On Mon, 10 Aug 2015 16:33:29 -0400, Phil Hobbs <pcdhSpamMeSenseless@electrooptical.net> wrote:>On 08/10/2015 04:22 PM, George Herold wrote: >> On Sunday, August 9, 2015 at 7:25:05 PM UTC-4, Phil Hobbs wrote: >>> Hi, Jim, >>> >>> If you've got some spare bandwidth, I could really use an improved >>> OPA2140 model. >>> >>> It's a very good part for moderate speed, low current, high >>> linearity TIAs, but it's a bear to simulate because the model won't >>> converge on an operating point in LTspice. >>> >>> I took the TINA model TI supplies and replaced the VSWITCH cards >>> with LTspice SW cards with negative hysteresis (more or less like >>> your fave tanh curve), but it still won't converge on ac or noise >>> sims. >>> >>> Thanks >>> >>> Phil Hobbs >> >> Hey that is a nice opamp. I'll get some and try them in a PD >> circuit. It currently uses an opa124, which looks OK (well slow) but >> has a nasty noise peak out at 20 kHz (or so). >> >> George H. >> > >OPA140s are great. Sort of an OPA111 on steroids, with nice low noise >levels. In LTspice I discover that you have to minutely adjust the >supplies so that the inputs are right in the middle, at which point >it'll find an operating point. > >Ramping up the supplies from zero works okay in a transient simulation. > It's a pity you can't just take a snapshot of the voltages and >currents in a circuit and say "Start here next time". That way we could >use the .TRAN tricks for getting circuits started, and save the results >for .AC and .NOISE. > >Cheers > >Phil HobbsYou can do that with PSpice: Save Bias Point / Load Bias Point. Save from a .TRAN, Load to a .AC I thought LTspice could do that as well ?? ...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.
AN: TL598 Spice Model
Started by ●August 9, 2015
Reply by ●August 10, 20152015-08-10
Reply by ●August 10, 20152015-08-10
On 8/10/2015 5:35 PM, Jim Thompson wrote:> On Mon, 10 Aug 2015 16:33:29 -0400, Phil Hobbs > <pcdhSpamMeSenseless@electrooptical.net> wrote: > >> On 08/10/2015 04:22 PM, George Herold wrote: >>> On Sunday, August 9, 2015 at 7:25:05 PM UTC-4, Phil Hobbs wrote: >>>> Hi, Jim, >>>> >>>> If you've got some spare bandwidth, I could really use an >>>> improved OPA2140 model. >>>> >>>> It's a very good part for moderate speed, low current, high >>>> linearity TIAs, but it's a bear to simulate because the model >>>> won't converge on an operating point in LTspice. >>>> >>>> I took the TINA model TI supplies and replaced the VSWITCH >>>> cards with LTspice SW cards with negative hysteresis (more or >>>> less like your fave tanh curve), but it still won't converge on >>>> ac or noise sims. >>>> >>>> Thanks >>>> >>>> Phil Hobbs >>> >>> Hey that is a nice opamp. I'll get some and try them in a PD >>> circuit. It currently uses an opa124, which looks OK (well slow) >>> but has a nasty noise peak out at 20 kHz (or so). >>> >>> George H. >>> >> >> OPA140s are great. Sort of an OPA111 on steroids, with nice low >> noise levels. In LTspice I discover that you have to minutely >> adjust the supplies so that the inputs are right in the middle, at >> which point it'll find an operating point. >> >> Ramping up the supplies from zero works okay in a transient >> simulation. It's a pity you can't just take a snapshot of the >> voltages and currents in a circuit and say "Start here next time". >> That way we could use the .TRAN tricks for getting circuits >> started, and save the results for .AC and .NOISE. >> >> Cheers >> >> Phil Hobbs > > You can do that with PSpice: Save Bias Point / Load Bias Point. > > Save from a .TRAN, Load to a .AC > > I thought LTspice could do that as well ?? ...Jim Thompson >There's .savebias / .loadbias, but they're not the same thing. It iterates to a bias point (hopefully) and then saves that, not the results of the transient. Cheers Phil Hobbs -- Dr Philip C D Hobbs Principal Consultant ElectroOptical Innovations LLC Optics, Electro-optics, Photonics, Analog Electronics 160 North State Road #203 Briarcliff Manor NY 10510 hobbs at electrooptical dot net http://electrooptical.net
