"Jim Thompson" wrote in message news:oaj7o9tqh696a3lodtri7i5m3uov8o44va@4ax.com... On Mon, 26 May 2014 16:12:25 -0700, "garyr" <garyr@fidalgo.net> wrote:>[snip] >> >> You'll need to change library calls and create library for MyTL081 >> (unwrap as neessary)... >>>> C1 0 N2 {1/(2*PI*GBW*1E6)} >> C2 N4 N7 {sqrt(L)} ;1 >> L1 N7 N6 {sqrt(L)} ;{L}>I'm trying to establish myself in the business of creating behavioral >Spice models... models that work properly... _and_ match the real >device and the datasheet.Well, its a very good idea NOT to use inductors unless they are actually needed. They can cause convergence issues. Even in the expensive Cadence Spectre RF, I am currently having to put clamps across inductors for PSS simulations in order to get it them work. Inductors like to generate MVs whilst the answer is being iterated out. Kevin Aylward B.Sc. www.kevinaylward.co.uk www.anasoft.co.uk - SuperSpice
Headphone amp simulation
Started by ●May 26, 2014
Reply by ●May 27, 20142014-05-27
Reply by ●May 27, 20142014-05-27
On Tue, 27 May 2014 17:30:52 +0100, "Kevin Aylward" <ExtractkevinRemove@kevinaylward.co.uk> wrote:>"Jim Thompson" wrote in message >news:oaj7o9tqh696a3lodtri7i5m3uov8o44va@4ax.com... > >On Mon, 26 May 2014 16:12:25 -0700, "garyr" <garyr@fidalgo.net> wrote: > >>[snip] >>> >>> You'll need to change library calls and create library for MyTL081 >>> (unwrap as neessary)... >>> > >>> C1 0 N2 {1/(2*PI*GBW*1E6)} >>> C2 N4 N7 {sqrt(L)} ;1 >>> L1 N7 N6 {sqrt(L)} ;{L} > > >>I'm trying to establish myself in the business of creating behavioral >>Spice models... models that work properly... _and_ match the real >>device and the datasheet. > >Well, its a very good idea NOT to use inductors unless they are actually >needed. They can cause convergence issues. Even in the expensive Cadence >Spectre RF, I am currently having to put clamps across inductors for PSS >simulations in order to get it them work. Inductors like to generate MVs >whilst the answer is being iterated out. > > >Kevin Aylward B.Sc. >www.kevinaylward.co.uk >www.anasoft.co.uk - SuperSpiceThat's an all-pass to model the OpAmp excess phase... and it is low-Q, so I don't think it'll ever be an issue in this application. As for your inductor problems... you just need to use TANH >:-} ...Jim Thompson -- | James E.Thompson | mens | | Analog Innovations | et | | Analog/Mixed-Signal ASIC's and Discrete Systems | manus | | San Tan Valley, AZ 85142 Skype: skypeanalog | | | Voice:(480)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.
Reply by ●May 27, 20142014-05-27
"Jim Thompson" wrote in message news:6hf9o9tq1ojl91gs992a3vaha22muhpfuf@4ax.com... On Tue, 27 May 2014 17:30:52 +0100, "Kevin Aylward" <ExtractkevinRemove@kevinaylward.co.uk> wrote:>"Jim Thompson" wrote in message >news:oaj7o9tqh696a3lodtri7i5m3uov8o44va@4ax.com... > >On Mon, 26 May 2014 16:12:25 -0700, "garyr" <garyr@fidalgo.net> wrote: > >>[snip] >>> >>> You'll need to change library calls and create library for MyTL081 >>> (unwrap as neessary)... >>> > >>> C1 0 N2 {1/(2*PI*GBW*1E6)} >>> C2 N4 N7 {sqrt(L)} ;1 >>> L1 N7 N6 {sqrt(L)} ;{L} > > >>I'm trying to establish myself in the business of creating behavioral >>Spice models... models that work properly... _and_ match the real >>device and the datasheet. > >>Well, its a very good idea NOT to use inductors unless they are actually >>needed. They can cause convergence issues. Even in the expensive Cadence >>Spectre RF, I am currently having to put clamps across inductors for PSS >>simulations in order to get it them work. Inductors like to generate MVs >>whilst the answer is being iterated out. >>That's an all-pass to model the OpAmp excess phase... and it is low-Q, >so I don't think it'll ever be an issue in this application.Its one of those probability things. LC circuits like to ring. Just putting in one inductor can make the time steps multiply up to cause slower simulation. So, son, when you have the experience I have, you learn to look out for those little subtleties... Kevin Aylward B.Sc. www.kevinaylward.co.uk www.anasoft.co.uk - SuperSpice
