FAQFAQ   SearchSearch   MemberlistMemberlist   UsergroupsUsergroups 
 ProfileProfile   PreferencesPreferences   Log in to check your private messagesLog in to check your private messages   Log inLog in 
Forum index » Electronix » cad
What S/W will simulate a transmission line type pulse transformer?
Post new topic   Reply to topic Page 1 of 1 [14 Posts] View previous topic :: View next topic
Author Message
jpsmith123@yahoo.com
electronics forum beginner


Joined: 26 Dec 2005
Posts: 3

PostPosted: Sun Jun 18, 2006 3:57 am    Post subject: What S/W will simulate a transmission line type pulse transformer? Reply with quote

I tried simulating a transmission line transformer (one end connected
in parallel, the other end in series) using "CircuitMaker 2000" and
"MultiSim 8", but apparently the models these programs use (even the
lossy line model) are not appropriate for this type of simulation.

I'm wondering, does anyone know of software that will realistically
simulate such transmission line based circuits in the time domain?
Thank you.
Back to top
John Popelish
electronics forum Guru


Joined: 29 Apr 2005
Posts: 1601

PostPosted: Sun Jun 18, 2006 4:15 am    Post subject: Re: What S/W will simulate a transmission line type pulse transformer? Reply with quote

jpsmith123@yahoo.com wrote:
Quote:
I tried simulating a transmission line transformer (one end connected
in parallel, the other end in series) using "CircuitMaker 2000" and
"MultiSim 8", but apparently the models these programs use (even the
lossy line model) are not appropriate for this type of simulation.

I'm wondering, does anyone know of software that will realistically
simulate such transmission line based circuits in the time domain?
Thank you.

I have been working up a spice model of a transmission line

transformer that approximates it with 16 inductances and 17
capacitances. It was meant to model a transformer wound through two
flat cable cores, so that the winding pair runs straight down the
slots, with the ends as far as possible from each other. It includes
the 120 mutual inductance coupling factors that model the reduction of
coupling efficiency as turns get further apart and both the normal
transmission line capacitance per length and the capacitance between 1
turn and the next of the pair. The responses have not been tested
against actual measurements, but they look quite reasonable, as long
as the phase shift per inductance segment is a small part of a cycle.

I selected the inductance and capacitance values to fit test data on a
particular example, but you can change them.

I built it for LTspice, free download at:
http://www.linear.com/company/software.jsp

If you would like to have a copy of this component model and its
symbol file, email me.
Back to top
John Larkin
electronics forum Guru


Joined: 29 Apr 2005
Posts: 4320

PostPosted: Sun Jun 18, 2006 4:43 am    Post subject: Re: What S/W will simulate a transmission line type pulse transformer? Reply with quote

On Sun, 18 Jun 2006 00:15:46 -0400, John Popelish <jpopelish@rica.net>
wrote:

Quote:
jpsmith123@yahoo.com wrote:
I tried simulating a transmission line transformer (one end connected
in parallel, the other end in series) using "CircuitMaker 2000" and
"MultiSim 8", but apparently the models these programs use (even the
lossy line model) are not appropriate for this type of simulation.

I'm wondering, does anyone know of software that will realistically
simulate such transmission line based circuits in the time domain?
Thank you.

I have been working up a spice model of a transmission line
transformer that approximates it with 16 inductances and 17
capacitances. It was meant to model a transformer wound through two
flat cable cores, so that the winding pair runs straight down the
slots, with the ends as far as possible from each other. It includes
the 120 mutual inductance coupling factors that model the reduction of
coupling efficiency as turns get further apart and both the normal
transmission line capacitance per length and the capacitance between 1
turn and the next of the pair. The responses have not been tested
against actual measurements, but they look quite reasonable, as long
as the phase shift per inductance segment is a small part of a cycle.

I selected the inductance and capacitance values to fit test data on a
particular example, but you can change them.

I built it for LTspice, free download at:
http://www.linear.com/company/software.jsp

If you would like to have a copy of this component model and its
symbol file, email me.

A long string of L's and C's makes a good transmission line model, but
the number of sections explodes as a power of the delay/risetime
ratio. I've done lines with hundreds of sections.

Most Spice transmission line models contain a hidden isolation
transformer (you can apply DC between the 'shields' of opposite ends)
and aren't very realistic for things like transmission-line
transformers.