Reply by ●August 10, 20152015-08-10
On Mon, 10 Aug 2015 17:44:14 -0400, Phil Hobbs <pcdhSpamMeSenseless@electrooptical.net> wrote:>On 8/10/2015 5:35 PM, Jim Thompson wrote: >> On Mon, 10 Aug 2015 16:33:29 -0400, Phil Hobbs >> <pcdhSpamMeSenseless@electrooptical.net> wrote: >> >>> On 08/10/2015 04:22 PM, George Herold wrote: >>>> On Sunday, August 9, 2015 at 7:25:05 PM UTC-4, Phil Hobbs wrote: >>>>> Hi, Jim, >>>>> >>>>> If you've got some spare bandwidth, I could really use an >>>>> improved OPA2140 model. >>>>> >>>>> It's a very good part for moderate speed, low current, high >>>>> linearity TIAs, but it's a bear to simulate because the model >>>>> won't converge on an operating point in LTspice. >>>>> >>>>> I took the TINA model TI supplies and replaced the VSWITCH >>>>> cards with LTspice SW cards with negative hysteresis (more or >>>>> less like your fave tanh curve), but it still won't converge on >>>>> ac or noise sims. >>>>> >>>>> Thanks >>>>> >>>>> Phil Hobbs >>>> >>>> Hey that is a nice opamp. I'll get some and try them in a PD >>>> circuit. It currently uses an opa124, which looks OK (well slow) >>>> but has a nasty noise peak out at 20 kHz (or so). >>>> >>>> George H. >>>> >>> >>> OPA140s are great. Sort of an OPA111 on steroids, with nice low >>> noise levels. In LTspice I discover that you have to minutely >>> adjust the supplies so that the inputs are right in the middle, at >>> which point it'll find an operating point. >>> >>> Ramping up the supplies from zero works okay in a transient >>> simulation. It's a pity you can't just take a snapshot of the >>> voltages and currents in a circuit and say "Start here next time". >>> That way we could use the .TRAN tricks for getting circuits >>> started, and save the results for .AC and .NOISE. >>> >>> Cheers >>> >>> Phil Hobbs >> >> You can do that with PSpice: Save Bias Point / Load Bias Point. >> >> Save from a .TRAN, Load to a .AC >> >> I thought LTspice could do that as well ?? ...Jim Thompson >> > >There's .savebias / .loadbias, but they're not the same thing. > >It iterates to a bias point (hopefully) and then saves that, not the >results of the transient. > >Cheers > >Phil HobbsIn PSpice, do a .OP, SaveBias (to a file) Setup .TRAN, LoadBias (that file you saved), run .TRAN ...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 ●August 10, 20152015-08-10
On Sun, 9 Aug 2015 16:24:53 -0700 (PDT), Phil Hobbs <pcdhobbs@gmail.com> wrote:>Hi, Jim, > >If you've got some spare bandwidth, I could really use an improved OPA2140 model. > >It's a very good part for moderate speed, low current, high linearity TIAs, but it's a bear to simulate because the model won't converge on an operating point in LTspice. > > I took the TINA model TI supplies and replaced the VSWITCH cards with LTspice SW cards with negative hysteresis (more or less like your fave tanh curve), but it still won't converge on ac or noise sims. > >Thanks > >Phil HobbsHow do you set the parameters of the SW in LTspice? ...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 ●August 10, 20152015-08-10
