Keyboard Shortcuts
ctrl + shift + ? :
Show all keyboard shortcuts
ctrl + g :
Navigate to a group
ctrl + shift + f :
Find
ctrl + / :
Quick actions
esc to dismiss
Likes
- LTspice
- Messages
Search
|
Re: Graph Color
John Woodgate
In message <llj19s+16o17n9@...>, dated Wed, 21 May 2014, "1sailingbear@... [LTspice]" <LTspice@...> writes:
I am new here and have a newbie question.It is possible, I think, but rather complicated. But do you really need all 27 curves on the same plot? You can have more than one plot on the screen (tiled) and you can choose which curves to display on each. With the screen focus on a plot pane, View => Visible traces. -- OOO - Own Opinions Only. With best wishes. See www.jmwa.demon.co.uk Nondum ex silvis sumus John Woodgate, J M Woodgate and Associates, Rayleigh, Essex UK |
|
Re: Graph Color
Hello Sven,
1. Attach a cursor to e.g. V(out). 2. Use the up/down arrow key of he keyboard to jump to the waveform you are interested. 3. Move the mouse cursor near the waveform-crosshair. The mouse cursor will then change to 1, if it's the first of the two possible cursors. Now right mouse click. LTspice will then report: Cursor 1: a=... b=... c=... (Run 7/15) Best regards, Helmut |
|
Simulating LM 6172
I am new to LT spice. I want to use the component LM 6172 in my schematic, I have downloaded the include file from the the path and used a generic opamp2.asy. However, the attributed is same as general opamp even after including the file. Could you help me how to solve this problem? Also, the way to include the .MOD extension file in LT Spice found in the group.?
|
|
Graph Color
Hi there, I am new here and have a newbie question. The .ac analysis of my tube schematic shows 27 graphs as I run 3 potentiometer with a step directive: .step param a list .1 .5 .99 The Graph has now 27 lines in different colors. Where can I find which color belongs to which settings of my potentiometer? Regards Sven |
|
Re: Pull-Push transformer for valve amp in LTspice
No, it wasn't about basic usage such as this, I think it was about analogspiceman's "xfrmr" library, two primaries for a push-pull or similar, some year or two ago. I tried to search the archives but I couldn't find anything. It doesn't matter, anyway, the OP got his answer. Vlad ______________________ -- holding, among others: a universal analog/digital filter, block-level models for power electronics (and not only), math blocks with a more stream-lined approach, some digital ADC, DAC, (synchronous-)counter, JKflop, etc. |
|
Re: Pull-Push transformer for valve amp in LTspice
? ?"...?I really can't escape the feeling there was a topic somewhere about some impossibility of having two primaries in a transformer.?"
There may be special cases. ?Other than that, though, coupled windings are just windings and it makes no difference whether you call one a primary winding or a secondary winding. ?LTspice correctly handles more than two coupled windings, no problem.
One special case where two primaries can be a problem (if modeled incorrectly), is the not-uncommon dual-voltage power transformer, which has two primary windings that are connected either in parallel or in series, to adapt to the AC mains voltage in your country. ?If you model the primary by simply taking two inductors with no resistance, and connect them in parallel, LTspice will complain about that, and quit. ?It is a legitimate complaint, because paralleled lossless inductors and/or voltage sources are not allowed in SPICE ... easily fixed by adding any amount of series resistance in each winding.
I vaguely recall another situation in this email list, where someone was using a bizarre mixture of both inductors and controlled sources to represent his transformer. ?(Recall that transformers can be modeled using EITHER coupled inductors, OR a network of resistors and controlled sources (google "ideal transformer model"). ?This one haphazardly combined both.)
