[LTSpice IV] Circuit with floating nodes on using relaysw

[Olaf]

Hi,

from the attached schematics I've got the error/warning:

WARNING: Node N005 is floating.
WARNING: Node N007 is floating.
WARNING: Node N003 is floating.
WARNING: Node N013 is floating.

....

This circuit has floating nodes.

I'm not aware on floating nodes. I assume a simple on/off switch with 2
contacts - since I use 4 of them this could produce the problem
mentioned above. Further more there are only 2 wire handles on the symbol.

Did I miss something? How to fix it?

Thanks,
Olaf

 

[qrk]

On Tue, 16 Dec 2008 13:44:14 +0100, Olaf <is.er@inter.net> wrote:

Hi,

from the attached schematics I've got the error/warning:

WARNING: Node N005 is floating.
WARNING: Node N007 is floating.
WARNING: Node N003 is floating.
WARNING: Node N013 is floating.

...

This circuit has floating nodes.

I'm not aware on floating nodes. I assume a simple on/off switch with 2
contacts - since I use 4 of them this could produce the problem
mentioned above. Further more there are only 2 wire handles on the symbol.

Did I miss something? How to fix it?

Thanks,
Olaf

Your input terminals on the switches are floating. Grounding all the
minus input terminals of the switches will solve your floating node
issue.

---
Mark

 

[Olaf]

I'm not aware on floating nodes. I assume a simple on/off switch with 2
contacts - since I use 4 of them this could produce the problem
mentioned above. Further more there are only 2 wire handles on the symbol.

Did I miss something? How to fix it?

Thanks,
Olaf

Your input terminals on the switches are floating. Grounding all the
minus input terminals of the switches will solve your floating node
issue.

Thank you! It would be interesting how to design different grounds than.

Anyway, I still have problems. I found the hint that I should label the
nets to get information about nodes which does have problems (otherwise
only the node number is shown). Is this really the only way? At this
time, I've got the error about singular matrix:

Singular matrix: Check nodes c_low and c_high
Iteration No. 6
Fatal Error: Singular matrix: check nodes c_low and c_high
Iteration No. 6

Did I miss something again?

Thanks,
Olaf

 

[Olaf]

Thank you! It would be interesting how to design different grounds than.

Anyway, I still have problems. I found the hint that I should label the
nets to get information about nodes which does have problems (otherwise
only the node number is shown). Is this really the only way? At this
time, I've got the error about singular matrix:

Singular matrix: Check nodes c_low and c_high
Iteration No. 6
Fatal Error: Singular matrix: check nodes c_low and c_high
Iteration No. 6

Did I miss something again?

yes, after changing the treshold of switches to 0.9V it works.

Greetings,
Olaf

 

[Olaf]

Now I'm really confused. I added a lossy transmission line LTRA which
results in an floating node "B". I can't get rip up of this. What's
wrong with it?

Thanks,
Olaf

 

[krw]

In article <gib02j$cgn$1@fuerst.cs.uni-magdeburg.de>,
is.er@inter.net says...>

Now I'm really confused. I added a lossy transmission line LTRA which
results in an floating node "B". I can't get rip up of this. What's
wrong with it?

I don't use LT Spice, but I often have to insert 1G resistors
around capacitors and inductors to get circuits to converge.
Thinking about what happens in an "ideal" world, this sort of thing
is understandable.

 

[Jim Thompson]

On Wed, 17 Dec 2008 09:55:50 -0600, krw <krw@att.zzzzzzzzz> wrote:

In article <gib02j$cgn$1@fuerst.cs.uni-magdeburg.de>,
is.er@inter.net says...
Now I'm really confused. I added a lossy transmission line LTRA which
results in an floating node "B". I can't get rip up of this. What's
wrong with it?

I don't use LT Spice, but I often have to insert 1G resistors
around capacitors and inductors to get circuits to converge.
Thinking about what happens in an "ideal" world, this sort of thing
is understandable.