On 8/10/2015 9:04 PM, Jim Thompson wrote:> On Sun, 9 Aug 2015 16:24:53 -0700 (PDT), Phil Hobbs > <pcdhobbs@gmail.com> wrote: > >> Hi, Jim, >> >> If you've got some spare bandwidth, I could really use an improved >> OPA2140 model. >> >> It's a very good part for moderate speed, low current, high >> linearity TIAs, but it's a bear to simulate because the model won't >> converge on an operating point in LTspice. >> >> I took the TINA model TI supplies and replaced the VSWITCH cards >> with LTspice SW cards with negative hysteresis (more or less like >> your fave tanh curve), but it still won't converge on ac or noise >> sims. >> >> Thanks >> >> Phil Hobbs > > How do you set the parameters of the SW in LTspice? ...Jim Thompson >RON, ROFF, which do what you'd expect; VT, which is the switching threshold (the switch looks like RON for V > VT, and ROFF for V < VT); and VH, the hysteresis. If VH is positive, then the upward-going transition occurs at V = VT + VH and the downward-going one at V = VT - VH. (IOW it does what you expect except that VH is the half-width of the deadband, not the full width.) Negative values of VH cause a smooth transition between RON and ROFF, so that the switching begins at VT + VH (which is less than VT in this case) and is complete at VT - VH (which is more than VT). IIRC the function is some smooth polynomial approximation to the arctan, so at least the first few derivatives are continuous. Cheers Phil Hobbs -- Dr Philip C D Hobbs Principal Consultant ElectroOptical Innovations LLC Optics, Electro-optics, Photonics, Analog Electronics 160 North State Road #203 Briarcliff Manor NY 10510 hobbs at electrooptical dot net http://electrooptical.net
Reply by ●August 10, 20152015-08-10
On Mon, 10 Aug 2015 21:11:51 -0400, Phil Hobbs <hobbs@electrooptical.net> wrote:>On 8/10/2015 9:04 PM, Jim Thompson wrote: >> On Sun, 9 Aug 2015 16:24:53 -0700 (PDT), Phil Hobbs >> <pcdhobbs@gmail.com> wrote: >> >>> Hi, Jim, >>> >>> If you've got some spare bandwidth, I could really use an improved >>> OPA2140 model. >>> >>> It's a very good part for moderate speed, low current, high >>> linearity TIAs, but it's a bear to simulate because the model won't >>> converge on an operating point in LTspice. >>> >>> I took the TINA model TI supplies and replaced the VSWITCH cards >>> with LTspice SW cards with negative hysteresis (more or less like >>> your fave tanh curve), but it still won't converge on ac or noise >>> sims. >>> >>> Thanks >>> >>> Phil Hobbs >> >> How do you set the parameters of the SW in LTspice? ...Jim Thompson >> > >RON, ROFF, which do what you'd expect; >VT, which is the switching threshold (the switch looks like RON for V > >VT, and ROFF for V < VT); >and VH, the hysteresis. > >If VH is positive, then the upward-going transition occurs at V = VT + >VH and the downward-going one at V = VT - VH. (IOW it does what you >expect except that VH is the half-width of the deadband, not the full >width.) > >Negative values of VH cause a smooth transition between RON and ROFF, so >that the switching begins at VT + VH (which is less than VT in this >case) and is complete at VT - VH (which is more than VT). IIRC the >function is some smooth polynomial approximation to the arctan, so at >least the first few derivatives are continuous. > >Cheers > >Phil HobbsI'm used to PSpice, click on a symbol and you see a table where you fill in the blanks. I click on SW in LTspice, I see several blank lines... SpiceLine SpicelIne2 Where do I enter Ron, Roff, Von, Voff, etc? ...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 ●August 10, 20152015-08-10
On 8/10/2015 10:18 PM, Jim Thompson wrote:> On Mon, 10 Aug 2015 21:11:51 -0400, Phil Hobbs > <hobbs@electrooptical.net> wrote: > >> On 8/10/2015 9:04 PM, Jim Thompson wrote: >>> On Sun, 9 Aug 2015 16:24:53 -0700 (PDT), Phil Hobbs >>> <pcdhobbs@gmail.com> wrote: >>> >>>> Hi, Jim, >>>> >>>> If you've got some spare bandwidth, I could really use an improved >>>> OPA2140 model. >>>> >>>> It's a very good part for moderate speed, low current, high >>>> linearity TIAs, but it's a bear to simulate because the model won't >>>> converge on an operating point in LTspice. >>>> >>>> I took the TINA model TI supplies and replaced the VSWITCH cards >>>> with LTspice