Regards,
Andy |
|
Re: Pull-Push transformer for valve amp in LTspice
John Woodgate
In message <537CC53F.1010307@...>, dated Wed, 21 May 2014, "Jerry Lee Marcel jerryleemarcel@... [LTspice]" <LTspice@...> writes:
The description says total primary L=100 and the individual inductances of both half-primaries is spec'd at 50H.The model works as you say, but the total inductance is 200 H not 100 H. -- OOO - Own Opinions Only. With best wishes. See www.jmwa.demon.co.uk Nondum ex silvis sumus John Woodgate, J M Woodgate and Associates, Rayleigh, Essex UK |
|
Re: Pull-Push transformer for valve amp in LTspice
¿ªÔÆÌåÓýOut of morbid curiosity, I opened the "transPPb.INC" model file, and noticed a gross error.The description says total primary L=100 and the individual inductances of both half-primaries is spec'd at 50H. It doesn't prevent the sim to work, but I doubt it's the correct value. It just shows that people who are clever enough to create models don't necessarily undestand the physics of it. Le 21/05/2014 15:59, Vlad
imbvlad@... [LTspice] a ¨¦crit?:
? |
|
Re: Pull-Push transformer for valve amp in LTspice
John Woodgate
In message <CALFKJk5yokRyVCrWd5VAgEppt-AGJ7Wy6+mx5utH+s0T8JX7_A@...>, dated Wed, 21 May 2014, "Vlad imbvlad@... [LTspice]" <LTspice@...> writes:
It's not only you, by any means. Transformers come up here quite often, and I always try to respond because it's clear that many do not understand them. But just like 'Upload to Files => Temp' doesn't seem to register, neither does the transformer 'lore'. What you may be dimly recalling is something about having two generators feeding two separate windings. It MAY be OK if the numbers are right, but it MAY produce huge currents. For example, suppose there are two identical windings and 10 V is applied to one. 10 V will appear across the other one, too. Now connect a 100 V source to that second winding as well, and watch the pretty smoke. -- OOO - Own Opinions Only. With best wishes. See www.jmwa.demon.co.uk Nondum ex silvis sumus John Woodgate, J M Woodgate and Associates, Rayleigh, Essex UK |
|
Re: Pull-Push transformer for valve amp in LTspice
>??I'm really surprised > at the responses that show considerable uncertainty. Guilty, what can I say, but I really can't escape the feeling there was a topic somewhere about some impossibility of having two primaries in a transformer. Maybe there are some crossed neurons somewhere. If so, I'd rather have that checked after I'm gone. Vlad ______________________ -- holding, among others: a universal analog/digital filter, block-level models for power electronics (and not only), math blocks with a more stream-lined approach, some digital ADC, DAC, (synchronous-)counter, JKflop, etc. |
|
Re: Pull-Push transformer for valve amp in LTspice
John Woodgate
In message <lli8ok+1jht4cj@...>, dated Wed, 21 May 2014,
"pha0001@... [LTspice]" <LTspice@...> writes: Rather than point you to things to copy, I'll show you how to design. Please post to Files-Temp, not anywhere else unless advised. You have made the astonishingly common mistake of expecting transformers with microhenry inductors to work at audio or mains frequencies. The inductances need to be LARGE; their impedances need to be around 10 times the associated circuit impedances. For example, your secondary winding is 314 MICROhms at 50 Hz and the load is 8 ohms. We start with the 6.7 k a-a impedance. That is what the 8 ohms has to look like when 'seen' through the transformer. 6700/8 = 837.5 and the turns ratio of the transformer is the square root of that, i.e. 29. Now the inductance of the primary needs to be high compared with the 6.7 k at the lowest frequency you are interested in. I'll assume 20 Hz, since I don't have to buy the transformer and find room for it, but I'll use a factor of 5 for 'high'. The inductance L = 6700/(2pi*20) = 267 H. The secondary inductance is 267/837.5 = 319 millihenrys. To model in LTspice, you make the primary of two identical inductors, each a QUARTER of the total inductance and set k=1. I'm really surprised at the responses that show considerable uncertainty. Now if you were going to make the transformer you would have to consider the power to be handled and from that choose a core size and material. But I don't suppose you want to go that far. -- OOO - Own Opinions Only. With best wishes. See www.jmwa.demon.co.uk Nondum ex silvis sumus John Woodgate, J M Woodgate and Associates, Rayleigh, Essex UK |