John
Back to top
Mike Engelhardt
electronics forum addict


Joined: 14 May 2005
Posts: 61

PostPosted: Sun Jun 18, 2006 7:05 pm    Post subject: Re: What S/W will simulate a transmission line type pulse transformer? Reply with quote

John,

Quote:
Most Spice transmission line models contain a hidden
isolation transformer (you can apply DC between the
'shields' of opposite ends) and aren't very realistic
for things like transmission-line transformers.

In SPICE-speak, the transmission line device of SPICE
handles a single node. A length of coax has two nodes,
normal mode and common mode. To invert, you need to
model both modes. The classic example is in Larry
Nagel's PhD thesis(Berkeley 1975), but here's a
deck that will show how to do a transmission line
inverter in LTspice on the netlist level:

* transmission line inverter
T2 0 0 OUT 0 Td=50n Z0=75 ; center conductor
T1 IN 0 0 OUT Td=70n Z0=50 ; shield higher Z but faster
V1 IN 0 PULSE(0 1 0 1n 1n 10n) Rser=50
..tran 0 500n 0 1n
..end

The general case is that a cable has as many modes
as conductors including the shield. That the SPICE
transmission line device supplies only a single node
is an odd concept to be sure -- a cable with but a
single wire but controlled impedance. Just the same,
it's supper useful if you ground each end of one of
the sides. Then you can simulate the normal mode and
skip the common mode if it doesn't interest you.

--Mike
Back to top
John Larkin
electronics forum Guru


Joined: 29 Apr 2005
Posts: 4320

PostPosted: Sun Jun 18, 2006 10:59 pm    Post subject: Re: What S/W will simulate a transmission line type pulse transformer? Reply with quote

On Sun, 18 Jun 2006 19:05:32 GMT, "Mike Engelhardt" <nospam@spam.org>
wrote:

Quote:
John,

Most Spice transmission line models contain a hidden
isolation transformer (you can apply DC between the
'shields' of opposite ends) and aren't very realistic
for things like transmission-line transformers.

In SPICE-speak, the transmission line device of SPICE
handles a single node. A length of coax has two nodes,
normal mode and common mode. To invert, you need to
model both modes.


This is a super-wideband inverter, in both Spice and real life:

(----------------)
in+ ----( coax )----(---------------)
in- ----(----------------)----( coax )------ out+
(---------------)------ out-

The Spice version is perfect. The real version has problems if IN- and
OUT- are both grounded (the whole thing becomes a short) and that
limits low-frequency response. Slipping a ferrite over it somewhere
helps the lf end a lot. The center crossover should be zero-length.
Done with a couple of hunks of hardline, it's very impressive.

John
Back to top
Mike Engelhardt
electronics forum addict


Joined: 14 May 2005
Posts: 61

PostPosted: Sun Jun 18, 2006 11:38 pm    Post subject: Re: What S/W will simulate a transmission line type pulse transformer? Reply with quote

John,

Quote:
Most Spice transmission line models contain a hidden
isolation transformer (you can apply DC between the
'shields' of opposite ends) and aren't very realistic
for things like transmission-line transformers.

In SPICE-speak, the transmission line device of SPICE
handles a single node. A length of coax has two nodes,
normal mode and common mode. To invert, you need to
model both modes. To invert, you need to model both
modes. The classic example is in Larry Nagel's PhD
thesis(Berkeley 1975), but here's a deck that will
show how to do a transmission line inverter in LTspice
on the netlist level:

* transmission line inverter
T2 0 0 OUT 0 Td=50n Z0=75 ; center conductor
T1 IN 0 0 OUT Td=70n Z0=50 ; shield higher Z but faster
V1 IN 0 PULSE(0 1 0 1n 1n 10n) Rser=50
.tran 0 500n 0 1n
.end

The general case is that a cable has as many modes
as conductors including the shield. That the SPICE
transmission line device supplies only a single node
is an odd concept to be sure -- a cable with but a
single wire but controlled impedance. Just the same,
it's supper useful if you ground each end of one of
the sides. Then you can simulate the normal mode and
skip the common mode if it doesn't interest you.