Reply by ●May 27, 20142014-05-27
On Tue, 27 May 2014 20:57:01 +0100, "Kevin Aylward" <ExtractkevinRemove@kevinaylward.co.uk> wrote:>"Jim Thompson" wrote in message >news:6hf9o9tq1ojl91gs992a3vaha22muhpfuf@4ax.com... > >On Tue, 27 May 2014 17:30:52 +0100, "Kevin Aylward" ><ExtractkevinRemove@kevinaylward.co.uk> wrote: > >>"Jim Thompson" wrote in message >>news:oaj7o9tqh696a3lodtri7i5m3uov8o44va@4ax.com... >> >>On Mon, 26 May 2014 16:12:25 -0700, "garyr" <garyr@fidalgo.net> wrote: >> >>>[snip] >>>> >>>> You'll need to change library calls and create library for MyTL081 >>>> (unwrap as neessary)... >>>> >> >>>> C1 0 N2 {1/(2*PI*GBW*1E6)} >>>> C2 N4 N7 {sqrt(L)} ;1 >>>> L1 N7 N6 {sqrt(L)} ;{L} >> >> >>>I'm trying to establish myself in the business of creating behavioral >>>Spice models... models that work properly... _and_ match the real >>>device and the datasheet. >> >>>Well, its a very good idea NOT to use inductors unless they are actually >>>needed. They can cause convergence issues. Even in the expensive Cadence >>>Spectre RF, I am currently having to put clamps across inductors for PSS >>>simulations in order to get it them work. Inductors like to generate MVs >>>whilst the answer is being iterated out. >> > > >>That's an all-pass to model the OpAmp excess phase... and it is low-Q, >>so I don't think it'll ever be an issue in this application. > >Its one of those probability things. > >LC circuits like to ring. Just putting in one inductor can make the time >steps multiply up to cause slower simulation. So, son, when you have the >experience I have, you learn to look out for those little subtleties... > >Kevin Aylward B.Sc. >www.kevinaylward.co.uk >www.anasoft.co.uk - SuperSpiceSon? Unless you're 94+, there's no way "son" applies ;-) By low-Q, like Q~1, so I'm safe. Inductor in a switcher, that's another animal altogether. But I will take your advice and create a part "L-bounded", at-the-ready in case I have a problem >:-} ...Jim Thompson -- | James E.Thompson | mens | | Analog Innovations | et | | Analog/Mixed-Signal ASIC's and Discrete Systems | manus | | San Tan Valley, AZ 85142 Skype: skypeanalog | | | Voice:(480)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.
Reply by ●May 27, 20142014-05-27
On Mon, 26 May 2014 11:32:05 -0700, Jim Thompson <To-Email-Use-The-Envelope-Icon@On-My-Web-Site.com> wrote:> >>TEXT -536 496 Left 2 !.lib C:\\Program=20 >>Files\\LTC\\LTspiceIV\\lib\\mylib\\supertex.lib >>TEXT -536 464 Left 2 !.tran 0.1 startup uic >>TEXT -536 528 Left 2 !.include C:\\Program=20 >>Files\\LTC\\LTspiceIV\\lib\\mylib\\TL082.lib >> > >LTspice doesn't like those last "TEXT" lines, complaining of a syntax >problem. > >Anyone (everyone :-) more familiar with LTspice than me, how should >those library calls be corrected? > =09 > ...Jim ThompsonThe embedded spaces in the full path file names are causing problems. = They need to be placed in quote characters("). There may be other issues as well. ?-) =20
Reply by ●May 28, 20142014-05-28
"Jim Thompson" wrote in message news:u9s9o9hc78co0rd9r4k3bjjll2ts11170p@4ax.com... On Tue, 27 May 2014 20:57:01 +0100, "Kevin Aylward" <ExtractkevinRemove@kevinaylward.co.uk> wrote:>"Jim Thompson" wrote in message >news:6hf9o9tq1ojl91gs992a3vaha22muhpfuf@4ax.com... > >On Tue, 27 May 2014 17:30:52 +0100, "Kevin Aylward" ><ExtractkevinRemove@kevinaylward.co.uk> wrote: > >>"Jim Thompson" wrote in message >>news:oaj7o9tqh696a3lodtri7i5m3uov8o44va@4ax.com... >> >>On Mon, 26 May 2014 16:12:25 -0700, "garyr" <garyr@fidalgo.net> wrote: >> >>>[snip] >>>> >>>> You'll need to change library calls and create library for MyTL081 >>>> (unwrap as neessary)... >>>> >> >>>> C1 0 N2 {1/(2*PI*GBW*1E6)} >>>> C2 N4 N7 {sqrt(L)} ;1 >>>> L1 N7 N6 {sqrt(L)} ;{L} >> >> >>>I'm trying to establish myself in the business of creating behavioral >>>Spice models... models that work properly... _and_ match the real >>>device and the datasheet. >> >>>Well, its a very good idea NOT to use inductors unless they are actually >>>needed. They can cause convergence issues. Even in the expensive Cadence >>>Spectre RF, I am currently having to put clamps across inductors for PSS >>>simulations in order to get it them work. Inductors like to generate MVs >>>whilst the answer is being iterated out. >> > > >>That's an all-pass to model the OpAmp excess phase... and it is low-Q, >>so I don't think it'll ever be an issue in this application. > >Its one of those probability things. > >LC circuits like to ring. Just putting in one inductor can make the time >steps multiply up to cause slower simulation. So, son, when you have the >experience I have, you learn to look out for those little subtleties...