Hi, I have the AD8014 Spice model from Analog Devices, and I have LT Spice. The model file AD8014.cir starts with... AD8014 SPICE model * Node assignments * non-inverting input * | inverting input * | | positive supply * | | | negative supply * | | | | output * | | | | | .SUBCKT AD8014 1 2 99 50 28 So, how do I draw an LT Spice schematic, with the usual opamp symbol, and plug this model into it? I'm having a small problem with my ramp circuit ftp://jjlarkin.lmi.net/Ramp.JPG and it would be more convenient, just now, to tweak it by simulating instead of soldering. Yes, yes, I should know this, but I don't use Spice often enough to remember all the mechanics. Speaking of which, we have more ideas and stuff to do than we have time and energy. It would be great to have someone who could do Spice setups and simulations and parts research and maybe a little breadboarding for us occasionally, for pay of course. John
LT Spice question
Started by ●December 15, 2011
Reply by ●December 15, 20112011-12-15
On 15 Dec., 17:21, John Larkin <jjlar...@highNOTlandTHIStechnologyPART.com> wrote:> Hi, > > I have the AD8014 Spice model from Analog Devices, and I have LT > Spice. > > The model file AD8014.cir starts with... > > AD8014 =A0SPICE model > > * =A0 =A0 =A0Node assignments > * =A0 =A0 =A0 =A0 =A0 =A0 =A0 =A0 =A0 =A0 =A0 =A0non-inverting input > * =A0 =A0 =A0 =A0 =A0 =A0 =A0 =A0 =A0 =A0 =A0 =A0| =A0inverting input > * =A0 =A0 =A0 =A0 =A0 =A0 =A0 =A0 =A0 =A0 =A0 =A0| =A0| =A0positive suppl=y> * =A0 =A0 =A0 =A0 =A0 =A0 =A0 =A0 =A0 =A0 =A0 =A0| =A0| =A0| =A0 negative=supply> * =A0 =A0 =A0 =A0 =A0 =A0 =A0 =A0 =A0 =A0 =A0 =A0| =A0| =A0| =A0 | =A0out=put> * =A0 =A0 =A0 =A0 =A0 =A0 =A0 =A0 =A0 =A0 =A0 =A0| =A0| =A0| =A0 | =A0| > .SUBCKT AD8014 =A0 =A0 =A0 =A0 =A0 1 =A02 =A099 =A050 28 > > So, how do I draw an LT Spice schematic, with the usual opamp symbol, > and plug this model into it? > > I'm having a small problem with my ramp circuit > > ftp://jjlarkin.lmi.net/Ramp.JPG > > and it would be more convenient, just now, to tweak it by simulating > instead of soldering. > > Yes, yes, I should know this, but I don't use Spice often enough to > remember all the mechanics. > > Speaking of which, we have more ideas and stuff to do than we have > time and energy. It would be great to have someone who could do Spice > setups and simulations and parts research and maybe a little > breadboarding for us occasionally, for pay of course. > > Johninclude the file, or paste all of it as a spice statement on the schematic that way it is all in one file put an opamp2 on the schematic and right-click to change its 'value' to AD8014 check the pin order -Lasse
Reply by ●December 15, 20112011-12-15
John Larkin wrote:> Hi, > > I have the AD8014 Spice model from Analog Devices, and I have LT > Spice. > > The model file AD8014.cir starts with... > > > AD8014 SPICE model > > * Node assignments > * non-inverting input > * | inverting input > * | | positive supply > * | | | negative supply > * | | | | output > * | | | | | > .SUBCKT AD8014 1 2 99 50 28 > > > So, how do I draw an LT Spice schematic, with the usual opamp symbol, > and plug this model into it? > > I'm having a small problem with my ramp circuit > > ftp://jjlarkin.lmi.net/Ramp.JPG > > and it would be more convenient, just now, to tweak it by simulating > instead of soldering. > > Yes, yes, I should know this, but I don't use Spice often enough to > remember all the mechanics. >It's been very long ago that I crammed in another opamp but it's mostly about the correct order of nodes. This seems like a good step-by-step descritpion: http://dev.emcelettronica.com/how-to-use-manufacturer-supplied-model-ltspice> Speaking of which, we have more ideas and stuff to do than we have > time and energy. It would be great to have someone who could do Spice > setups and simulations and parts research and maybe a little > breadboarding for us occasionally, for pay of course. >I don't know anyone in the S.F. area. But I do know someone who is experienced in fast FPGA stuff if that ever comes up, about a mile from you guys. -- Regards, Joerg http://www.analogconsultants.com/
