¿ªÔÆÌåÓý

  1. LTspice
  2. Messages
Expanded Topics Messages Polls
Date
Re: Analog MUX

 

--- In LTspice@..., "polapart <sahawley@m...>"
<sahawley@m...> wrote:
I was looking around for a model of a low voltage MUX like the
74lv4051. I found a a 6 pin fragment in the Philips LV library
() called SWI1. I wired
it
up and it ran fine with DC control input, but when I attempted to
toggle the switch with a square wave, once it turned off it never
turned on again.

Any ideas what's going on here and or pointers to a fully
functional
part model.
Hello,
unfortunately I don't know any other source of SPICE model for this
part. The behaviour looked indeed strange. It was ok with static
driven control input, but failed with a pulse source. I already
speculated about a problem of LTSpice.
The last resort was to sketch the circuit from the netlist through
all levels of subcircuits. That was a hard work and I wouldn't have
done it, if I hadn't feared a problem of the LTSpice simulator.
I found an inverter output connected to no other stage in the used
subcircuit LLCN. The subcircuit levels are SWI1 -> LLCN. This
circuit contains a first inverter, a two stage level shifter and two
more following inverters. The output of the first inverter was
connected to no other circuit. Obviously this is wrong. Either MP1 or
MP2 has to be connected to node '4'. I supposed MP2. The simulation
now runs with pulse sources as expected.

Conclusion: There is a bug in this Philips model. This is really a
pain and now I have low confidence about the quality of this library.

It is in zhree files: Lvnomi.cir, lvfast.cir, lvslow.cir .
I suppose to change the line in the .subckt LLCN ...

MP2 6 2 50 50 MLVPEN W=135U .......

to

MP2 6 4 50 50 MLVPEN W=135U .......

The interested reader can draw the schematic from the netlist.

Hope that helps and please next time an easier problem.


Best Regards
Helmut



Original subcircuit in file lvnomi.cir, lvfast.cir and lvslow.cir:
------------------------------------------------------------------
.SUBCKT LLCN 2 3 40 50 60
* LEVEL CONVERTER
* INA = 2, OUT = 3, VEE = 40, VCC = 50, GND = 60
MP4 4 2 50 50 MLVPEN W= 30U L= 2.4U AD=120P AS=120P PD= 40U PS=
30U
MN4 4 2 60 60 MLVNEN W= 15U L= 2.4U AD= 60P AS= 60P PD= 20U PS=
15U
MP1 5 2 50 50 MLVPEN W=135U L= 2.4U AD=500P AS=500P PD=100U
PS=135U
MP2 6 2 50 50 MLVPEN W=135U L= 2.4U AD=500P AS=500P PD=100U
PS=135U
MN1 5 6 40 40 MLVNEN W=6.4U L=18.8U AD= 25P AS= 25P PD= 20U
PS=6.4U
MN2 6 5 40 40 MLVNEN W=6.4U L=18.8U AD= 25P AS= 25P PD= 20U
PS=6.4U
MP3 7 6 50 50 MLVPEN W= 10U L= 4.0U AD= 40P AS= 40P PD= 20U PS=
10U
MN3 7 6 40 40 MLVNEN W= 5U L= 4.0U AD= 20P AS= 20P PD= 10U PS=
5U
MP5 3 7 50 50 MLVPEN W= 30U L= 2.4U AD=120P AS=120P PD= 40U PS=
30U
MN5 3 7 40 40 MLVNEN W= 15U L= 2.4U AD= 60P AS= 60P PD= 20U PS=
15U
.ENDS



Corrected subcircuit
--------------------
.SUBCKT LLCN 2 3 40 50 60
* LEVEL CONVERTER
* INA = 2, OUT = 3, VEE = 40, VCC = 50, GND = 60
MP4 4 2 50 50 MLVPEN W= 30U L= 2.4U AD=120P AS=120P PD= 40U PS=
30U
MN4 4 2 60 60 MLVNEN W= 15U L= 2.4U AD= 60P AS= 60P PD= 20U PS=
15U
MP1 5 2 50 50 MLVPEN W=135U L= 2.4U AD=500P AS=500P PD=100U
PS=135U
*** Changed node '2' to '4' in the next line ***
MP2 6 4 50 50 MLVPEN W=135U L= 2.4U AD=500P AS=500P PD=100U
PS=135U
MN1 5 6 40 40 MLVNEN W=6.4U L=18.8U AD= 25P AS= 25P PD= 20U
PS=6.4U
MN2 6 5 40 40 MLVNEN W=6.4U L=18.8U AD= 25P AS= 25P PD= 20U
PS=6.4U
MP3 7 6 50 50 MLVPEN W= 10U L= 4.0U AD= 40P AS= 40P PD= 20U PS=
10U
MN3 7 6 40 40 MLVNEN W= 5U L= 4.0U AD= 20P AS= 20P PD= 10U PS=
5U
MP5 3 7 50 50 MLVPEN W= 30U L= 2.4U AD=120P AS=120P PD= 40U PS=
30U
MN5 3 7 40 40 MLVNEN W= 15U L= 2.4U AD= 60P AS= 60P PD= 20U PS=
15U
.ENDS
Analog MUX