This is a super-wideband inverter, in both Spice and real
life:

(----------------)
in+ ----( coax )----(---------------)
in- ----(----------------)----( coax )------ out+
(---------------)------ out-

The Spice version is perfect. The real version has problems
if IN- and OUT- are both grounded (the whole thing becomes a
short) and that limits low-frequency response. Slipping a
ferrite over it somewhere helps the lf end a lot. The center
crossover should be zero-length. Done with a couple of hunks
of hardline, it's very impressive.

Interesting example. Thanks.

But it doesn't work very in SPICE if you dutifully model both
modes of each cable. Your circuit above requires four SPICE
transmission line elements. Yes, if you ignore two
propagation modes, it's perfect in SPICE but that is an
error in the application of SPICE. Below is an LTspice
schematic that illustrates perfect behavior from incorrect
analysis and the results from using 4 ideal propagation modes.

Regards,

--Mike

--- xmissionbs.asc ---

Version 4
SHEET 1 880 680
WIRE -240 208 -240 -96
WIRE -240 272 -240 208
WIRE -240 400 -240 352
WIRE -160 -96 -240 -96
WIRE -160 208 -240 208
WIRE 16 -16 -80 -16
WIRE 16 -16 16 -64
WIRE 16 16 16 -16
WIRE 16 96 16 48
WIRE 48 272 -48 272
WIRE 48 272 48 240
WIRE 48 288 48 272
WIRE 64 -96 -80 -96
WIRE 64 -64 16 -64
WIRE 64 16 16 16
WIRE 64 48 16 48
WIRE 96 208 -80 208
WIRE 96 240 48 240
WIRE 208 -64 160 -64
WIRE 208 -16 208 -64
WIRE 208 16 160 16
WIRE 208 16 208 -16
WIRE 208 48 160 48
WIRE 208 96 208 48
WIRE 240 -96 160 -96
WIRE 240 -16 208 -16
WIRE 240 240 192 240
WIRE 240 288 240 240
WIRE 256 208 192 208
WIRE 256 240 240 240
WIRE 288 208 256 240
WIRE 288 240 256 208
WIRE 304 -96 240 -16
WIRE 304 -16 240 -96
WIRE 336 -16 304 -16
WIRE 336 -16 336 -64
WIRE 336 16 336 -16
WIRE 336 96 336 48
WIRE 352 208 288 208
WIRE 352 240 288 240
WIRE 384 -96 304 -96
WIRE 384 -64 336 -64
WIRE 384 16 336 16
WIRE 384 48 336 48
WIRE 496 240 448 240
WIRE 496 288 496 240
WIRE 528 -64 480 -64
WIRE 528 -16 528 -64
WIRE 528 16 480 16
WIRE 528 16 528 -16
WIRE 528 48 480 48
WIRE 528 96 528 48
WIRE 560 208 448 208
WIRE 576 288 496 288
WIRE 608 -96 480 -96
WIRE 768 -16 528 -16
FLAG 48 288 0
FLAG 240 288 0
FLAG -240 400 0
FLAG -48 272 0
FLAG 560 208 0
FLAG 16 96 0
FLAG 208 96 0
FLAG -80 -16 0
FLAG 336 96 0
FLAG 528 96 0
FLAG 608 -96 0
SYMBOL tline 144 224 R0
WINDOW 3 -76 43 Left 0
SYMATTR Value Td=70n Z0=50
SYMATTR InstName T1
SYMBOL voltage -240 256 R0
WINDOW 123 0 0 Left 0
WINDOW 39 24 132 Left 0
SYMATTR InstName V1
SYMATTR Value PULSE(0 1 0 1n 1n 10n)
SYMBOL tline 400 224 R0
WINDOW 3 -76 43 Left 0
SYMATTR Value Td=70n Z0=50
SYMATTR InstName T3
SYMBOL tline 112 -80 R0
WINDOW 3 -76 43 Left 0
SYMATTR Value Td=70n Z0=50
SYMATTR InstName T2
SYMBOL tline 112 32 R0
WINDOW 3 -76 43 Left 0
SYMATTR Value Td=50n Z0=75
SYMATTR InstName T4
SYMBOL tline 432 -80 R0
WINDOW 3 -76 43 Left 0
SYMATTR Value Td=70n Z0=50
SYMATTR InstName T5
SYMBOL tline 432 32 R0
WINDOW 3 -76 43 Left 0
SYMATTR Value Td=50n Z0=75
SYMATTR InstName T6
SYMBOL res -64 192 R90
WINDOW 0 0 56 VBottom 0
WINDOW 3 32 56 VTop 0
SYMATTR InstName R1
SYMATTR Value 50
SYMBOL res -64 -112 R90
WINDOW 0 0 56 VBottom 0
WINDOW 3 32 56 VTop 0
SYMATTR InstName R2
SYMATTR Value 50
TEXT 288 352 Left 0 !.tran 0 500n 0 1n
TEXT -16 208 Bottom 0 ;IN+
TEXT -16 272 Bottom 0 ;IN-
TEXT 528 208 Bottom 0 ;OUT-
TEXT 536 288 Bottom 0 ;OUT+
TEXT -48 -96 Bottom 0 ;IN+
TEXT -48 -16 Bottom 0 ;IN-
TEXT 560 -96 Bottom 0 ;OUT-
TEXT 568 -16 Bottom 0 ;OUT+
TEXT 272 -104 Bottom 0 ;"Correct"
TEXT 272 176 Bottom 0 ;"Incorrect"
Back to top
Jeroen Belleman
electronics forum beginner