Reply by ●December 15, 20112011-12-15
On Thu, 15 Dec 2011 08:39:16 -0800, Joerg <invalid@invalid.invalid> wrote:>John Larkin wrote: >> Hi, >> >> I have the AD8014 Spice model from Analog Devices, and I have LT >> Spice. >> >> The model file AD8014.cir starts with... >> >> >> AD8014 SPICE model >> >> * Node assignments >> * non-inverting input >> * | inverting input >> * | | positive supply >> * | | | negative supply >> * | | | | output >> * | | | | | >> .SUBCKT AD8014 1 2 99 50 28 >> >> >> So, how do I draw an LT Spice schematic, with the usual opamp symbol, >> and plug this model into it? >> >> I'm having a small problem with my ramp circuit >> >> ftp://jjlarkin.lmi.net/Ramp.JPG >> >> and it would be more convenient, just now, to tweak it by simulating >> instead of soldering. >> >> Yes, yes, I should know this, but I don't use Spice often enough to >> remember all the mechanics. >> > >It's been very long ago that I crammed in another opamp but it's mostly >about the correct order of nodes. This seems like a good step-by-step >descritpion: > >http://dev.emcelettronica.com/how-to-use-manufacturer-supplied-model-ltspice > > >> Speaking of which, we have more ideas and stuff to do than we have >> time and energy. It would be great to have someone who could do Spice >> setups and simulations and parts research and maybe a little >> breadboarding for us occasionally, for pay of course. >> > >I don't know anyone in the S.F. area. But I do know someone who is >experienced in fast FPGA stuff if that ever comes up, about a mile from >you guys.Connect us up! We're constantly overloaded on FPGA design. There's a beer in it for you. We are working with a really good guy in San Diego, but he's in San Diego. http://www.amazon.com/Blaine-C.-Readler/e/B001K7PSRM/ref=sr_ntt_srch_lnk_7?qid=1323968214&sr=1-7 Check out his books. John
Reply by ●December 15, 20112011-12-15
On 12/15/2011 11:21 AM, John Larkin wrote:> Hi, > > I have the AD8014 Spice model from Analog Devices, and I have LT > Spice. > > The model file AD8014.cir starts with... > > > AD8014 SPICE model > > * Node assignments > * non-inverting input > * | inverting input > * | | positive supply > * | | | negative supply > * | | | | output > * | | | | | > .SUBCKT AD8014 1 2 99 50 28 > > > So, how do I draw an LT Spice schematic, with the usual opamp symbol, > and plug this model into it? > > I'm having a small problem with my ramp circuit > > ftp://jjlarkin.lmi.net/Ramp.JPG > > and it would be more convenient, just now, to tweak it by simulating > instead of soldering. > > Yes, yes, I should know this, but I don't use Spice often enough to > remember all the mechanics. > > Speaking of which, we have more ideas and stuff to do than we have > time and energy. It would be great to have someone who could do Spice > setups and simulations and parts research and maybe a little > breadboarding for us occasionally, for pay of course. > > John >.include AD8014.CIR F2->OpAmp2->set value to AD8014 Oh, and make sure the pins are in the right order in the .SUBCKT line--check by comparison to a model that you know works. 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 845-480-2058 hobbs at electrooptical dot net http://electrooptical.net
Reply by ●December 15, 20112011-12-15
On 12/15/2011 11:59 AM, John Larkin wrote:> On Thu, 15 Dec 2011 08:39:16 -0800, Joerg<invalid@invalid.invalid> > wrote: > >> John Larkin wrote: >>> Hi, >>> >>> I have the AD8014 Spice model from Analog Devices, and I have LT >>> Spice. >>> >>> The model file AD8014.cir starts with... >>> >>> >>> AD8014 SPICE model >>> >>> * Node assignments >>> * non-inverting input >>> * | inverting input >>> * | | positive supply >>> * | | | negative supply >>> * | | | | output >>> * | | | | | >>> .SUBCKT AD8014 1 2 99 50 28 >>> >>> >>> So, how do I draw an LT Spice schematic, with the usual opamp symbol, >>> and