I made a symbol for PSpice...

_
-|_|

(with a "X" in the box, can't do in ASCII ;-)

easy to tack onto a schematic without taking up space... it netlists
as a 1G resistor to ground/node-zero.

...Jim Thompson
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona 85048 Skype: Contacts Only | |
| Voice480)460-2350 Fax: Available upon request | Brass Rat |
| E-mail Icon at http://www.analog-innovations.com | 1962 |

I love to cook with wine Sometimes I even put it in the food

 

[Charlie E.]

On Wed, 17 Dec 2008 14:50:11 +0100, Olaf <is.er@inter.net> wrote:

Now I'm really confused. I added a lossy transmission line LTRA which
results in an floating node "B". I can't get rip up of this. What's
wrong with it?

Thanks,
Olaf

Olaf,
I didn't look at your circuit, but the guideline is that EVERY node
needs to have a DC path to ground. Some parts, like transformers and
transmission lines modeled via 'behavioral' modeling, don't have a
path through them for DC, so you have to have an actual ground at both
ends.

You mentioned having different grounds for different areas of the
circuit. To do this, you use a 'buffered' ground, a ground isolated
by a large resistance, such as 10MEG, or even 1G between the ground
and the circuit in question. You still have the DC path so that the
simulator can establish voltage levels, but the 'ground' level between
the two sections can now be at different levels.

For more info, look at:
http://edmondsonengineering.com/grounds.aspx


Charlie

 

[Jim Thompson]

On Wed, 17 Dec 2008 16:24:56 GMT, Charlie E. <edmondson@ieee.org>
wrote:

On Wed, 17 Dec 2008 14:50:11 +0100, Olaf <is.er@inter.net> wrote:

Now I'm really confused. I added a lossy transmission line LTRA which
results in an floating node "B". I can't get rip up of this. What's
wrong with it?

Thanks,
Olaf

Olaf,
I didn't look at your circuit, but the guideline is that EVERY node
needs to have a DC path to ground. Some parts, like transformers and
transmission lines modeled via 'behavioral' modeling, don't have a
path through them for DC, so you have to have an actual ground at both
ends.

You mentioned having different grounds for different areas of the
circuit. To do this, you use a 'buffered' ground, a ground isolated
by a large resistance, such as 10MEG, or even 1G between the ground
and the circuit in question. You still have the DC path so that the
simulator can establish voltage levels, but the 'ground' level between
the two sections can now be at different levels.

For more info, look at:
http://edmondsonengineering.com/grounds.aspx


Charlie

"Advanced users often create a custom part that they use to place
between equivalent nets."

Yes we do, after we find that Crapture screws us with vague "Warnings"
;-)

...Jim Thompson
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona 85048 Skype: Contacts Only | |
| Voice480)460-2350 Fax: Available upon request | Brass Rat |
| E-mail Icon at http://www.analog-innovations.com | 1962 |

I love to cook with wine Sometimes I even put it in the food

 

[krw]

In article <lh9ik418h33mfla54bsrjsh71d2sluc3mk@4ax.com>, To-Email-
Use-The-Envelope-Icon@My-Web-Site.com says...>

On Wed, 17 Dec 2008 09:55:50 -0600, krw <krw@att.zzzzzzzzz> wrote:

In article <gib02j$cgn$1@fuerst.cs.uni-magdeburg.de>,
is.er@inter.net says...
Now I'm really confused. I added a lossy transmission line LTRA which
results in an floating node "B". I can't get rip up of this. What's
wrong with it?

I don't use LT Spice, but I often have to insert 1G resistors
around capacitors and inductors to get circuits to converge.
Thinking about what happens in an "ideal" world, this sort of thing
is understandable.

I made a symbol for PSpice...

_
-|_|

(with a "X" in the box, can't do in ASCII ;-)

easy to tack onto a schematic without taking up space... it netlists
as a 1G resistor to ground/node-zero.

That's a good idea! I'll have to figure out the best way to do it.