polapart <[email protected]>
 

I was looking around for a model of a low voltage MUX like the
74lv4051. I found a a 6 pin fragment in the Philips LV library
() called SWI1. I wired it
up and it ran fine with DC control input, but when I attempted to
toggle the switch with a square wave, once it turned off it never
turned on again.

Any ideas what's going on here and or pointers to a fully functional
part model.

Thanks
SH
Re: Hierarchical schematics

 

--- In LTspice@..., Panama Mike <panamatex@y...> wrote:
Many thanks for your help. I moved the Spice
directive ".lib opamp.sub" to the top level as
suggested, and the sim ran. It seems rather
awkward to have to remember to put all
hierarchical subcircuit calls at the top
level when constructing a hierarchical
schematic, but I guess there's no way around
it. (Is there?)
a few minutes ago I sent Mike Engelhardt this
question and asked him to answer into this
thread at the YAHOO-LTSpice group.
Oh, yes. That is awkward. I'll see if I can't
improve on this.
I put up a version today(2.00t) that enables nested
subcircuit definitions. Initial tests suggest the
parameter passing is properly scoped. Please report
any problems or crashes as soon as you detect them.
Hello Mike,
thank you very much for the work on solving the .lib problem
in lower level hierarchy. Version 2.00x now works with the
configuration from Ron, too. It is now no longer necessary to put the
.include or .lib statement to the top level.

Best Regards
Helmut


Let me sketch the three level hierarchy for the people interested:
------------------------------------------------------------------

Top: Level-1 schematic: ressitors, instance of level-2

Next Level-2: instance of level-3, resistors, opamp.asy
.include opamp.sub

Next Level-3: transistors, diodes, G-sources
A small correction for the CD4093 model

Peter Kapas
 

Please, change in the schematic CD4093.asc and symbol CD4093.asy
node name gnd to G. It is universal, you can shift the level of the "GND"
node.

Peter
Re: Digest Number 23

Peter Kapas
 

Hi Neil /New user: how to edit digital models?
-----------------------------------------------

Try these:

CD4093.asc
------------------------------------------------
Version 4
SHEET 1 892 692
WIRE 288 304 304 304
WIRE 160 320 112 320
WIRE 160 256 112 256
WIRE 160 272 128 272
WIRE 128 272 128 352
WIRE 128 352 160 352
WIRE 160 352 160 336
WIRE 160 352 240 352
WIRE 240 352 240 320
WIRE 160 352 160 368
FLAG 112 256 a
IOPIN 112 256 In
FLAG 112 320 b
IOPIN 112 320 In
FLAG 304 304 c
IOPIN 304 304 Out
FLAG 160 368 gnd
IOPIN 160 368 BiDir
SYMBOL C:&#92;Program&#92; Files&#92;LTC&#92;SwCADIII&#92;Digital&#92;and 256 224 R0
WINDOW 3 0 0 Invisible 0
SYMATTR Value Vlow=.1 Vhigh={VDD}
SYMATTR InstName A1
SYMATTR Value2 Trise=2n Tfall=2n
SYMBOL C:&#92;Program&#92; Files&#92;LTC&#92;SwCADIII&#92;Digital&#92;schmtbuf 160 192 R0
WINDOW 3 8 60 Invisible 0
SYMATTR Value Vt={Vtt} Vh={Vhh} Trise=10n Tfall=10n
SYMATTR InstName A2
SYMATTR Value2 Vlow=.1 Vhigh={VDD} Td=193n
SYMBOL C:&#92;Program&#92; Files&#92;LTC&#92;SwCADIII&#92;Digital&#92;schmtbuf 160 256 R0
WINDOW 3 17 89 Invisible 0
SYMATTR Value Vt={Vtt} Vh={Vhh} Trise=10n Tfall=10n
SYMATTR InstName A3
SYMATTR Value2 Vlow=.1 Vhigh={VDD} Td=193n
------------------------------------------------
CD4093.asy
------------------------------------------------
Version 4
SymbolType BLOCK
LINE Normal 16 -32 -32 -32
LINE Normal 17 32 -32 32
LINE Normal -32 32 -32 -32
LINE Normal 0 -16 16 -16
LINE Normal -8 16 0 -16
LINE Normal -16 16 -8 16
LINE Normal 0 16 -8 16
LINE Normal 8 -16 0 16
CIRCLE Normal 64 8 48 -8
ARC Normal -15 -32 48 32 17 32 16 -32
WINDOW 0 49 -42 Left 0
WINDOW 1 66 28 Left 0
PIN -32 -16 NONE 8
PINATTR PinName a
PINATTR SpiceOrder 1
PIN -32 16 NONE 8
PINATTR PinName b
PINATTR SpiceOrder 2
PIN 64 0 NONE 8
PINATTR PinName c
PINATTR SpiceOrder 3
PIN 0 32 NONE 8
PINATTR PinName gnd
PINATTR SpiceOrder 4
-------------------------------------------
and finally an example:
Relax.asc
-------------------------------------------
Version 4
SHEET 1 900 700
WIRE 80 -80 160 -80
WIRE 160 -80 160 48
WIRE 160 48 112 48
WIRE 16 32 -16 32
WIRE -80 32 -80 96
WIRE 16 64 -16 64
WIRE -16 64 -16 32
WIRE -16 32 -80 32
WIRE -16 32 -16 -80
WIRE -16 -80 0 -80
WIRE -80 192 -80 176
WIRE -80 176 48 176
WIRE -80 176 -80 160
WIRE 48 176 48 80
FLAG -80 192 0
SYMBOL C:&#92;Program&#92; Files&#92;LTC&#92;SwCADIII&#92;DC4093 48 48 R0
SYMATTR InstName U1
SYMATTR SpiceLine k=3 VDD=5*k Vtt=2.4*k Vhh=.532*k
SYMBOL cap -96 96 R0
SYMATTR InstName C1
SYMATTR Value 1n
SYMBOL res 96 -96 R90
WINDOW 0 0 56 VBottom 0
WINDOW 3 32 56 VTop 0
SYMATTR InstName R1
SYMATTR Value 20k
TEXT -100 216 Left 0 !.tran 1000u
-------------------------------------------

----- Original Message -----
From: <LTspice@...>
To: <LTspice@...>
Sent: Saturday, February 15, 2003 1:39 AM
Subject: [LTspice] Digest Number 23


To unsubscribe from this group, send an email to:
LTspice-unsubscribe@...


------------------------------------------------------------------------

There are 4 messages in this issue.

Topics in this digest:

1. Some basic uestions
From: Massimo Gaspari <gaspari@...>
2. Re: Some basic uestions
From: Panama Mike <panamatex@...>
3. New user: how to edit digital models?
From: "neel_christian <neel_c@...>"
<neel_c@...>
4. Re: New user: how to edit digital models?
From: "Helmut Sennewald <helmutsennewald@...>"
<helmutsennewald@...>


________________________________________________________________________
________________________________________________________________________

Message: 1
Date: Fri, 14 Feb 2003 21:41:24 +0100
From: Massimo Gaspari <gaspari@...>
Subject: Some basic uestions

Hi everybody,

I am a new user of LTSpice.

Looking into the model list I am not
able to find the models for a semiconducor (diffused) resistors and
capacitors.
They are not very important but some netlists are using them.
Are these models available in LTSpice? They are standard models in
Berkeley Spice3, may be useful to add them for compatibility.


Is there an upper limit for the numeber of components in the standard.*
libraries (diode,resistor,capacitor...)?

Using the .STEP statement it seems difficult to analyze the different
waveforms because it is not possible (is it right?) to understand which
value of the parameter is related with a particular waveform. Is there a
way to show which value is used with any waveforms?


Regards

Massimo


--

''~``
( o o )
+------------------.oooO--(_)--Oooo.------------------+
| |
| e-mail: gaspari@... |
| |
| ICQ # = 166939207 |
| |
| PGP fingerprint16: |
| 76 80 F2 F9 8D 70 F3 D1 42 2B CD 80 29 49 CB 25 |
| |
| .oooO |
| ( ) Oooo. |
+---------------------&#92; (----( )--------------------+
&#92;_) ) /
(_/




________________________________________________________________________
________________________________________________________________________

Message: 2
Date: Fri, 14 Feb 2003 13:10:50 -0800 (PST)
From: Panama Mike <panamatex@...>
Subject: Re: Some basic uestions

Looking into the model list I am not able to find
the
models for a semiconductor (diffused) resistors and
capacitors. They are not very important but some
netlists are using them. Are these models available
in LTSpice? They are standard models in Berkeley
Spice3, may be useful to add them for compatibility.
You can use the standard resistor and capacitors model
statements. It should be able to understand both
Berkeley and PSpice syntax.