Joined: 19 May 2005
Posts: 38

PostPosted: Mon Jun 19, 2006 12:56 pm    Post subject: Re: What S/W will simulate a transmission line type pulse transformer? Reply with quote

Mike Engelhardt wrote:
Quote:
John Larkin wrote:

This is a super-wideband inverter, in both Spice and real
life:

(----------------)
in+ ----( coax )----(---------------)
in- ----(----------------)----( coax )------ out+
(---------------)------ out-


Interesting example. Thanks.

But it doesn't work very in SPICE if you dutifully model both
modes of each cable. Your circuit above requires four SPICE
transmission line elements. Yes, if you ignore two
propagation modes, it's perfect in SPICE but that is an
error in the application of SPICE. [...]

The actual arrangement sure works a whole lot better than your
"correct" SPICE model!

I obtained a fair match to reality by modelling a transmission
line transformer as a tline with both screen terminals connected
together, followed by a pair of coupled coils wired as a balun.
The tline acounts for delay effects and the balun for imperfect
coupling and common mode currents. For an example, see:
http://jeroen.web.cern.ch/jeroen/reports/wbhybrid.pdf

Regards,
Jeroen Belleman
Back to top
John Larkin
electronics forum Guru


Joined: 29 Apr 2005
Posts: 4320

PostPosted: Mon Jun 19, 2006 5:01 pm    Post subject: Re: What S/W will simulate a transmission line type pulse transformer? Reply with quote

On Sun, 18 Jun 2006 23:38:06 GMT, "Mike Engelhardt" <nospam@spam.org>
wrote:


Quote:
This is a super-wideband inverter, in both Spice and real
life:

(----------------)
in+ ----( coax )----(---------------)
in- ----(----------------)----( coax )------ out+
(---------------)------ out-

The Spice version is perfect. The real version has problems
if IN- and OUT- are both grounded (the whole thing becomes a
short) and that limits low-frequency response. Slipping a
ferrite over it somewhere helps the lf end a lot. The center
crossover should be zero-length. Done with a couple of hunks
of hardline, it's very impressive.

Interesting example. Thanks.

But it doesn't work very in SPICE if you dutifully model both
modes of each cable. Your circuit above requires four SPICE
transmission line elements. Yes, if you ignore two
propagation modes, it's perfect in SPICE but that is an
error in the application of SPICE. Below is an LTspice
schematic that illustrates perfect behavior from incorrect
analysis and the results from using 4 ideal propagation modes.

Regards,

--Mike


I'll post some scope pics to a.b.s.e. Interestingly, "outside mode"
impedance doesn't seem to matter. In fact, squeezing the coax close to
the crossover improves the waveforms a bit.

When Spice conflicts with reality, where's the error?

