LTspice has a nice Tian probe to study feedback.
There is also the more complex but even more informative Middlebrook2006 method.
Better information on differential feedback is now the next step forward and there is no convenient tool, AFAIK.
Dr Paul Hurst has a paper about the use of baluns to separate out the common mode and differential mode loops and Frank Wiedmann has a link to a paper by Ken Kundert about how to do this in the Spectre simulator.
Ken's paper has a little information on Spice but anyone already have a sub-circuit for this in LTspice?
It needs ideal transformers, never done this in LTSpice, any ideas?
David.
There is also the more complex but even more informative Middlebrook2006 method.
Better information on differential feedback is now the next step forward and there is no convenient tool, AFAIK.
Dr Paul Hurst has a paper about the use of baluns to separate out the common mode and differential mode loops and Frank Wiedmann has a link to a paper by Ken Kundert about how to do this in the Spectre simulator.
Ken's paper has a little information on Spice but anyone already have a sub-circuit for this in LTspice?
It needs ideal transformers, never done this in LTSpice, any ideas?
David.
Last edited:
http://www.intusoft.com/articles/satcore.pdf in the usual Google search shows one DC ideal spice xmfr - fig. 3
Intusoft is a general spice modeling resource - do check thier news mletters, app notes
I remeber a more symmetric looking model - I thought by Mike, somewhere on the Ltspice Yahoo users group, but couldn't find it last I looked - and I really don't want to try again with the new "infinite scroll" UI yahoo cursed us with
I am looking in sim at a circuit with fully diferential amp and finding weird cross modulation/mode conversion showing us as a annoying diff AC response imbalanace around the intercept frequency of the cm loop - don't know if its real or a LT1994 op amp modeling fail
Intusoft is a general spice modeling resource - do check thier news mletters, app notes
I remeber a more symmetric looking model - I thought by Mike, somewhere on the Ltspice Yahoo users group, but couldn't find it last I looked - and I really don't want to try again with the new "infinite scroll" UI yahoo cursed us with
I am looking in sim at a circuit with fully diferential amp and finding weird cross modulation/mode conversion showing us as a annoying diff AC response imbalanace around the intercept frequency of the cm loop - don't know if its real or a LT1994 op amp modeling fail
Last edited:
Thank you for the link and the Intusoft recommendation. Expected they were mostly proprietary but coincidentally was just about to search them.
Need a DC-DC transformer and that claims to do it but lack of symmetry makes it not quite obvious, will check.
And I really hate the Yahoo interface too, I also tried and quit, hence my question here and not in their LTSpice forum.
Best wishes
David
PS. Some of the information looks very useful for another query I had about real transformers.
Extraordinary how often Middlebrook is involved in smart work.
Last edited:
Checked and had a think.
Found another balun, this time for the Eldo Spice simulator, also built with ideal transformers.
Ideal transformers seem to be a primitive even in the previously unknown to me Eldo, but not in LTSpice.
Rather than build ideal transformers from controlled sources and then build baluns from ideal transformers I may build the balun directly.
Anyone have an LTSpice balun?
David
Neat solution, simple and effective on a low impedance source.
But I would like check some internal loops and I am not sure it would be accurate there.
On a related topic from an earlier post.
You mentioned a Tian probe inside EC OPS with a counter intuitive plot.
I also have noticed unexpected phase response from Tian probes around the VAS.
Seemed mathematically consistent so maybe just a problem with my expectations.
I plan to check this with Middlebrook 2006 probe eventually.
I have looked at Rosenstark 1984 and Frank Wiedmann but still not entirely clear. There are question of interpretation.
You had any more ideas on this?