Is there an upper limit for the number of components
in the standard.* libraries
(diode,resistor,capacitor...)?

Absolutely not, but there isn't any facility there you
help you organize your models. If you wish, you can
also keep your own libraries separate and include them
by putting a SPICE directive on the schematic of the
form ".lib <filenamepath>"

Using the .STEP statement it seems difficult to
analyze the different waveforms because it is not
possible (is it right?) to understand which value of
the parameter is related with a particular waveform.
Is there a way to show which value is used with any
waveforms?
Yes, it can be difficult. You can navigate an
attached
cursor from one dataset to the next with the up/down
keyboard cursor keys.

--Mike

__________________________________________________
Do you Yahoo!?
Yahoo! Shopping - Send Flowers for Valentine's Day



________________________________________________________________________
________________________________________________________________________

Message: 3
Date: Fri, 14 Feb 2003 23:25:22 -0000
From: "neel_christian <neel_c@...>"
<neel_c@...>
Subject: New user: how to edit digital models?

Hello Group,

I discovered LTSpice a few days ago and I find it very usefull, fun
and easy-to-use :-)

I am now trying to use mixed-mode simulation, and I cannot edit nor
see the models of simple parts like DFLOP (I just want to modify Hold
Time, Threshold, etc.). I did it easily for simple analog parts (like
nmos,pmos), but no way to find a file (even after a search in the
help files and FAQ) for digital parts...maybe I should buy new
glasses.

A Hint?

Thank you in advance for your help

Christian Nel




________________________________________________________________________
________________________________________________________________________

Message: 4
Date: Sat, 15 Feb 2003 00:00:07 -0000
From: "Helmut Sennewald <helmutsennewald@...>"
<helmutsennewald@...>
Subject: Re: New user: how to edit digital models?

--- In LTspice@..., "neel_christian <neel_c@c...>"
<neel_c@c...> wrote:
Hello Group,

I discovered LTSpice a few days ago and I find it very usefull,
fun
and easy-to-use :-)

I am now trying to use mixed-mode simulation, and I cannot edit nor
see the models of simple parts like DFLOP (I just want to modify
Hold
Time, Threshold, etc.). I did it easily for simple analog parts
(like
nmos,pmos), but no way to find a file (even after a search in the
help files and FAQ) for digital parts...maybe I should buy new
glasses.

A Hint?
Hello Christian,
new glasses wouldn't help. I had the same question half a year ago.
The developer of LTSpice, Mike Engelhardt, kindky send me the
necessary information.
By the way, he is around here in the group as Panama Mike,
but keep it for yourself. It is a secret.

The attached sample circuit helps to understand the syntax.
This file is also from Mike.

Hello Mike,
are there even more parameters for digital parts?

Best Regards
Helmut


Original answer from Mike:
--------------------------
The low and high levels are given with Vlow and Vhigh. The
logic thresholds default to half way between but can be
specified with ref. Hysteresis is not possible for gates,
but only for the Schmitt devices. Attached is and example
that hopefully illustrates. Tripdt is a type of temporal
accuracy it should strive for in switching.

Sample circuit file "gate.asc":
-------------------------------

Version 3
SHEET 1 892 692
WIRE 408 304 408 320
WIRE 420 292 436 292
WIRE 420 300 520 300
WIRE 344 356 344 340
WIRE 344 320 344 296
WIRE 344 296 404 296
WIRE 520 300 520 308
WIRE 520 328 520 340
WIRE 408 244 408 260
WIRE 420 232 436 232
WIRE 404 236 344 236
WIRE 344 236 344 296
WIRE 344 236 344 200
WIRE 344 200 404 200
WIRE 420 200 452 200
WIRE 404 204 404 212
FLAG 408 320 GND
FLAG 344 356 GND
FLAG 520 340 GND
FLAG 408 260 GND
FLAG 404 212 GND
SYMBOL digital&#92;and 412 280 R0
WINDOW 0 4 6 Left 0
WINDOW 3 4 28 Left 0
WINDOW 39 4 44 Left 0
WINDOW 40 4 52 Left 0
WINDOW 123 4 36 Left 0
SYMATTR InstName A1
SYMATTR Value Vhigh=5
SYMATTR Value2 Vlow=0 Rout=100
SYMATTR SpiceModel AND
SYMATTR SpiceLine Ref=2 Td=50n tripdt=3n
SYMATTR SpiceLine2 Trise=20n Tfall=40n
SYMBOL voltage 344 316 R0
WINDOW 0 6 4 Left 0
WINDOW 3 6 26 Left 0
SYMATTR InstName V1
SYMATTR Value pulse(0 5 0 100n 100n 0 200n)
SYMBOL res 516 304 R0
WINDOW 0 9 10 Left 0
WINDOW 3 9 19 Left 0
SYMATTR InstName R1
SYMATTR Value 1K
SYMBOL digital&#92;and 412 220 R0
WINDOW 0 4 6 Left 0
WINDOW 3 4 28 Left 0
WINDOW 39 4 44 Left 0
WINDOW 40 4 52 Left 0
WINDOW 123 4 36 Left 0
SYMATTR InstName A2
SYMATTR Value Vhigh=5
SYMATTR Value2 Vlow=0 Rout=100
SYMATTR SpiceModel AND
SYMATTR SpiceLine Ref=2 Td=50n tripdt=3n
SYMATTR SpiceLine2 Tau=10n
SYMBOL digital&#92;schmtbuf 404 184 R0
WINDOW 0 2 8 Left 0
WINDOW 3 5 24 Left 0
WINDOW 123 5 32 Left 0
SYMATTR InstName A3
SYMATTR Value Vt=2.5 Vh=1
SYMATTR Value2 tripdt=3n
SYMATTR SpiceModel SCHMITT
text 328 368 Left 0 !.tran 1u