John
Back to top
Jim Thompson
electronics forum Guru


Joined: 06 May 2005
Posts: 5440

PostPosted: Mon Jun 19, 2006 5:34 pm    Post subject: Re: What S/W will simulate a transmission line type pulse transformer? Reply with quote

On Mon, 19 Jun 2006 10:01:04 -0700, John Larkin
<jjlarkin@highNOTlandTHIStechnologyPART.com> wrote:

[snip]
Quote:

I'll post some scope pics to a.b.s.e. Interestingly, "outside mode"
impedance doesn't seem to matter. In fact, squeezing the coax close to
the crossover improves the waveforms a bit.

When Spice conflicts with reality, where's the error?

John

In the model.

...Jim Thompson
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona Voice:(480)460-2350 | |
| E-mail Address at Website Fax:(480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |

I love to cook with wine. Sometimes I even put it in the food.
Back to top
martin griffith
electronics forum Guru


Joined: 06 May 2005
Posts: 1098

PostPosted: Mon Jun 19, 2006 5:45 pm    Post subject: Re: What S/W will simulate a transmission line type pulse transformer? Reply with quote

On Mon, 19 Jun 2006 10:01:04 -0700, in sci.electronics.design John
Larkin <jjlarkin@highNOTlandTHIStechnologyPART.com> wrote:

Quote:
On Sun, 18 Jun 2006 23:38:06 GMT, "Mike Engelhardt" <nospam@spam.org
wrote:


This is a super-wideband inverter, in both Spice and real
life:

(----------------)
in+ ----( coax )----(---------------)
in- ----(----------------)----( coax )------ out+
(---------------)------ out-

The Spice version is perfect. The real version has problems
if IN- and OUT- are both grounded (the whole thing becomes a
short) and that limits low-frequency response. Slipping a
ferrite over it somewhere helps the lf end a lot. The center
crossover should be zero-length. Done with a couple of hunks
of hardline, it's very impressive.

Interesting example. Thanks.

But it doesn't work very in SPICE if you dutifully model both
modes of each cable. Your circuit above requires four SPICE
transmission line elements. Yes, if you ignore two
propagation modes, it's perfect in SPICE but that is an
error in the application of SPICE. Below is an LTspice
schematic that illustrates perfect behavior from incorrect
analysis and the results from using 4 ideal propagation modes.

Regards,

--Mike


I'll post some scope pics to a.b.s.e. Interestingly, "outside mode"
impedance doesn't seem to matter. In fact, squeezing the coax close to
the crossover improves the waveforms a bit.

When Spice conflicts with reality, where's the error?

John

The lack of Dark Matter in spice?


martin
Back to top
Mike Engelhardt
electronics forum addict


Joined: 14 May 2005
Posts: 61

PostPosted: Mon Jun 19, 2006 8:23 pm    Post subject: Re: What S/W will simulate a transmission line type pulse transformer? Reply with quote

John,

Quote:
When Spice conflicts with reality, where's
the error?

Opps, The schematic I posted has the outputs
incorrectly connected. Below is a revised
schematic. It becomes an ideal inverter as
the current in the shield in driven to zero.

The thing I'm trying to point out is what the
SPICE transmission line element is doing -- a
single mode. To do a transmission line inverter,
you need two modes or two transmission line
elements as in the 1st netlist I posted. The
other mode results in the field that is external
to the cable and will be more problematic to
model. In Larry Nagel's Ph.D. thesis, he just
assumed it was faster propagating and higher-Z,
as if the thing were in open air.

It's a common error to think that the transmission
line element element is intended to model some
lenght of coax.

Quote:
Slipping a ferrite over it somewhere
helps the lf end a lot.

If you have field outside of the cable(your clue
is that the ferrite outside the cable helps),
you'll best model both modes of propagation.