 

[Jim Thompson]

On Wed, 17 Dec 2008 12:24:42 -0600, krw <krw@att.zzzzzzzzz> wrote:

In article <lh9ik418h33mfla54bsrjsh71d2sluc3mk@4ax.com>, To-Email-
Use-The-Envelope-Icon@My-Web-Site.com says...
On Wed, 17 Dec 2008 09:55:50 -0600, krw <krw@att.zzzzzzzzz> wrote:

In article <gib02j$cgn$1@fuerst.cs.uni-magdeburg.de>,
is.er@inter.net says...
Now I'm really confused. I added a lossy transmission line LTRA which
results in an floating node "B". I can't get rip up of this. What's
wrong with it?

I don't use LT Spice, but I often have to insert 1G resistors
around capacitors and inductors to get circuits to converge.
Thinking about what happens in an "ideal" world, this sort of thing
is understandable.

I made a symbol for PSpice...

_
-|_|

(with a "X" in the box, can't do in ASCII ;-)

easy to tack onto a schematic without taking up space... it netlists
as a 1G resistor to ground/node-zero.

That's a good idea! I'll have to figure out the best way to do it.

The trick is that it's a 1-pin subcircuit... node "0" is global.

If you're using PSpice I can E-mail you the "sym" file (it's text).

...Jim Thompson
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona 85048 Skype: Contacts Only | |
| Voice480)460-2350 Fax: Available upon request | Brass Rat |
| E-mail Icon at http://www.analog-innovations.com | 1962 |

I love to cook with wine Sometimes I even put it in the food

 

[krw]

In article <ftkik4luiphep37rsao8hi1033v7g1hvcr@4ax.com>, To-Email-
Use-The-Envelope-Icon@My-Web-Site.com says...>

On Wed, 17 Dec 2008 12:24:42 -0600, krw <krw@att.zzzzzzzzz> wrote:

In article <lh9ik418h33mfla54bsrjsh71d2sluc3mk@4ax.com>, To-Email-
Use-The-Envelope-Icon@My-Web-Site.com says...
On Wed, 17 Dec 2008 09:55:50 -0600, krw <krw@att.zzzzzzzzz> wrote:

In article <gib02j$cgn$1@fuerst.cs.uni-magdeburg.de>,
is.er@inter.net says...
Now I'm really confused. I added a lossy transmission line LTRA which
results in an floating node "B". I can't get rip up of this. What's
wrong with it?

I don't use LT Spice, but I often have to insert 1G resistors
around capacitors and inductors to get circuits to converge.
Thinking about what happens in an "ideal" world, this sort of thing
is understandable.

I made a symbol for PSpice...

_
-|_|

(with a "X" in the box, can't do in ASCII ;-)

easy to tack onto a schematic without taking up space... it netlists
as a 1G resistor to ground/node-zero.

That's a good idea! I'll have to figure out the best way to do it.


The trick is that it's a 1-pin subcircuit... node "0" is global.

I'm pretty sure ground is global, but I'll have to test it again.

If you're using PSpice I can E-mail you the "sym" file (it's text).

Nope. Can't afford PSpice. Unfortunately, I'm stuck with @#*$&
Tina. If anyone one is looking at Tina, FORGET IT! The Freebie TI
version is alright for what it is, but the real version is next to
worthless. In fact worthless would be less aggravating.

 

[qrk]

On Wed, 17 Dec 2008 14:11:28 -0600, krw <krw@att.zzzzzzzzz> wrote:

In article <ftkik4luiphep37rsao8hi1033v7g1hvcr@4ax.com>, To-Email-
Use-The-Envelope-Icon@My-Web-Site.com says...
On Wed, 17 Dec 2008 12:24:42 -0600, krw <krw@att.zzzzzzzzz> wrote:

In article <lh9ik418h33mfla54bsrjsh71d2sluc3mk@4ax.com>, To-Email-
Use-The-Envelope-Icon@My-Web-Site.com says...
On Wed, 17 Dec 2008 09:55:50 -0600, krw <krw@att.zzzzzzzzz> wrote:

In article <gib02j$cgn$1@fuerst.cs.uni-magdeburg.de>,
is.er@inter.net says...
Now I'm really confused. I added a lossy transmission line LTRA which
results in an floating node "B". I can't get rip up of this. What's
wrong with it?