________________________________________________________________________
________________________________________________________________________



Your use of Yahoo! Groups is subject to

Re: New user: how to edit digital models?

 

--- In LTspice@..., "neel_christian <neel_c@c...>"
<neel_c@c...> wrote:
--- In LTspice@..., "Helmut Sennewald >
The attached sample circuit helps to understand the syntax.
This file is also from Mike.

Hello Mike,
are there even more parameters for digital parts?

Best Regards
Helmut
Thank you very much Helmut,

In the meantime, I debugged my digital design (a simple FSM) on
another mixed-mode simulator (evaluation version of Microcap). Now
I'll try to implement it with LTSpice where my main analog design
is,
using Mikes's example.
Probably more feedback at the end of the week-end.
Hello Christian,
I forgot a very important detail.
You have to specify some delay Td for every flipflop.

All my simulated counters and flipflops have run as expected only
when I specified a delay for every flipflop(e.g. Td=10ns).

Your FSM(Finite State Machine) has flipflops and so you have to
add this value "Td=xx" to your flipflops. See also the Td parameter
in the last gate exmple.

Best Regards
Helmut
Re: New user: how to edit digital models?

 

--- In LTspice@..., "Helmut Sennewald >
The attached sample circuit helps to understand the syntax.
This file is also from Mike.

Hello Mike,
are there even more parameters for digital parts?

Best Regards
Helmut
Thank you very much Helmut,

In the meantime, I debugged my digital design (a simple FSM) on
another mixed-mode simulator (evaluation version of Microcap). Now
I'll try to implement it with LTSpice where my main analog design is,
using Mikes's example.
Probably more feedback at the end of the week-end.

Best regards

Christian
Re: New user: how to edit digital models?

 

--- In LTspice@..., "neel_christian <neel_c@c...>"
<neel_c@c...> wrote:
Hello Group,

I discovered LTSpice a few days ago and I find it very usefull,
fun
and easy-to-use :-)

I am now trying to use mixed-mode simulation, and I cannot edit nor
see the models of simple parts like DFLOP (I just want to modify
Hold
Time, Threshold, etc.). I did it easily for simple analog parts
(like
nmos,pmos), but no way to find a file (even after a search in the
help files and FAQ) for digital parts...maybe I should buy new
glasses.

A Hint?
Hello Christian,
new glasses wouldn't help. I had the same question half a year ago.
The developer of LTSpice, Mike Engelhardt, kindky send me the
necessary information.
By the way, he is around here in the group as Panama Mike,
but keep it for yourself. It is a secret.

The attached sample circuit helps to understand the syntax.
This file is also from Mike.

Hello Mike,
are there even more parameters for digital parts?

Best Regards
Helmut


Original answer from Mike:
--------------------------
The low and high levels are given with Vlow and Vhigh. The
logic thresholds default to half way between but can be
specified with ref. Hysteresis is not possible for gates,
but only for the Schmitt devices. Attached is and example
that hopefully illustrates. Tripdt is a type of temporal
accuracy it should strive for in switching.

