sci.electronics.design | LTSpice UI| page 4

Reply by Clive Arthur ●March 7, 20232023-03-07

On 07/03/2023 15:18, Phil Hobbs wrote:
> On 2023-03-07 05:54, Clive Arthur wrote:> On 02/03/2023 23:25, Ricky wrote:

<snip>

>  > LTspice XVII
>  >
>  > If you have a group of .params, eg...
>  >
>  > .param Rlim 75 .param Clift 10n .param Cbp 180p
>  >
>  > ...and you right click on one of them on the schematic, edit its
>  > value and click 'ok', then nothing happens.
> 
> Works fine for me--I just type <enter> when I'm done, and it remembers.

So it does!  It's the OK which doesn't work, thanks.

-- 
Cheers
Clive

Reply by John Larkin ●March 7, 20232023-03-07

On Tue, 7 Mar 2023 10:18:44 -0500, Phil Hobbs
<pcdhSpamMeSenseless@electrooptical.net> wrote:

>On 2023-03-07 05:54, Clive Arthur wrote:> On 02/03/2023 23:25, Ricky wrote:
> >> Is there anyone here who thinks LTspice has a good UI?
> >>
> >> I've been working with it for a week or so, after not using for
> >> over a year.  It's very hard to reacclimate to the zoom in and out
> >> being backwards from every UI I know under Windows.  The Function
> >> keys will become familiar again, if I continue using it, but what
> >> an uphill climb.
> >>
> >> I saw in an LTspice post that Mike E. is writing a new simulator.
> >> I hope he makes it compatible with the existing models.  But I
> >> suppose he would not be able to work with the company models that
> >> don't have accessible contents.  I'm wondering how useful it will
> >> be to the engineering community as a whole.  There are lots of
> >> models you just can't get other than as locked by ADI.  I think TI
> >> has given up on the idea of TINA being their goto simulator.
> >> LTspice just has too much steam on the boiler.
> >>
> >
> > LTspice XVII
> >
> > If you have a group of .params, eg...
> >
> > .param Rlim 75 .param Clift 10n .param Cbp 180p
> >
> > ...and you right click on one of them on the schematic, edit its
> > value and click 'ok', then nothing happens.
>
>Works fine for me--I just type <enter> when I'm done, and it remembers.
>
>They did make it harder to avoid the specialized edit dialogs in XVII--I 
>just put stuff in multi-line directive groups,  e.g.
>
>; SIMULATION COMMAND
>; .tran 100u
>.ac oct 100 10 1g
>
>
>; PARAMETERS
>.param Ree 2
>.step param Ree list 1 2 5
>
>You double-click on the heading, and a normal OS dialog box comes up 
>that you type into as usual.  in wine you have to use <ctrl><enter> to 
>get a new line, not <ctl>M, but that's the only difference I notice.
>
>I generally like XVII--for instance, there are some improvements in 
>dealing with crappy models such as TI's.  In early versions, and in IV, 
>the OPA140 model would fail to converge unless the supplies were 
>-exactly- symmetric, and often not even then.
>
>The current version handles the exact same OPA140 model just fine, 
>probably on account of some workaround for all the sharp corners and 
>discontinuities in the TI model.
>
> > Instead, you have to right click, then click 'cancel', then edit from
> > the list and press 'ok'.  A bit annoying, but other than that the UI
> > works ok once you've defined your keys to do more 'sensible' things.
> > (M for move, R for rotate, Ctrl-C for copy etc)
>
>Sure, and f5 for "run simulation".  Makes it more like Visual Studio. 
>LTspice gets credit for making that pretty easy.
>
> > Oh - copy and paste on a transformer changes the annotation for the
> > windings, but not for the coupling coefficient.
>
>Ain't no such thing as a transformer in my LTspice--dunno about yours. 
>Just individual inductors with coupling coefficients.  If you copy and 
>paste, you have to specify the coupling between the two new inductors.

Copy and paste preserves node names too, which can create interesting
long-distance shorts.

>
>There's no way I can think of to automate that in a useful fashion--do 
>you want it to guess, based on the way the inductors are arranged on the 
>schematic?  Not for me, thanks--that's definitely your pistol-shoehorn 
>combination, right there.
>
>Cheers
>
>Phil Hobbs

Last time I checked, it still entangles parameters between transient
and frequency analysis, hence the need to mess with semicolons to
switch sim mode. Version IV switched modes properly.

Reply by Clive Arthur ●March 7, 20232023-03-07

On 07/03/2023 15:52, John Larkin wrote:

<snip>

> 
> Last time I checked, [LTspice XVII] still entangles parameters between transient
> and frequency analysis, hence the need to mess with semicolons to
> switch sim mode. Version IV switched modes properly.
> 

Ah yes, forgot that one.