SW cards with negative hysteresis (more or less like >>>> your fave tanh curve), but it still won't converge on ac or noise >>>> sims. >>>> >>>> Thanks >>>> >>>> Phil Hobbs >>> >>> How do you set the parameters of the SW in LTspice? ...Jim Thompson >>> >> >> RON, ROFF, which do what you'd expect; >> VT, which is the switching threshold (the switch looks like RON for V > >> VT, and ROFF for V < VT); >> and VH, the hysteresis. >> >> If VH is positive, then the upward-going transition occurs at V = VT + >> VH and the downward-going one at V = VT - VH. (IOW it does what you >> expect except that VH is the half-width of the deadband, not the full >> width.) >> >> Negative values of VH cause a smooth transition between RON and ROFF, so >> that the switching begins at VT + VH (which is less than VT in this >> case) and is complete at VT - VH (which is more than VT). IIRC the >> function is some smooth polynomial approximation to the arctan, so at >> least the first few derivatives are continuous. >> >> Cheers >> >> Phil Hobbs > > I'm used to PSpice, click on a symbol and you see a table where you > fill in the blanks. I click on SW in LTspice, I see several blank > lines... > > SpiceLine > SpicelIne2 > > Where do I enter Ron, Roff, Von, Voff, etc? > > ...Jim Thompson >You have to put in a .model statement: .model simplesw sw(Vt=1 Vh=-.5 Ron=1 Roff=1T) and put 'simplesw' on the 'value' line in the dialogue box. To make a NC switch, you can interchange the values of Ron and Roff, i.e. .model simpleNC sw(Vt=1 Vh=-.5 Ron=1T Roff=1) Cheers Phil Hobbs -- Dr Philip C D Hobbs Principal Consultant ElectroOptical Innovations LLC Optics, Electro-optics, Photonics, Analog Electronics 160 North State Road #203 Briarcliff Manor NY 10510 hobbs at electrooptical dot net http://electrooptical.net
Reply by ●August 11, 20152015-08-11
On Mon, 10 Aug 2015 22:37:04 -0400, Phil Hobbs <pcdhSpamMeSenseless@electrooptical.net> wrote:>On 8/10/2015 10:18 PM, Jim Thompson wrote: >> On Mon, 10 Aug 2015 21:11:51 -0400, Phil Hobbs >> <hobbs@electrooptical.net> wrote: >> >>> On 8/10/2015 9:04 PM, Jim Thompson wrote: >>>> On Sun, 9 Aug 2015 16:24:53 -0700 (PDT), Phil Hobbs >>>> <pcdhobbs@gmail.com> wrote: >>>> >>>>> Hi, Jim, >>>>> >>>>> If you've got some spare bandwidth, I could really use an improved >>>>> OPA2140 model. >>>>> >>>>> It's a very good part for moderate speed, low current, high >>>>> linearity TIAs, but it's a bear to simulate because the model won't >>>>> converge on an operating point in LTspice. >>>>> >>>>> I took the TINA model TI supplies and replaced the VSWITCH cards >>>>> with LTspice SW cards with negative hysteresis (more or less like >>>>> your fave tanh curve), but it still won't converge on ac or noise >>>>> sims. >>>>> >>>>> Thanks >>>>> >>>>> Phil Hobbs >>>> >>>> How do you set the parameters of the SW in LTspice? ...Jim Thompson >>>> >>> >>> RON, ROFF, which do what you'd expect; >>> VT, which is the switching threshold (the switch looks like RON for V > >>> VT, and ROFF for V < VT); >>> and VH, the hysteresis. >>> >>> If VH is positive, then the upward-going transition occurs at V = VT + >>> VH and the downward-going one at V = VT - VH. (IOW it does what you >>> expect except that VH is the half-width of the deadband, not the full >>> width.) >>> >>> Negative values of VH cause a smooth transition between RON and ROFF, so >>> that the switching begins at VT + VH (which is less than VT in this >>> case) and is complete at VT - VH (which is more than VT). IIRC the >>> function is some smooth polynomial approximation to the arctan, so at >>> least the first few derivatives are continuous. >>> >>> Cheers >>> >>> Phil Hobbs >> >> I'm used to PSpice, click on a symbol and you see a table where you >> fill in the blanks. I click on SW in LTspice, I see