>Son? Unless you're 94+, there's no way "son" applies ;-)>By low-Q, like Q~1, so I'm safe.>Inductor in a switcher, that's another animal altogether.>But I will take your advice and create a part "L-bounded", >at-the-ready in case I have a problem >:-}LTSpice should handle this potential issue no problem because it has inherent dampers in its two terminal, multi-element models for Ls and Cs. I am not aware of any other spice having such a facility. Cadence Spectre does not, and it is a major blemish for such a "high end" simulator. Kevin Aylward B.Sc. www.kevinaylward.co.uk www.anasoft.co.uk - SuperSpice
Reply by ●May 28, 20142014-05-28
On Wed, 28 May 2014 17:19:58 +0100, "Kevin Aylward" <ExtractkevinRemove@kevinaylward.co.uk> wrote:>"Jim Thompson" wrote in message >news:u9s9o9hc78co0rd9r4k3bjjll2ts11170p@4ax.com... > >On Tue, 27 May 2014 20:57:01 +0100, "Kevin Aylward" ><ExtractkevinRemove@kevinaylward.co.uk> wrote: > >>"Jim Thompson" wrote in message >>news:6hf9o9tq1ojl91gs992a3vaha22muhpfuf@4ax.com... >> >>On Tue, 27 May 2014 17:30:52 +0100, "Kevin Aylward" >><ExtractkevinRemove@kevinaylward.co.uk> wrote: >> >>>"Jim Thompson" wrote in message >>>news:oaj7o9tqh696a3lodtri7i5m3uov8o44va@4ax.com... >>> >>>On Mon, 26 May 2014 16:12:25 -0700, "garyr" <garyr@fidalgo.net> wrote: >>> >>>>[snip] >>>>> >>>>> You'll need to change library calls and create library for MyTL081 >>>>> (unwrap as neessary)... >>>>> >>> >>>>> C1 0 N2 {1/(2*PI*GBW*1E6)} >>>>> C2 N4 N7 {sqrt(L)} ;1 >>>>> L1 N7 N6 {sqrt(L)} ;{L} >>> >>> >>>>I'm trying to establish myself in the business of creating behavioral >>>>Spice models... models that work properly... _and_ match the real >>>>device and the datasheet. >>> >>>>Well, its a very good idea NOT to use inductors unless they are actually >>>>needed. They can cause convergence issues. Even in the expensive Cadence >>>>Spectre RF, I am currently having to put clamps across inductors for PSS >>>>simulations in order to get it them work. Inductors like to generate MVs >>>>whilst the answer is being iterated out. >>> >> >> >>>That's an all-pass to model the OpAmp excess phase... and it is low-Q, >>>so I don't think it'll ever be an issue in this application. >> >>Its one of those probability things. >> >>LC circuits like to ring. Just putting in one inductor can make the time >>steps multiply up to cause slower simulation. So, son, when you have the >>experience I have, you learn to look out for those little subtleties... > >>Son? Unless you're 94+, there's no way "son" applies ;-) > >>By low-Q, like Q~1, so I'm safe. > >>Inductor in a switcher, that's another animal altogether. > >>But I will take your advice and create a part "L-bounded", >>at-the-ready in case I have a problem >:-} > >LTSpice should handle this potential issue no problem because it has >inherent dampers in its two terminal, multi-element models for Ls and Cs. I >am not aware of any other spice having such a facility. Cadence Spectre does >not, and it is a major blemish for such a "high end" simulator. > > >Kevin Aylward B.Sc. >www.kevinaylward.co.uk >www.anasoft.co.uk - SuperSpiceI had occasion, the first three months of this year, to have to use my least favorite simulation tool, Cadence Virtuoso and derivatives... what a royal pile of CAD-doo-doo! How they get away with selling such an inadequate tool I'll never know... though I suspect they con _clueless_management_ into thinking that you need their whole CAD suite to properly design, layout and fab a chip... which is pure baloney... I have ~70 functioning chips, designed in PSpice (MicroSim) Schematics, then laid out with IC Editor... LVS is no sweat... I can match the layout netlist requirements of _any_ layout tool. Back to the inductor... a TANH G-source across the inductor with adjustable voltage limits (in both directions) should do the trick ;-) ...Jim Thompson -- | James E.Thompson | mens | | Analog Innovations | et | | Analog/Mixed-Signal ASIC's and Discrete Systems | manus | | San Tan Valley, AZ 85142 Skype: skypeanalog | | | Voice:(480)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.