|
Re: Pull-Push transformer for valve amp in LTspice
¿ªÔÆÌåÓýI believe you see why I prefer the multiple winding solution. Having to open the model with a text editor and reloading it in the .asc file is not my idea of immediacy.Le 21/05/2014 15:59, Vlad
imbvlad@... [LTspice] a ¨¦crit?:
? |
|
Re: Pull-Push transformer for valve amp in LTspice
¿ªÔÆÌåÓýThe problem with multiple primaries is that it may create conflictss if two sources are too strongly coupled.Indeed, when using multiple primaries, one must make sure the voltages, phases and source resistance vs. parasitic resistance are sensible. I think some transformer sub-circuits don't accept the notion of more than one excitation winding. Le 21/05/2014 15:54, Vlad
imbvlad@... [LTspice] a ¨¦crit?:
? |
|
Re: Pull-Push transformer for valve amp in LTspice
> To my great shame I must admit I haven't been able to edit the OT values in the Fender schemo. Using the "Fender Twin Reverb" example, the output transformer is modeled in the model file "transPPb.INC". Any text editor should do. I also see extra nodes/elements for parasitic resistances & co. instead of using the builtin Rser/Rpar/etc, but maybe it's intentional, for the purpose of showing. Vlad ______________________ -- holding, among others: a universal analog/digital filter, block-level models for power electronics (and not only), math blocks with a more stream-lined approach, some digital ADC, DAC, (synchronous-)counter, JKflop, etc. |
|
Re: Pull-Push transformer for valve amp in LTspice
> Indeed a dual primary xfmr can be created in LTspice. Well, I just tried it and you're right, it does work, but I know there was a discussion some time ago (years, probably) about not being able to make a more than one primary transformer in LTspice. Maybe with the Chan core? I really can't remember now. Vlad ______________________ -- holding, among others: a universal analog/digital filter, block-level models for power electronics (and not only), math blocks with a more stream-lined approach, some digital ADC, DAC, (synchronous-)counter, JKflop, etc. |
|
Re: Pull-Push transformer for valve amp in LTspice
¿ªÔÆÌåÓýIn fact all these examples use a sub-circuit instead of coupled inductors, but I know that coupled inductors work and are IMO easier to edit.To my great shame I must admit I haven't been able to edit the OT values in the Fender schemo. Le 21/05/2014 15:41, Jerry Lee Marcel
jerryleemarcel@... [LTspice] a ¨¦crit?:
? |
|
Re: Pull-Push transformer for valve amp in LTspice
¿ªÔÆÌåÓýIndeed a dual primary xfmr can be created in LTspice.You need to include all windings in the K statement. There is a beautiful example of tube amp in the Files, in fact more than one: Fender Twin Reverb AB763 and Fender Twin Reverb AA270 Also Fisher500c and Laney_Marshall_EL34_50Watt Le 21/05/2014 15:32, Vlad
imbvlad@... [LTspice] a ¨¦crit?:
? |
|
Re: Pull-Push transformer for valve amp in LTspice
I don't know if it's possible to simulate a double-primary transformer in LTspice. At least not with inductors and coupling between them. Still, if others have different answers, it would be useful to follow the steps in the group's home page about asking for help, how to upload schematics and where. Vlad ______________________ -- holding, among others: a universal analog/digital filter, block-level models for power electronics (and not only), math blocks with a more stream-lined approach, some digital ADC, DAC, (synchronous-)counter, JKflop, etc. |
|
Pull-Push transformer for valve amp in LTspice
I am having trouble modelling an ideal Pull-Push center tap 8 ohms transformer with a 6.7k primary anode-anode impedance in LTspice.? |
to navigate to use esc to dismiss