several blank >> lines... >> >> SpiceLine >> SpicelIne2 >> >> Where do I enter Ron, Roff, Von, Voff, etc? >> >> ...Jim Thompson >> >You have to put in a .model statement: > >.model simplesw sw(Vt=1 Vh=-.5 Ron=1 Roff=1T) > >and put 'simplesw' on the 'value' line in the dialogue box. > >To make a NC switch, you can interchange the values of Ron and Roff, i.e. > >.model simpleNC sw(Vt=1 Vh=-.5 Ron=1T Roff=1) > >Cheers > >Phil HobbsChecked it out, LTspice switch with negative hysteresis looks exactly same V-I curve as in PSpice... PSpice runs the OPA2140, LTspice will not, so it looks like a major makeover. If you need only GBW and noise, that can be done simply, otherwise the long winter ;-) <http://www.analog-innovations.com/SED/OP2140_JT_2015-08-11_07-39-39.jpg> ...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 ●August 11, 20152015-08-11
On Tue, 11 Aug 2015 07:45:28 -0700, Jim Thompson <To-Email-Use-The-Envelope-Icon@On-My-Web-Site.com> wrote:>On Mon, 10 Aug 2015 22:37:04 -0400, Phil Hobbs ><pcdhSpamMeSenseless@electrooptical.net> wrote: > >>On 8/10/2015 10:18 PM, Jim Thompson wrote: >>> On Mon, 10 Aug 2015 21:11:51 -0400, Phil Hobbs >>> <hobbs@electrooptical.net> wrote: >>> >>>> On 8/10/2015 9:04 PM, Jim Thompson wrote: >>>>> On Sun, 9 Aug 2015 16:24:53 -0700 (PDT), Phil Hobbs >>>>> <pcdhobbs@gmail.com> wrote: >>>>> >>>>>> Hi, Jim, >>>>>> >>>>>> If you've got some spare bandwidth, I could really use an improved >>>>>> OPA2140 model. >>>>>> >>>>>> It's a very good part for moderate speed, low current, high >>>>>> linearity TIAs, but it's a bear to simulate because the model won't >>>>>> converge on an operating point in LTspice. >>>>>> >>>>>> I took the TINA model TI supplies and replaced the VSWITCH cards >>>>>> with LTspice SW cards with negative hysteresis (more or less like >>>>>> your fave tanh curve), but it still won't converge on ac or noise >>>>>> sims. >>>>>> >>>>>> Thanks >>>>>> >>>>>> Phil Hobbs >>>>> >>>>> How do you set the parameters of the SW in LTspice? ...Jim Thompson >>>>> >>>> >>>> RON, ROFF, which do what you'd expect; >>>> VT, which is the switching threshold (the switch looks like RON for V > >>>> VT, and ROFF for V < VT); >>>> and VH, the hysteresis. >>>> >>>> If VH is positive, then the upward-going transition occurs at V = VT + >>>> VH and the downward-going one at V = VT - VH. (IOW it does what you >>>> expect except that VH is the half-width of the deadband, not the full >>>> width.) >>>> >>>> Negative values of VH cause a smooth transition between RON and ROFF, so >>>> that the switching begins at VT + VH (which is less than VT in this >>>> case) and is complete at VT - VH (which is more than VT). IIRC the >>>> function is some smooth polynomial approximation to the arctan, so at >>>> least the first few derivatives are continuous. >>>> >>>> Cheers >>>> >>>> Phil Hobbs >>> >>> I'm used to PSpice, click on a symbol and you see a table where you >>> fill in the blanks. I click on SW in LTspice, I see several blank >>> lines... >>> >>> SpiceLine >>> SpicelIne2 >>> >>> Where do I enter Ron, Roff, Von, Voff, etc? >>> >>> ...Jim Thompson >>> >>You have to put in a .model statement: >> >>.model simplesw sw(Vt=1 Vh=-.5 Ron=1 Roff=1T) >> >>and put 'simplesw' on the 'value' line in the dialogue box. >> >>To make a NC switch, you can interchange the values of Ron and Roff, i.e. >> >>.model simpleNC sw(Vt=1 Vh=-.5 Ron=1T Roff=1) >> >>Cheers >> >>Phil Hobbs > >Checked it out, LTspice switch with negative hysteresis looks exactly >same V-I curve as in PSpice... PSpice runs the OPA2140, LTspice will >not, so it looks like a major makeover. > >If you need only GBW and noise, that can be done simply, otherwise the >long winter ;-) > ><http://www.analog-innovations.com/SED/OP2140_JT_2015-08-11_07-39-39.jpg> > > ...Jim ThompsonBTW: PSpice won't converge on asymmetric supplies either. So the TI model is crap :-( ...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 ●August 11, 20152015-08-11