Sample circuit file "gate.asc":
-------------------------------

Version 3
SHEET 1 892 692
WIRE 408 304 408 320
WIRE 420 292 436 292
WIRE 420 300 520 300
WIRE 344 356 344 340
WIRE 344 320 344 296
WIRE 344 296 404 296
WIRE 520 300 520 308
WIRE 520 328 520 340
WIRE 408 244 408 260
WIRE 420 232 436 232
WIRE 404 236 344 236
WIRE 344 236 344 296
WIRE 344 236 344 200
WIRE 344 200 404 200
WIRE 420 200 452 200
WIRE 404 204 404 212
FLAG 408 320 GND
FLAG 344 356 GND
FLAG 520 340 GND
FLAG 408 260 GND
FLAG 404 212 GND
SYMBOL digital&#92;and 412 280 R0
WINDOW 0 4 6 Left 0
WINDOW 3 4 28 Left 0
WINDOW 39 4 44 Left 0
WINDOW 40 4 52 Left 0
WINDOW 123 4 36 Left 0
SYMATTR InstName A1
SYMATTR Value Vhigh=5
SYMATTR Value2 Vlow=0 Rout=100
SYMATTR SpiceModel AND
SYMATTR SpiceLine Ref=2 Td=50n tripdt=3n
SYMATTR SpiceLine2 Trise=20n Tfall=40n
SYMBOL voltage 344 316 R0
WINDOW 0 6 4 Left 0
WINDOW 3 6 26 Left 0
SYMATTR InstName V1
SYMATTR Value pulse(0 5 0 100n 100n 0 200n)
SYMBOL res 516 304 R0
WINDOW 0 9 10 Left 0
WINDOW 3 9 19 Left 0
SYMATTR InstName R1
SYMATTR Value 1K
SYMBOL digital&#92;and 412 220 R0
WINDOW 0 4 6 Left 0
WINDOW 3 4 28 Left 0
WINDOW 39 4 44 Left 0
WINDOW 40 4 52 Left 0
WINDOW 123 4 36 Left 0
SYMATTR InstName A2
SYMATTR Value Vhigh=5
SYMATTR Value2 Vlow=0 Rout=100
SYMATTR SpiceModel AND
SYMATTR SpiceLine Ref=2 Td=50n tripdt=3n
SYMATTR SpiceLine2 Tau=10n
SYMBOL digital&#92;schmtbuf 404 184 R0
WINDOW 0 2 8 Left 0
WINDOW 3 5 24 Left 0
WINDOW 123 5 32 Left 0
SYMATTR InstName A3
SYMATTR Value Vt=2.5 Vh=1
SYMATTR Value2 tripdt=3n
SYMATTR SpiceModel SCHMITT
text 328 368 Left 0 !.tran 1u
New user: how to edit digital models?

 

Hello Group,

I discovered LTSpice a few days ago and I find it very usefull, fun
and easy-to-use :-)

I am now trying to use mixed-mode simulation, and I cannot edit nor
see the models of simple parts like DFLOP (I just want to modify Hold
Time, Threshold, etc.). I did it easily for simple analog parts (like
nmos,pmos), but no way to find a file (even after a search in the
help files and FAQ) for digital parts...maybe I should buy new
glasses.

A Hint?

Thank you in advance for your help

Christian N¨¦el
Re: Some basic uestions

 

Looking into the model list I am not able to find
the
models for a semiconductor (diffused) resistors and
capacitors. They are not very important but some
netlists are using them. Are these models available
in LTSpice? They are standard models in Berkeley
Spice3, may be useful to add them for compatibility.
You can use the standard resistor and capacitors model
statements. It should be able to understand both
Berkeley and PSpice syntax.

Is there an upper limit for the number of components
in the standard.* libraries
(diode,resistor,capacitor...)?

Absolutely not, but there isn't any facility there you
help you organize your models. If you wish, you can
also keep your own libraries separate and include them
by putting a SPICE directive on the schematic of the
form ".lib <filenamepath>"

Using the .STEP statement it seems difficult to
analyze the different waveforms because it is not
possible (is it right?) to understand which value of
the parameter is related with a particular waveform.
Is there a way to show which value is used with any
waveforms?
Yes, it can be difficult. You can navigate an
attached
cursor from one dataset to the next with the up/down
keyboard cursor keys.

--Mike

__________________________________________________
Do you Yahoo!?
Yahoo! Shopping - Send Flowers for Valentine's Day
Some basic uestions

 

Hi everybody,

I am a new user of LTSpice.

Looking into the model list I am not
able to find the models for a semiconducor (diffused) resistors and capacitors.
They are not very important but some netlists are using them.
Are these models available in LTSpice? They are standard models in Berkeley Spice3, may be useful to add them for compatibility.


Is there an upper limit for the numeber of components in the standard.*
libraries (diode,resistor,capacitor...)?

Using the .STEP statement it seems difficult to analyze the different waveforms because it is not possible (is it right?) to understand which
value of the parameter is related with a particular waveform. Is there a
way to show which value is used with any waveforms?