I don't use LT Spice, but I often have to insert 1G resistors
around capacitors and inductors to get circuits to converge.
Thinking about what happens in an "ideal" world, this sort of thing
is understandable.

I made a symbol for PSpice...

_
-|_|

(with a "X" in the box, can't do in ASCII ;-)

easy to tack onto a schematic without taking up space... it netlists
as a 1G resistor to ground/node-zero.

That's a good idea! I'll have to figure out the best way to do it.


The trick is that it's a 1-pin subcircuit... node "0" is global.

I'm pretty sure ground is global, but I'll have to test it again.

If you're using PSpice I can E-mail you the "sym" file (it's text).

Nope. Can't afford PSpice. Unfortunately, I'm stuck with @#*$&
Tina. If anyone one is looking at Tina, FORGET IT! The Freebie TI
version is alright for what it is, but the real version is next to
worthless. In fact worthless would be less aggravating.


You could use LTspice. Works good, compatible with PSpice syntax, and

free. The new multithreaded capability is interesting, but I don't
have the time right now to figure out how to set it up so it's faster
than version 3 (in limited trials, limiting the number of threads to
number of processors minus 1 seemed to work best).

---
Mark

 

[krw]

In article <9ptkk49dna65ruuqldsqsoccs6ekfpeema@4ax.com>,
SpamTrap@spam.net says...>

On Wed, 17 Dec 2008 14:11:28 -0600, krw <krw@att.zzzzzzzzz> wrote:

In article <ftkik4luiphep37rsao8hi1033v7g1hvcr@4ax.com>, To-Email-
Use-The-Envelope-Icon@My-Web-Site.com says...
On Wed, 17 Dec 2008 12:24:42 -0600, krw <krw@att.zzzzzzzzz> wrote:

In article <lh9ik418h33mfla54bsrjsh71d2sluc3mk@4ax.com>, To-Email-
Use-The-Envelope-Icon@My-Web-Site.com says...
On Wed, 17 Dec 2008 09:55:50 -0600, krw <krw@att.zzzzzzzzz> wrote:

In article <gib02j$cgn$1@fuerst.cs.uni-magdeburg.de>,
is.er@inter.net says...
Now I'm really confused. I added a lossy transmission line LTRA which
results in an floating node "B". I can't get rip up of this. What's
wrong with it?

I don't use LT Spice, but I often have to insert 1G resistors
around capacitors and inductors to get circuits to converge.
Thinking about what happens in an "ideal" world, this sort of thing
is understandable.

I made a symbol for PSpice...

_
-|_|

(with a "X" in the box, can't do in ASCII ;-)

easy to tack onto a schematic without taking up space... it netlists
as a 1G resistor to ground/node-zero.

That's a good idea! I'll have to figure out the best way to do it.


The trick is that it's a 1-pin subcircuit... node "0" is global.

I'm pretty sure ground is global, but I'll have to test it again.

If you're using PSpice I can E-mail you the "sym" file (it's text).

Nope. Can't afford PSpice. Unfortunately, I'm stuck with @#*$&
Tina. If anyone one is looking at Tina, FORGET IT! The Freebie TI
version is alright for what it is, but the real version is next to
worthless. In fact worthless would be less aggravating.


You could use LTspice. Works good, compatible with PSpice syntax, and
free. The new multithreaded capability is interesting, but I don't
have the time right now to figure out how to set it up so it's faster
than version 3 (in limited trials, limiting the number of threads to
number of processors minus 1 seemed to work best).