plug this model into it? >>> >>> I'm having a small problem with my ramp circuit >>> >>> ftp://jjlarkin.lmi.net/Ramp.JPG >>> >>> and it would be more convenient, just now, to tweak it by simulating >>> instead of soldering. >>> >>> Yes, yes, I should know this, but I don't use Spice often enough to >>> remember all the mechanics. >>> >> >> It's been very long ago that I crammed in another opamp but it's mostly >> about the correct order of nodes. This seems like a good step-by-step >> descritpion: >> >> http://dev.emcelettronica.com/how-to-use-manufacturer-supplied-model-ltspice >> >> >>> Speaking of which, we have more ideas and stuff to do than we have >>> time and energy. It would be great to have someone who could do Spice >>> setups and simulations and parts research and maybe a little >>> breadboarding for us occasionally, for pay of course. >>> >> >> I don't know anyone in the S.F. area. But I do know someone who is >> experienced in fast FPGA stuff if that ever comes up, about a mile from >> you guys. > > Connect us up! We're constantly overloaded on FPGA design. There's a > beer in it for you. > > We are working with a really good guy in San Diego, but he's in San > Diego. > > http://www.amazon.com/Blaine-C.-Readler/e/B001K7PSRM/ref=sr_ntt_srch_lnk_7?qid=1323968214&sr=1-7 > > Check out his books. > > John >He writes books about FPGAs and monsters in the attic. I see the common thread. ;) 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 845-480-2058 hobbs at electrooptical dot net http://electrooptical.net
Reply by ●December 15, 20112011-12-15
John Larkin wrote:> On Thu, 15 Dec 2011 08:39:16 -0800, Joerg <invalid@invalid.invalid> > wrote: > >> John Larkin wrote: >>> Hi, >>> >>> I have the AD8014 Spice model from Analog Devices, and I have LT >>> Spice. >>> >>> The model file AD8014.cir starts with... >>> >>> >>> AD8014 SPICE model >>> >>> * Node assignments >>> * non-inverting input >>> * | inverting input >>> * | | positive supply >>> * | | | negative supply >>> * | | | | output >>> * | | | | | >>> .SUBCKT AD8014 1 2 99 50 28 >>> >>> >>> So, how do I draw an LT Spice schematic, with the usual opamp symbol, >>> and plug this model into it? >>> >>> I'm having a small problem with my ramp circuit >>> >>> ftp://jjlarkin.lmi.net/Ramp.JPG >>> >>> and it would be more convenient, just now, to tweak it by simulating >>> instead of soldering. >>> >>> Yes, yes, I should know this, but I don't use Spice often enough to >>> remember all the mechanics. >>> >> It's been very long ago that I crammed in another opamp but it's mostly >> about the correct order of nodes. This seems like a good step-by-step >> descritpion: >> >> http://dev.emcelettronica.com/how-to-use-manufacturer-supplied-model-ltspice >> >> >>> Speaking of which, we have more ideas and stuff to do than we have >>> time and energy. It would be great to have someone who could do Spice >>> setups and simulations and parts research and maybe a little >>> breadboarding for us occasionally, for pay of course. >>> >> I don't know anyone in the S.F. area. But I do know someone who is >> experienced in fast FPGA stuff if that ever comes up, about a mile from >> you guys. > > Connect us up! We're constantly overloaded on FPGA design. There's a > beer in it for you. >Done.> We are working with a really good guy in San Diego, but he's in San > Diego. > > http://www.amazon.com/Blaine-C.-Readler/e/B001K7PSRM/ref=sr_ntt_srch_lnk_7?qid=1323968214&sr=1-7 > > Check out his books. >He's got some really interesting books :-) It is great when engineers also do other totally non-EE stuff, else they become nerds. The most drastic career change I saw is an EE who used to design 750kV equipment and transmission lines, then decided to start a care home for Alzheimer's patients. And he is amazingly good at that. -- Regards, Joerg http://www.analogconsultants.com/
Reply by ●December 15, 20112011-12-15