--Mike

Version 4
SHEET 1 880 680
WIRE -240 208 -240 -96
WIRE -240 272 -240 208
WIRE -240 400 -240 352
WIRE -160 -96 -240 -96
WIRE -160 208 -240 208
WIRE 16 -16 -80 -16
WIRE 16 -16 16 -64
WIRE 16 16 16 -16
WIRE 16 96 16 48
WIRE 48 272 -48 272
WIRE 48 272 48 240
WIRE 48 288 48 272
WIRE 64 -96 -80 -96
WIRE 64 -64 16 -64
WIRE 64 16 16 16
WIRE 64 48 16 48
WIRE 96 208 -80 208
WIRE 96 240 48 240
WIRE 208 -64 160 -64
WIRE 208 -16 208 -64
WIRE 208 16 160 16
WIRE 208 16 208 -16
WIRE 208 48 160 48
WIRE 208 96 208 48
WIRE 240 -96 160 -96
WIRE 240 -16 208 -16
WIRE 240 240 192 240
WIRE 240 288 240 240
WIRE 256 208 192 208
WIRE 256 240 240 240
WIRE 288 208 256 240
WIRE 288 240 256 208
WIRE 304 -96 240 -16
WIRE 304 -16 240 -96
WIRE 336 -16 304 -16
WIRE 336 -16 336 -64
WIRE 336 16 336 -16
WIRE 336 96 336 48
WIRE 352 208 288 208
WIRE 352 240 288 240
WIRE 384 -96 304 -96
WIRE 384 -64 336 -64
WIRE 384 16 336 16
WIRE 384 48 336 48
WIRE 496 240 448 240
WIRE 496 288 496 240
WIRE 528 -64 480 -64
WIRE 528 -16 528 -64
WIRE 528 16 480 16
WIRE 528 16 528 -16
WIRE 528 48 480 48
WIRE 528 96 528 48
WIRE 560 208 448 208
WIRE 576 288 496 288
WIRE 608 -96 480 -96
WIRE 768 -16 528 -16
FLAG 48 288 0
FLAG 240 288 0
FLAG -240 400 0
FLAG -48 272 0
FLAG 560 208 0
FLAG 16 96 0
FLAG 208 96 0
FLAG -80 -16 0
FLAG 336 96 0
FLAG 528 96 0
FLAG 608 -96 0
SYMBOL tline 144 224 R0
WINDOW 3 -76 43 Left 0
SYMATTR Value Td=70n Z0=50
SYMATTR InstName T1
SYMBOL voltage -240 256 R0
WINDOW 123 0 0 Left 0
WINDOW 39 24 132 Left 0
SYMATTR InstName V1
SYMATTR Value PULSE(0 1 0 1n 1n 10n)
SYMBOL tline 400 224 R0
WINDOW 3 -76 43 Left 0
SYMATTR Value Td=70n Z0=50
SYMATTR InstName T3
SYMBOL tline 112 -80 R0
WINDOW 3 -76 43 Left 0
SYMATTR Value Td=70n Z0=50
SYMATTR InstName T2
SYMBOL tline 112 32 R0
WINDOW 3 -76 43 Left 0
SYMATTR Value Td=50n Z0=75
SYMATTR InstName T4
SYMBOL tline 432 -80 R0
WINDOW 3 -76 43 Left 0
SYMATTR Value Td=70n Z0=50
SYMATTR InstName T5
SYMBOL tline 432 32 R0
WINDOW 3 -76 43 Left 0
SYMATTR Value Td=50n Z0=75
SYMATTR InstName T6
SYMBOL res -64 192 R90
WINDOW 0 0 56 VBottom 0
WINDOW 3 32 56 VTop 0
SYMATTR InstName R1
SYMATTR Value 50
SYMBOL res -64 -112 R90
WINDOW 0 0 56 VBottom 0
WINDOW 3 32 56 VTop 0
SYMATTR InstName R2
SYMATTR Value 50
TEXT 288 352 Left 0 !.tran 0 500n 0 1n
TEXT -16 208 Bottom 0 ;IN+
TEXT -16 272 Bottom 0 ;IN-
TEXT 528 208 Bottom 0 ;OUT-
TEXT 536 288 Bottom 0 ;OUT+
TEXT -48 -96 Bottom 0 ;IN+
TEXT -48 -16 Bottom 0 ;IN-
TEXT 560 -96 Bottom 0 ;OUT-
TEXT 568 -16 Bottom 0 ;OUT+
TEXT 272 -104 Bottom 0 ;"Correct"
TEXT 272 176 Bottom 0 ;"Incorrect"
Back to top
John Larkin
electronics forum Guru


Joined: 29 Apr 2005
Posts: 4320

PostPosted: Mon Jun 19, 2006 8:39 pm    Post subject: Re: What S/W will simulate a transmission line type pulse transformer? Reply with quote

On Mon, 19 Jun 2006 20:23:55 GMT, "Mike Engelhardt" <nospam@spam.org>
wrote:

Quote:
John,

When Spice conflicts with reality, where's
the error?