-- 
Cheers
Clive

Reply by Phil Hobbs ●March 7, 20232023-03-07

On 2023-03-07 10:47, Clive Arthur wrote:
> On 07/03/2023 15:18, Phil Hobbs wrote:
>> On 2023-03-07 05:54, Clive Arthur wrote:> On 02/03/2023 23:25, Ricky 
>> wrote:
> 
> <snip>
>>
>> &nbsp;> Oh - copy and paste on a transformer changes the annotation for the
>> &nbsp;> windings, but not for the coupling coefficient.
>>
>> Ain't no such thing as a transformer in my LTspice--dunno about yours. 
>> Just individual inductors with coupling coefficients.&nbsp; If you copy and 
>> paste, you have to specify the coupling between the two new inductors.
>>
>> There's no way I can think of to automate that in a useful fashion--do 
>> you want it to guess, based on the way the inductors are arranged on 
>> the schematic?&nbsp; Not for me, thanks--that's definitely your 
>> pistol-shoehorn combination, right there.
>>
>> Cheers
>>
>> Phil Hobbs
>>
>>
> Yeah, I guess it would be tricky.&nbsp; I always draw my transformers with 
> the K..... between the windings as if it were the core (it looks kewl!), 
> so copying as one 'box' might give me unrealistic expectations that the 
> coupling annotations should change too.

Ah, okay, it's vitally important to be cooler than your CAD software, 
for sure. ;)

> Another useful thing would be to temporarily lock the scaling on the 
> plot screen, so you can zoom in, lock it, change something and run 
> again.&nbsp; (Or maybe there is a way?)
> 

Agreed--the autoscaling on the plots is fascism at its best. ;)

One approach is to plot not v(out) but min(high, max(low, v(out)) ).

On the X axis you can tell the sim to start storing data at some time 
t_start instead of t = 0.

A recurring beef of mine is that the plot window code is stupid about 
units--you have to use (1V/1A) a lot instead of 1ohm, for instance.  In 
noise plots, when inoise is a current, you often you want to check the 
input-referred noise due to some part on the schematic.

"No worries", you say, "I'll just divide by the built-in variable 
'gain'".  Then you find that you have two vertical scales, one in 
A/sqrt(Hz) and the other in V/(ohm sqrt(Hz)).  To get one scale, you 
have to multiply by 'inoise/v(onoise)'.

That's a pain when building TIAs.

Cheers

Phil Hobbs

-- 
Dr Philip C D Hobbs
Principal Consultant
ElectroOptical Innovations LLC / Hobbs ElectroOptics
Optics, Electro-optics, Photonics, Analog Electronics
Briarcliff Manor NY 10510

http://electrooptical.net
http://hobbs-eo.com

Reply by Phil Hobbs ●March 7, 20232023-03-07

On 2023-03-07 10:52, John Larkin wrote:
 > On Tue, 7 Mar 2023 10:18:44 -0500, Phil Hobbs
> <pcdhSpamMeSenseless@electrooptical.net> wrote:
> 
>> On 2023-03-07 05:54, Clive Arthur wrote:> On 02/03/2023 23:25, 
>> Ricky wrote:
>>>> Is there anyone here who thinks LTspice has a good UI?
<snip>

>>> the windings, but not for the coupling coefficient.
>> 
>> Ain't no such thing as a transformer in my LTspice--dunno about 
>> yours. Just individual inductors with coupling coefficients.  If 
>> you copy and paste, you have to specify the coupling between the 
>> two new inductors.
> 
> Copy and paste preserves node names too, which can create interesting
> long-distance shorts.

Yeah.  Of course Diptrace will do that on your circuit board too, and
screw up all the board traces besides. :(

(We switched to Kicad 7.  It's actually a professional EDA tool now.)

>> 
>> There's no way I can think of to automate that in a useful 
>> fashion--do you want it to guess, based on the way the inductors 
>> are arranged on the schematic?  Not for me, thanks--that's 
>> definitely your pistol-shoehorn combination, right there.

> Last time I checked, it still entangles parameters between transient 
> and frequency analysis, hence the need to mess with semicolons to 
> switch sim mode. Version IV switched modes properly.

Yup.  I used the semicolons in IV as well, though, because the dialog
box contents aren't preserved when the program exits.

Cheers

Phil Hobbs



-- 
Dr Philip C D Hobbs
Principal Consultant
ElectroOptical Innovations LLC / Hobbs ElectroOptics
Optics, Electro-optics, Photonics, Analog Electronics
Briarcliff Manor NY 10510

http://electrooptical.net
http://hobbs-eo.com