Reply by ●May 29, 20142014-05-29
>"Jim Thompson" wrote in message >news:086co9dl2abi3p7tb0cl60eaoebsudgtdd@4ax.com...> >>LTSpice should handle this potential issue no problem because it has >>inherent dampers in its two terminal, multi-element models for Ls and Cs. >>I >>am not aware of any other spice having such a facility. Cadence Spectre >>does >>not, and it is a major blemish for such a "high end" simulator. > >>I had occasion, the first three months of this year, to have to use my >least favorite simulation tool, Cadence Virtuoso and derivatives... >what a royal pile of CAD-doo-doo!>How they get away with selling such an inadequate tool I'll never >know... though I suspect they con _clueless_management_ into thinking >that you need their whole CAD suite to properly design, layout and fab >a chip... which is pure baloney... I have ~70 functioning chips, >designed in PSpice (MicroSim) Schematics, then laid out with IC >Editor... LVS is no sweat... I can match the layout netlist >requirements of _any_ layout tool.Well... I am still a huge supporter of Cadence and its whole tool flow, despite its blemishes. I wouldn't want to use anything else. Its environment and facilities are still orders above PSpice. There is just so much you can do that just isn't in the more "schoolboy" tools. I don't consider PSpice a professional level ASIC design tool, despite someone's ability to work around its deficiencies for ASIC design. I don't agree that management is conned. I had to personally fight very hard when I started my current job to get Simetrix ditched and Cadence brought in. Its a no contest.>Back to the inductor... a TANH G-source across the inductor with >adjustable voltage limits (in both directions) should do the trick ;-)Note that even 100 Mohms across the inductance of a xtal can kill its oscillation. Kevin Aylward B.Sc. www.kevinaylward.co.uk www.anasoft.co.uk - SuperSpice
Reply by ●May 29, 20142014-05-29
On Thu, 29 May 2014 09:24:24 +0100, "Kevin Aylward" <ExtractkevinRemove@kevinaylward.co.uk> wrote:>>"Jim Thompson" wrote in message >>news:086co9dl2abi3p7tb0cl60eaoebsudgtdd@4ax.com... > >> >>>LTSpice should handle this potential issue no problem because it has >>>inherent dampers in its two terminal, multi-element models for Ls and Cs. >>>I >>>am not aware of any other spice having such a facility. Cadence Spectre >>>does >>>not, and it is a major blemish for such a "high end" simulator. >> >> > >>I had occasion, the first three months of this year, to have to use my >>least favorite simulation tool, Cadence Virtuoso and derivatives... >>what a royal pile of CAD-doo-doo! > >>How they get away with selling such an inadequate tool I'll never >>know... though I suspect they con _clueless_management_ into thinking >>that you need their whole CAD suite to properly design, layout and fab >>a chip... which is pure baloney... I have ~70 functioning chips, >>designed in PSpice (MicroSim) Schematics, then laid out with IC >>Editor... LVS is no sweat... I can match the layout netlist >>requirements of _any_ layout tool. > >Well... I am still a huge supporter of Cadence and its whole tool flow, >despite its blemishes. I wouldn't want to use anything else. Its environment >and facilities are still orders above PSpice. There is just so much you can >do that just isn't in the more "schoolboy" tools.Name something Cadence can do that I can't with PSpice (other than PSpice doesn't do layout >:-}>I don't consider PSpice a >professional level ASIC design tool, despite