to use
their chips.
Click to expand...
Interesting you mentioned Xilinx. 5 or 6 years ago I was able to buy their
Foundation series software + a serial port programmer for $99 on a special.
Last I looked, the price was back to $1000 +.

Tam
Or, they could do like you, and charge big bucks for a half-fast
simulator.

-Chuck Harris
Click to expand...
 
On Fri, 26 Mar 2004 12:58:37 +0000, the renowned Terry Pinnell
<terrypin@dial.pipex.com> wrote:

That was my point: data sheet prediction plus my measurement
contradict SWCADIII simulation. Mike has now answered with a No; it's
not meant to be realistic. (See also my earlier post re minor error re
5mS v 10 mA line; immaterial in context though.)
Click to expand...
Terry, I'm sure you know how to do this, but for the possible benefit
of others, I've attached part of your image showing a graphical way to
do it with a 1K load. The "typical" high output voltage is the
intersection of the slanted line from 5mA/0V to 3mA/2V with the output
voltage drop curves. The slant comes from Ohm's law, with a 2V drop
there will be 3mA through the 1K load, with a 0V drop 5mA (give a 5V
supply). Of course, it can be done iteratively, too- look at the drop
with a 5mA load, re-calculate the current, look at the drop again, and
it quickly converges to the same answer.

BTW, it just so happens that the 555 outputs about zero volts with a
load resistor to ground, but that can't be depended on, sometimes the
output voltage of a circuit stops at some non-zero voltage (continues
to source current) when it is saturated. One has to look at the
schematic (if provided) or the datasheet (if specified) or test a
sample (if you can't get a sample it's best to move on..) .

Best regards,
Spehro Pefhany
--
"it's the network..." "The Journey is the reward"
speff@interlog.com Info for manufacturers: http://www.trexon.com
Embedded software/hardware/analog Info for designers: http://www.speff.com
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top