On 08/11/2015 12:52 PM, Jim Thompson wrote:> On Tue, 11 Aug 2015 07:45:28 -0700, Jim Thompson > <To-Email-Use-The-Envelope-Icon@On-My-Web-Site.com> wrote: > >> On Mon, 10 Aug 2015 22:37:04 -0400, Phil Hobbs >> <pcdhSpamMeSenseless@electrooptical.net> wrote: >> >>> On 8/10/2015 10:18 PM, Jim Thompson wrote: >>>> On Mon, 10 Aug 2015 21:11:51 -0400, Phil Hobbs >>>> <hobbs@electrooptical.net> wrote: >>>> >>>>> On 8/10/2015 9:04 PM, Jim Thompson wrote: >>>>>> On Sun, 9 Aug 2015 16:24:53 -0700 (PDT), Phil Hobbs >>>>>> <pcdhobbs@gmail.com> wrote: >>>>>> >>>>>>> Hi, Jim, >>>>>>> >>>>>>> If you've got some spare bandwidth, I could really use an improved >>>>>>> OPA2140 model. >>>>>>> >>>>>>> It's a very good part for moderate speed, low current, high >>>>>>> linearity TIAs, but it's a bear to simulate because the model won't >>>>>>> converge on an operating point in LTspice. >>>>>>> >>>>>>> I took the TINA model TI supplies and replaced the VSWITCH cards >>>>>>> with LTspice SW cards with negative hysteresis (more or less like >>>>>>> your fave tanh curve), but it still won't converge on ac or noise >>>>>>> sims. >>>>>>> >>>>>>> Thanks >>>>>>> >>>>>>> Phil Hobbs >>>>>> >>>>>> How do you set the parameters of the SW in LTspice? ...Jim Thompson >>>>>> >>>>> >>>>> RON, ROFF, which do what you'd expect; >>>>> VT, which is the switching threshold (the switch looks like RON for V > >>>>> VT, and ROFF for V < VT); >>>>> and VH, the hysteresis. >>>>> >>>>> If VH is positive, then the upward-going transition occurs at V = VT + >>>>> VH and the downward-going one at V = VT - VH. (IOW it does what you >>>>> expect except that VH is the half-width of the deadband, not the full >>>>> width.) >>>>> >>>>> Negative values of VH cause a smooth transition between RON and ROFF, so >>>>> that the switching begins at VT + VH (which is less than VT in this >>>>> case) and is complete at VT - VH (which is more than VT). IIRC the >>>>> function is some smooth polynomial approximation to the arctan, so at >>>>> least the first few derivatives are continuous. >>>>> >>>>> Cheers >>>>> >>>>> Phil Hobbs >>>> >>>> I'm used to PSpice, click on a symbol and you see a table where you >>>> fill in the blanks. I click on SW in LTspice, I see several blank >>>> lines... >>>> >>>> SpiceLine >>>> SpicelIne2 >>>> >>>> Where do I enter Ron, Roff, Von, Voff, etc? >>>> >>>> ...Jim Thompson >>>> >>> You have to put in a .model statement: >>> >>> .model simplesw sw(Vt=1 Vh=-.5 Ron=1 Roff=1T) >>> >>> and put 'simplesw' on the 'value' line in the dialogue box. >>> >>> To make a NC switch, you can interchange the values of Ron and Roff, i.e. >>> >>> .model simpleNC sw(Vt=1 Vh=-.5 Ron=1T Roff=1) >>> >>> Cheers >>> >>> Phil Hobbs >> >> Checked it out, LTspice switch with negative hysteresis looks exactly >> same V-I curve as in PSpice... PSpice runs the OPA2140, LTspice will >> not, so it looks like a major makeover. >> >> If you need only GBW and noise, that can be done simply, otherwise the >> long winter ;-) >> >> <http://www.analog-innovations.com/SED/OP2140_JT_2015-08-11_07-39-39.jpg> >> >> ...Jim Thompson > > BTW: PSpice won't converge on asymmetric supplies either. So the TI > model is crap :-( > > ...Jim Thompson >If I were more motivated I'd try it on TINA, but given the complexity of the model I'd be surprised if they'd fix it even if it's broken on TINA as well. Cheers Phil Hobbs -- Dr Philip C D Hobbs Principal Consultant ElectroOptical Innovations LLC Optics, Electro-optics, Photonics, Analog Electronics 160 North State Road #203 Briarcliff Manor NY 10510 hobbs at electrooptical dot net http://electrooptical.net