someone's ability to work >around its deficiencies for ASIC design.Name a deficiency. [Keep in mind that I am definitely yanking your chain... over the years I've written many "scripts" (Algebraic mostly, some IF,THEN,ELSE) so that I can even do binning automatically in PSpice :-]> >I don't agree that management is conned. I had to personally fight very hard >when I started my current job to get Simetrix ditched and Cadence brought >in. Its a no contest. > >>Back to the inductor... a TANH G-source across the inductor with >>adjustable voltage limits (in both directions) should do the trick ;-) > >Note that even 100 Mohms across the inductance of a xtal can kill its >oscillation.I've not had any run-away inductors, so I think it must be a Cadence issue.> >Kevin Aylward B.Sc. >www.kevinaylward.co.uk >www.anasoft.co.uk - SuperSpice...Jim Thompson -- | James E.Thompson | mens | | Analog Innovations | et | | Analog/Mixed-Signal ASIC's and Discrete Systems | manus | | San Tan Valley, AZ 85142 Skype: skypeanalog | | | Voice:(480)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.
Reply by ●May 29, 20142014-05-29
"Jim Thompson" wrote in message news:gcjeo91mdnisd7a0a0cpaa67c2t2vlbuub@4ax.com... On Thu, 29 May 2014 09:24:24 +0100, "Kevin Aylward" <ExtractkevinRemove@kevinaylward.co.uk> wrote:>>"Jim Thompson" wrote in message >>news:086co9dl2abi3p7tb0cl60eaoebsudgtdd@4ax.com... > >> >>>LTSpice should handle this potential issue no problem because it has >>>inherent dampers in its two terminal, multi-element models for Ls and Cs. >>>I >>>am not aware of any other spice having such a facility. Cadence Spectre >>>does >>>not, and it is a major blemish for such a "high end" simulator. >> >> > >>I had occasion, the first three months of this year, to have to use my >>least favorite simulation tool, Cadence Virtuoso and derivatives... >>what a royal pile of CAD-doo-doo! > >>>How they get away with selling such an inadequate tool I'll never >>>know... though I suspect they con _clueless_management_ into thinking >>>that you need their whole CAD suite to properly design, layout and fab >>>a chip... which is pure baloney... I have ~70 functioning chips, >>>designed in PSpice (MicroSim) Schematics, then laid out with IC >>>Editor... LVS is no sweat... I can match the layout netlist >>>requirements of _any_ layout tool. > >>Well... I am still a huge supporter of Cadence and its whole tool flow, >>despite its blemishes. I wouldn't want to use anything else. Its >>environment >>and facilities are still orders above PSpice. There is just so much you >>can >>do that just isn't in the more "schoolboy" tools.>Name something Cadence can do that I can't with PSpice (other than >PSpice doesn't do layout >:-}>>I don't consider PSpice a >>professional level ASIC design tool, despite someone's ability to work >>around its deficiencies for ASIC design.>Name a deficiency.Well, for one its a bloody 1G download, which I have just done to see whether or not my considerations are valid. I haven't use PSpice for over 10 years. I will give it a look over. It doesn't look like it can install in Program Files. I pressed the install, and now notice it installed in C:\ This is pretty much unacceptable for seconds. Assuming, as it looks, that everything is installed there, and that only one of those files gets modified by the program, it wont run as it should if installed in program files. Does it have an equivalent to Cadences "view switch"? That is, the ability to to switch with one change what set of schematics is actually attached to their symbols? Spent 15 mins so far, and cant even get an example schematic displayed.>Note that even 100 Mohms across the inductance of a xtal can kill its >oscillation.>I've not had any run-away inductors, so I think it must be a Cadence >issue.This is a physical reality issue. XTAL oscillator wont oscillate if damping resistance is "significant". A c1 of 10ff @ 50Mhz is an inductance of 1mH, which is an impedance of 300k. So care need to be taken on any clamps. Kevin Aylward B.Sc. kevin@kevinaylward.co.uk www.kevinaylward.co.uk