Regards

Massimo


--

''~``
( o o )
+------------------.oooO--(_)--Oooo.------------------+
| |
| e-mail: gaspari@... |
| |
| ICQ # = 166939207 |
| |
| PGP fingerprint16: |
| 76 80 F2 F9 8D 70 F3 D1 42 2B CD 80 29 49 CB 25 |
| |
| .oooO |
| ( ) Oooo. |
+---------------------&#92; (----( )--------------------+
&#92;_) ) /
(_/
Re: Need a model for a gas discharge tube (spark gap) and general help.

[email protected]
 

I need a model for a gas discharge tube similar to the Siemens A81-
C90X, if anyone can help I'd appreciate it. I have just started to
use LTSpice and would like to know if there is any information out
there that shows how to convert a manufactures model to something
that will keep LTSpice happy. I was hoping to use the DIAC that comes
with LTSpice but found out I have to supply my own model. Any hints
for a day-old user how to do this? So far it's a cool program.


To unsubscribe from this group, send an email to:
LTspice-unsubscribe@...



Your use of Yahoo! Groups is subject to
Try

Their may be something there you can use.

Regards

Brian

--
Brian Howie | Tel: 0131 343 5590
BAE SYSTEMS | Fax: 0131 343 5050
Sensor Systems Division | Email brian.howie@...
Silverknowes | bhowie@...
Edinburgh EH4 4AD | Web site www.baesystems.com
Re: Need a model for a gas discharge tube (spark gap) and general help.

 

--- In LTspice@..., "Helmut Sennewald
<helmutsennewald@y...>" <helmutsennewald@y...> wrote:
--- In LTspice@..., "bunnyblues2001
<bunnyblues2001@y...>" <bunnyblues2001@y...> wrote:
I need a model for a gas discharge tube similar to the Siemens A81-
C90X, if anyone can help I'd appreciate it. I have just started to
use LTSpice and would like to know if there is any information out
there that shows how to convert a manufactures model to something
that will keep LTSpice happy. I was hoping to use the DIAC that
comes
with LTSpice but found out I have to supply my own model. Any hints
for a day-old user how to do this? So far it's a cool program.

Hello,
are you referencing this model?

It contains lines with non LTSpice syntax.
These lines have to be modified.

Do you have a datasheet or any SPICE parameter?

Best Regards
Helmut

Thanks for the quick response. I have a few datasheets for different
devices. I don't now what parameters I'll need but not knowing has
never stopped me from giving it a shot.
Re: Need a model for a gas discharge tube (spark gap) and general help.

 

--- In LTspice@..., "bunnyblues2001
<bunnyblues2001@y...>" <bunnyblues2001@y...> wrote:
I need a model for a gas discharge tube similar to the Siemens A81-
C90X, if anyone can help I'd appreciate it. I have just started to
use LTSpice and would like to know if there is any information out
there that shows how to convert a manufactures model to something
that will keep LTSpice happy. I was hoping to use the DIAC that
comes
with LTSpice but found out I have to supply my own model. Any hints
for a day-old user how to do this? So far it's a cool program.

Hello,
are you referencing this model?

It contains lines with non LTSpice syntax.
These lines have to be modified.

Do you have a datasheet or any SPICE parameter?

Best Regards
Helmut
Need a model for a gas discharge tube (spark gap) and general help.

 

I need a model for a gas discharge tube similar to the Siemens A81-
C90X, if anyone can help I'd appreciate it. I have just started to
use LTSpice and would like to know if there is any information out
there that shows how to convert a manufactures model to something
that will keep LTSpice happy. I was hoping to use the DIAC that comes
with LTSpice but found out I have to supply my own model. Any hints
for a day-old user how to do this? So far it's a cool program.
Re: Hierarchical schematics

 

Many thanks for your help. I moved the Spice
directive ".lib opamp.sub" to the top level as
suggested, and the sim ran. It seems rather
awkward to have to remember to put all
hierarchical subcircuit calls at the top
level when constructing a hierarchical
schematic, but I guess there's no way around
it. (Is there?)
a few minutes ago I sent Mike Engelhardt this
question and asked him to answer into this
thread at the YAHOO-LTSpice group.
Oh, yes. That is awkward. I'll see if I can't
improve on this.
I put up a version today(2.00t) that enables nested
subcircuit definitions. Initial tests suggest the
parameter passing is properly scoped. Please report
any problems or crashes as soon as you detect them.