I tried LTspice and still have it loaded. I didn't like it either,
though given my problems with Tina I'll likely give it a third
chance. I can't remember what my issues with it were (perhaps
libraries).

--
Keith

 

[qrk]

On Fri, 19 Dec 2008 06:39:36 -0600, krw <krw@att.zzzzzzzzz> wrote:

In article <9ptkk49dna65ruuqldsqsoccs6ekfpeema@4ax.com>,
SpamTrap@spam.net says...
On Wed, 17 Dec 2008 14:11:28 -0600, krw <krw@att.zzzzzzzzz> wrote:

In article <ftkik4luiphep37rsao8hi1033v7g1hvcr@4ax.com>, To-Email-
Use-The-Envelope-Icon@My-Web-Site.com says...
On Wed, 17 Dec 2008 12:24:42 -0600, krw <krw@att.zzzzzzzzz> wrote:

In article <lh9ik418h33mfla54bsrjsh71d2sluc3mk@4ax.com>, To-Email-
Use-The-Envelope-Icon@My-Web-Site.com says...
On Wed, 17 Dec 2008 09:55:50 -0600, krw <krw@att.zzzzzzzzz> wrote:

In article <gib02j$cgn$1@fuerst.cs.uni-magdeburg.de>,
is.er@inter.net says...
Now I'm really confused. I added a lossy transmission line LTRA which
results in an floating node "B". I can't get rip up of this. What's
wrong with it?

I don't use LT Spice, but I often have to insert 1G resistors
around capacitors and inductors to get circuits to converge.
Thinking about what happens in an "ideal" world, this sort of thing
is understandable.

I made a symbol for PSpice...

_
-|_|

(with a "X" in the box, can't do in ASCII ;-)

easy to tack onto a schematic without taking up space... it netlists
as a 1G resistor to ground/node-zero.

That's a good idea! I'll have to figure out the best way to do it.


The trick is that it's a 1-pin subcircuit... node "0" is global.

I'm pretty sure ground is global, but I'll have to test it again.

If you're using PSpice I can E-mail you the "sym" file (it's text).

Nope. Can't afford PSpice. Unfortunately, I'm stuck with @#*$&
Tina. If anyone one is looking at Tina, FORGET IT! The Freebie TI
version is alright for what it is, but the real version is next to
worthless. In fact worthless would be less aggravating.


You could use LTspice. Works good, compatible with PSpice syntax, and
free. The new multithreaded capability is interesting, but I don't
have the time right now to figure out how to set it up so it's faster
than version 3 (in limited trials, limiting the number of threads to
number of processors minus 1 seemed to work best).

I tried LTspice and still have it loaded. I didn't like it either,
though given my problems with Tina I'll likely give it a third
chance. I can't remember what my issues with it were (perhaps
libraries).

I find that LTspice works well. The first few versions of the new
version 4 had big problems, but Mike E. fixed them quickly. The main
thing I don't like about LTspice is the output graphing and schematic
interface. PSpice has much better graphing utility. Libraries are easy
to deal with in LTspice. Adding diodes, transistors, and opamps to
LTspice's library is easy. LT updates to the libraries maintain your
additions. Big bonus is PSpice syntax compatibility which means
quicker learning curve for me and accepting PSpice card decks.

---
Mark

 

[krw]

In article <jbunk49tmuu7fes3kcnhu1b41su1ata314@4ax.com>,
SpamTrap@spam.net says...>

On Fri, 19 Dec 2008 06:39:36 -0600, krw <krw@att.zzzzzzzzz> wrote:

In article <9ptkk49dna65ruuqldsqsoccs6ekfpeema@4ax.com>,
SpamTrap@spam.net says...
On Wed, 17 Dec 2008 14:11:28 -0600, krw <krw@att.zzzzzzzzz> wrote:

In article <ftkik4luiphep37rsao8hi1033v7g1hvcr@4ax.com>, To-Email-
Use-The-Envelope-Icon@My-Web-Site.com says...
On Wed, 17 Dec 2008 12:24:42 -0600, krw <krw@att.zzzzzzzzz> wrote:

In article <lh9ik418h33mfla54bsrjsh71d2sluc3mk@4ax.com>, To-Email-
Use-The-Envelope-Icon@My-Web-Site.com says...
On Wed, 17 Dec 2008 09:55:50 -0600, krw <krw@att.zzzzzzzzz> wrote:

In article <gib02j$cgn$1@fuerst.cs.uni-magdeburg.de>,
is.er@inter.net says...
Now I'm really confused. I added a lossy transmission line LTRA which
results in an floating node "B". I can't get rip up of this. What's
wrong with it?

I don't use LT Spice, but I often have to insert 1G resistors
around capacitors and inductors to get circuits to converge.
Thinking about what happens in an "ideal" world, this sort of thing
is understandable.

I made a symbol for PSpice...

_
-|_|

(with a "X" in the box, can't do in ASCII ;-)

easy to tack onto a schematic without taking up space... it netlists
as a 1G resistor to ground/node-zero.

That's a good idea! I'll have to figure out the best way to do it.


The trick is that it's a 1-pin subcircuit... node "0" is global.

I'm pretty sure ground is global, but I'll have to test it again.

If you're using PSpice I can E-mail you the "sym" file (it's text).

Nope. Can't afford PSpice. Unfortunately, I'm stuck with @#*$&
Tina. If anyone one is looking at Tina, FORGET IT! The Freebie TI
version is alright for what it is, but the real version is next to
worthless. In fact worthless would be less aggravating.


You could use LTspice. Works good, compatible with PSpice syntax, and
free. The new multithreaded capability is interesting, but I don't
have the time right now to figure out how to set it up so it's faster
than version 3 (in limited trials, limiting the number of threads to
number of processors minus 1 seemed to work best).

I tried LTspice and still have it loaded. I didn't like it either,
though given my problems with Tina I'll likely give it a third
chance. I can't remember what my issues with it were (perhaps
libraries).

I find that LTspice works well. The first few versions of the new
version 4 had big problems, but Mike E. fixed them quickly. The main
thing I don't like about LTspice is the output graphing and schematic
interface. PSpice has much better graphing utility. Libraries are easy
to deal with in LTspice. Adding diodes, transistors, and opamps to
LTspice's library is easy. LT updates to the libraries maintain your
additions. Big bonus is PSpice syntax compatibility which means
quicker learning curve for me and accepting PSpice card decks.

Tina will accept PSpice models. Well, about as well as it does
anything. Its schematic entry is good, but the graphics I/O is
really buggy. It is impossible to get a consistent output without
tweaking a million things for every plot. I wish we could afford
PSpice, but I guess if it were my money I'd make do, too.

 

[Joel Koltner]

"krw" <krw@att.zzzzzzzzz> wrote in message
news:MPG.23b5b835656347d298971f@news.individual.net...

I wish we could afford
PSpice, but I guess if it were my money I'd make do, too.

You can get SI-Metrix -- which IMO is quite good -- bundled into various EDA
tool's "SPICE" offering... Pulsonix is one of the licensees, although I know
there are others. (Pulsonix w/SPICE is much less expensive than ORCAD
w/PSpice, although Pulsonix doesn't really qualify as "cheap" anymore.)

Easy-PC -- from the same company as Pulsonix -- used to bundle SI-Metrix into
their Easy-PC program, but it appears they no longer do (the screen shots on
page 5 of the Easy-PC brochure here:
http://www.pcb-sw.com/uploaded/files/Easy-PCBrochure.pdf ...are SI-Metrix, but
the makers of Easy-PC state here: http://www.numberone.com/easyspice.asp
....that they're no longer selling new copies of Easy-Spice). This might be
due to SI-Metrix having crept rather upwards in price over the past handful of
years, putting it out of the price range of the "low end" that Easy-PC seems
pretty committed to.

---Joel