Opps, The schematic I posted has the outputs
incorrectly connected. Below is a revised
schematic. It becomes an ideal inverter as
the current in the shield in driven to zero.

The thing I'm trying to point out is what the
SPICE transmission line element is doing -- a
single mode. To do a transmission line inverter,
you need two modes or two transmission line
elements as in the 1st netlist I posted. The
other mode results in the field that is external
to the cable and will be more problematic to
model. In Larry Nagel's Ph.D. thesis, he just
assumed it was faster propagating and higher-Z,
as if the thing were in open air.

It's a common error to think that the transmission
line element element is intended to model some
lenght of coax.

Slipping a ferrite over it somewhere
helps the lf end a lot.

If you have field outside of the cable(your clue
is that the ferrite outside the cable helps),
you'll best model both modes of propagation.


I tried all sorts of things to change the outer-mode impedance (like
putting dielectrics around the conductors) and nothing happens. A
lossy dielectric (like a loaded pc board, or my fingers) inhibits the
tiny ringing after the output step, but that's all.

The ferrite is just adding common-mode inductance, and it doesn't
matter where it's placed, even around an SMA connector on the sampling
head, so it's not affecting modes. Its permeability is probably close
to 1 at the 40 ps risetime edge we're seeing.

This is a lot easier to build than it is to model, so why model?

John
Back to top
Mike Engelhardt
electronics forum addict


Joined: 14 May 2005
Posts: 61

PostPosted: Tue Jun 20, 2006 12:52 am    Post subject: Re: What S/W will simulate a transmission line type pulse transformer? Reply with quote

John,

Quote:
Slipping a ferrite over it somewhere
helps the lf end a lot.

If you have field outside of the cable(your clue
is that the ferrite outside the cable helps),
you'll best model both modes of propagation.

The ferrite is just adding common-mode inductance,
and it doesn't matter where it's placed, even around
an SMA connector on the sampling head, so it's not
affecting modes.

It could affect the current into the common mode,
especially at LF. In the correct version of the
simulation with four SPICE transmission line elements,
it becomes an ideal inverting transmission line
transformer pretty much no matter how the common
mode current is driven to zero.

Quote:
This is a lot easier to build than it is to model,
so why model?

At the risk of being so fauxpaucious as to answer
a rhetorical question, I would venture that a
TDR would probably help understand the circuit
at least as easily as SPICE transmission lines.

--Mike
Back to top
Joerg
electronics forum Guru


Joined: 05 May 2005
Posts: 3533

PostPosted: Tue Jun 20, 2006 11:02 am    Post subject: Re: What S/W will simulate a transmission line type pulse transformer? Reply with quote

Hello Mike,

Quote:

If you have field outside of the cable(your clue
is that the ferrite outside the cable helps),
you'll best model both modes of propagation.


It has outside field. To keep the Federales away (FCC) it might be good
to shield somehow. On the lab bench I sometimes use Danish butter cookie
cans for that but this leads to weight issues :-(

--
Regards, Joerg

http://www.analogconsultants.com
Back to top
Google

Back to top
Display posts from previous:   
Post new topic   Reply to topic Page 1 of 1 [14 Posts] View previous topic :: View next topic
The time now is Wed Oct 18, 2017 2:59 pm | All times are GMT
Forum index » Electronix » cad
Jump to:  

Similar Topics
Topic Author Forum Replies Last Post
No new posts TV signal line converter Andy Basics 1 Thu Jul 20, 2006 10:12 am
No new posts Count 1ns pulse Paul Taylor design 48 Wed Jul 19, 2006 3:42 pm
No new posts Why are the KLK type(multimeter) fuses so expensive? itsme.ultimate@gmail.com Repair 1 Wed Jul 19, 2006 7:49 am
No new posts Programmable pulse generator. JimW design 14 Mon Jul 17, 2006 10:13 pm
No new posts pen type cases/ enclosures John Mitchell components 0 Fri Jul 14, 2006 12:39 pm

Copyright © 2004-2005 DeniX Solutions SRL
Other DeniX Solutions sites: Unix/Linux blog |  Unix/Linux documentation |  Unix/Linux forums |  Medicine forum |  Science forum  |  Send and track newsletters


Powered by phpBB © 2001, 2005 phpBB Group