Best wishes
David
.SUBCKT BALUN_DM_PROBE s1a s2a da s1b s2b db
*
* s1a = difference-mode floating signal 1 for input/output "a"
* s2a = difference-mode floating signal 2 for input/output "a"
* da = difference-mode ground-referenced signal for input/output "a"
* s1b = difference-mode floating signal 1 for input/output "b"
* s2b = difference-mode floating signal 2 for input/output "b"
* db = difference-mode ground-referenced signal for input/output "b"
*
* Connect da and db together externally with a loop gain probe
*
X1 db 0 s1b NCM TRANSFORMER
X2 db 0 NCM s2b TRANSFORMER
X3 da 0 s1a NCM TRANSFORMER
X4 da 0 NCM s2a TRANSFORMER
* R1, R2 and R3 prevent floating nodes
R1 da 0 1E9
R2 db 0 1E9
R3 NCM 0 1E9
*
.ENDS BALUN_DM_PROBE
.SUBCKT BALUN_CM_PROBE s1a s2a ca s1b s2b cb
*
* s1a = diff mode signal 1 for input/output "a"
* s2a = diff mode signal 2 for input/output "a"
* ca = common mode signal for input/output "a"
* s1b = diff mode signal 1 for input/output "b"
* s2b = diff mode signal 2 for input/output "b"
* cb = common mode signal for input/output "b"
*
* Connect ca and cb together externally with a loop gain probe
*
X1 NDM 0 s1b cb transformer
X2 NDM 0 cb s2b transformer
X3 NDM 0 s1a ca transformer
X4 NDM 0 ca s2a transformer
* R1, R2 and R3 prevent floating nodes
R1 ca 0 1E9
R2 cb 0 1E9
R3 NDM 0 1E9
*
.ENDS BALUN_CM_PROBE
Thanks, but I don't think this is too useful in LTSpice.
What simulator is it from?
Best wishes
David
PSpice. Why would this not work in LTSPICE? There is no specific trick or code, only subckt with transformers and resistors.
I know PSpice and LTspice have some incompatibilities but I don't know details.
AFAIK LTSpice does not have an ideal transformer as a primitive, in other words no "X" component.
Hence my earlier comments.
Best wishes
David
Last edited:
Are we grumpy today?
Took me about 5 seconds on Google: Transformers - LTwiki-Wiki for LTspice
You can't make a differential/common mode probe without baluns/transformers.
Yes I read that before I posted. Note
"I've created an ideal transformer so it should work at all frequencies, even including DC...?
No, but lots of users completely misunderstand or overlook this..."
The balun requires operation at DC and LTspice models transformers as coupled inductors so they don't work that way.
PSpice apparently models transformers differently, as ideal elements with equations that extend to DC.
Of course, that's the point of my enquiry. But a balun can be made from controlled sources as in JCX's link.
Pretty simple really, I just hoped someone would have an LTSpice ASC file to save me some time.
Not sure why you misinterpreted my mood, I appreciate responses.
It's a free forum so at worst it's no loss.
Best wishes
David
Last edited:
DC correct is valuable for inserting in circuits/feedback loops
the symmetric dependant source core of the last model is I think what I remembered
I believe that if instead of Lm in the middle you use a high vlaue R then the circuit works to DC
yep - thats the one:
the symmetric dependant source core of the last model is I think what I remembered
I believe that if instead of Lm in the middle you use a high vlaue R then the circuit works to DC
yep - thats the one:
Attachments
Last edited:
No, PSpice doesn't have any model beyond the same coupled inductors. For the diff and common mode probes balun, below is mine. Why didn't you ask "how to implement an ideal balun"?
* Ideal transformer with a secondary/primary turns ratio of 0.5
* ph = primary hot
* pc = primary cold
* sh = secondary hot
* sc = secondary cold
*
.SUBCKT TRANSFORMER ph pc sh sc
F1 ph pc V1 0.5
V1 N001 N002 0
* R1 prevents loops of voltage sources
R1 N002 sh 5e-7
E1 N001 sc ph pc 0.5
*
.ENDS TRANSFORMER
The Pspice model does appear have a model that is not the same as LTspice. AFAIK LTspice has no equivalent of your X components.
My first post did ask
"Dr Paul Hurst has a paper about the use of baluns to separate out the common mode and differential mode loops.".."anyone already have a sub-circuit for this in LTspice?"
Looks clear to me.
Best wishes
David
Very late here... X are not components
I can't imagine LTSpice doesn't have this, it's part of the original Berkeley Spice from day one:
----
Subcircuit instantiation
Purpose
This statement causes the referenced subcircuit to be inserted into the circuit using the given nodes to replace the argument nodes in the definition. It allows a block of circuitry to be defined once and then used in several places.
General form
X<name> [node]* <subcircuit name> [PARAMS: <<name> =<value>>*]
+ [TEXT: < <name> = <text value> >* ]
----
OK. I am not very familiar with netlist format because I usually work within LTSpice, I misinterpreted the syntax.
Nice to sort this out.
Best wishes
David
Last edited:
- Status
- This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.