--Mike

__________________________________________________
Do you Yahoo!?
Yahoo! Shopping - Send Flowers for Valentine's Day
Re: Noise source in Transient analysis #NOISE

 

--- In LTspice@..., "gm4dij <brian.howie@b...>"
<brian.howie@b...> wrote:
--- In LTspice@..., Panama Mike <panamatex@y...> wrote:
You might be able to use the rand() function
to get what you're looking for. Check the
example ./LTC/SwCADIII/examples/Educational/PLL.asc
There it is used to generate a random bit stream
by boolean comparison to 0.5.

--Mike
--- "ingodettmann
<ingod@y...>"
<ingod@y...> wrote:
Hi everbody,

does anyone know, how I can add a noise source in a
transient
simulation (if it is possible at all)?
I tried to modell a noise source with a behavioral
voltage source
but i didn't work.
rand and white on their own are no use -these are rectangular
random
variables.

Use a behavioural voltage source with V for example

V=SQRT(-2*LN(white(time*1.07G)+0.5))*COS(2*PI*(white
((time*0.93G+0.5)))


This is the Box-Mueller algorithm for Gaussian Noise. You need two
independent random variables. The factors 1.07 and 0.93 is an
attempt
to do this. You will need to alter these, and the time step to get
what you want. You also may need to scale to get the correct rms
value in your noise bandwidth.

It's not perfect.
Hello Brian,
thanks for the formula. I googled and found this reference.


I couldn't resist to test it immediately in LTSPICE.
I have got some extremely high peaks(30V) at 47us, 48us and 84us
with the setting ".tran 0 100000n 0 0.5n".
So the formula needs a little change to avoid extreme values at
log(0).


The original formula:

V=SQRT(-2*LN(white(time*1.07G)+0.5))*COS(2*PI*(white(time*0.93G+0.5)))

My slightly modified formula for LTSpice:

V=SQRT(-2*LN(0.999997*white(time*1.07e9) +0.50001))*COS(2*PI*white
(time*0.93e9+0.5))

This B-source doesn't have the above mentioned "defects".

Best Regards
Helmut
Re: Noise source in Transient analysis #NOISE

gm4dij <[email protected]>
 

--- In LTspice@..., Panama Mike <panamatex@y...> wrote:
You might be able to use the rand() function
to get what you're looking for. Check the
example ./LTC/SwCADIII/examples/Educational/PLL.asc
There it is used to generate a random bit stream
by boolean comparison to 0.5.

--Mike
--- "ingodettmann
<ingod@y...>"
<ingod@y...> wrote:
Hi everbody,

does anyone know, how I can add a noise source in a
transient
simulation (if it is possible at all)?
I tried to modell a noise source with a behavioral
voltage source
but i didn't work.
rand and white on their own are no use -these are rectangular random
variables.

Use a behavioural voltage source with V for example

V=SQRT(-2*LN(white(time*1.07G)+0.5))*COS(2*PI*(white
((time*0.93G+0.5)))


This is the Box-Mueller algorithm for Gaussian Noise. You need two
independent random variables. The factors 1.07 and 0.93 is an attempt
to do this. You will need to alter these, and the time step to get
what you want. You also may need to scale to get the correct rms
value in your noise bandwidth.

It's not perfect.

Brian Howie


Do you Yahoo!?
Yahoo! Mail Plus - Powerful. Affordable. Sign up now.
Re: Hierarchical schematics

 

Many thanks for your help. I moved the Spice
directive ".lib opamp.sub" to the top level as
suggested, and the sim ran. It seems rather
awkward to have to remember to put all
hierarchical subcircuit calls at the top
level when constructing a hierarchical
schematic, but I guess there's no way around
it. (Is there?)
a few minutes ago I sent Mike Engelhardt this
question and asked him to answer into this
thread at the YAHOO-LTSpice group.
Oh, yes. That is awkward. I'll see if I can't
improve on this. The situation comes about
historically because while the academic codes
often do allow nested subcircuit definitions,
the commercial codes do not. However, the
commercial codes allow subcircuit parameters to
be passed, which is usually more useful.
Anyway, LTspice follows the commercial
standards. Maybe I can make it follow a
superset language.

--Mike

__________________________________________________
Do you Yahoo!?
Yahoo! Mail Plus - Powerful. Affordable. Sign up now.
Re: Hierarchical schematics

 


Helmut and Mike,

Many thanks for your help. I moved the Spice directive ".lib
opamp.sub" to the top level as suggested, and the sim ran. It
seems
rather awkward to have to remember to put all hierarchical
subcircuit calls at the top level when constructing a hierarchical
schematic, but I guess there's no way around it. (Is there?)

Hello Ron,
a few minutes ago I sent Mike Engelhardt this question and asked him
to answer into this thread at the YAHOO-LTSpice group.

Best Regards
Helmut
157641 - 157660 of 157701