On Thu, 15 Dec 2011 12:07:04 -0500, Phil Hobbs <pcdhSpamMeSenseless@electrooptical.net> wrote:>On 12/15/2011 11:21 AM, John Larkin wrote: >> Hi, >> >> I have the AD8014 Spice model from Analog Devices, and I have LT >> Spice. >> >> The model file AD8014.cir starts with... >> >> >> AD8014 SPICE model >> >> * Node assignments >> * non-inverting input >> * | inverting input >> * | | positive supply >> * | | | negative supply >> * | | | | output >> * | | | | | >> .SUBCKT AD8014 1 2 99 50 28 >> >> >> So, how do I draw an LT Spice schematic, with the usual opamp symbol, >> and plug this model into it? >> >> I'm having a small problem with my ramp circuit >> >> ftp://jjlarkin.lmi.net/Ramp.JPG >> >> and it would be more convenient, just now, to tweak it by simulating >> instead of soldering. >> >> Yes, yes, I should know this, but I don't use Spice often enough to >> remember all the mechanics. >> >> Speaking of which, we have more ideas and stuff to do than we have >> time and energy. It would be great to have someone who could do Spice >> setups and simulations and parts research and maybe a little >> breadboarding for us occasionally, for pay of course. >> >> John >> > >.include AD8014.CIR > >F2->OpAmp2->set value to AD8014 > >Oh, and make sure the pins are in the right order in the .SUBCKT >line--check by comparison to a model that you know works. > >Cheers > >Phil HobbsOK, this works: Version 4 SHEET 1 916 680 WIRE 656 -304 608 -304 WIRE 704 -304 656 -304 WIRE 608 -256 608 -304 WIRE 560 -240 -272 -240 WIRE 192 -176 96 -176 WIRE 96 -128 96 -176 WIRE 608 -128 608 -176 WIRE 192 -112 192 -176 WIRE 560 -16 560 -192 WIRE -128 16 -192 16 WIRE 16 16 -64 16 WIRE 144 16 16 16 WIRE 272 16 224 16 WIRE -192 48 -192 16 WIRE 96 64 96 -48 WIRE 16 80 16 16 WIRE 64 80 16 80 WIRE 272 96 272 16 WIRE 272 96 128 96 WIRE 336 96 272 96 WIRE 448 96 416 96 WIRE 560 96 560 -16 WIRE 560 96 528 96 WIRE -352 112 -416 112 WIRE -272 112 -272 -240 WIRE -272 112 -352 112 WIRE 64 112 -272 112 WIRE 560 128 560 96 WIRE -416 144 -416 112 WIRE -272 144 -272 112 WIRE 560 224 560 192 WIRE -416 240 -416 224 WIRE -272 240 -272 208 WIRE 96 240 96 128 WIRE 96 368 96 320 FLAG -272 240 0 FLAG 560 224 0 FLAG -416 240 0 FLAG 192 -112 0 FLAG 96 368 0 FLAG -192 48 0 FLAG 608 -128 0 FLAG 656 -304 ERROR FLAG -352 112 RAMP FLAG 272 16 AMP FLAG 560 -16 OUT SYMBOL cap -288 144 R0 WINDOW 0 71 15 Left 2 WINDOW 3 64 50 Left 2 SYMATTR InstName C1 SYMATTR Value 47p SYMBOL cap 544 128 R0 WINDOW 0 71 11 Left 2 WINDOW 3 65 47 Left 2 SYMATTR InstName C2 SYMATTR Value 47p SYMBOL ind 432 112 R270 WINDOW 0 32 56 VTop 2 WINDOW 3 5 56 VBottom 2 SYMATTR InstName L1 SYMATTR Value 1n SYMBOL res 432 80 R90 WINDOW 0 0 56 VBottom 2 WINDOW 3 32 56 VTop 2 SYMATTR InstName R1 SYMATTR Value 50 SYMBOL current -416 224 R180 WINDOW 0 24 88 Left 2 WINDOW 3 -93 202 Left 2 WINDOW 123 0 0 Left 2 WINDOW 39 0 0 Left 2 SYMATTR InstName I1 SYMATTR Value PULSE(0 0.006 0 1n 1n 30n) SYMBOL Opamps\\opamp2 96 32 R0 WINDOW 0 45 101 Left 2 WINDOW 3 30 139 Left 2 SYMATTR InstName U1 SYMATTR Value AD8014 SYMBOL voltage 96 -32 R180 WINDOW 0 53 71 Left 2 WINDOW 3 61 36 Left 2 WINDOW 123 0 0 Left 2 WINDOW 39 0 0 Left 2 SYMATTR InstName V1 SYMATTR Value 5 SYMBOL voltage 96 336 R180 WINDOW 0 69 70 Left 2 WINDOW 3 75 33 Left 2 WINDOW 123 0 0 Left 2 WINDOW 39 0 0 Left 2 SYMATTR InstName V2 SYMATTR Value 5 SYMBOL res 240 0 R90 WINDOW 0 0 56 VBottom 2 WINDOW 3 32 56 VTop 2 SYMATTR InstName R2 SYMATTR Value 249 SYMBOL cap -64 0 R90 WINDOW 0 0 32 VBottom 2 WINDOW 3 32 32 VTop 2 SYMATTR InstName C3 SYMATTR Value 1p SYMBOL e 608 -272 R0 WINDOW 0 66 42 Left 2 WINDOW 3 64 76 Left 2 SYMATTR InstName E1 SYMATTR Value 10 TEXT -184 -176 Left 2 !.tran 0 30n 0 TEXT -200 -120 Left 2 !.lib AD8014.CIR I'm trying to get the most linear ramp at OUT, from +1 to +3 volts in 16 ns. AD8014 was probably a bad choice, and the best feedback resistor value is way below the 1K that ADI suggests for a follower. I had to use .lib instead of .include to make LT Spice happy. The default pin order was ok. If the opamp model is accurate (namely, it doesn't oscillate with the 249 ohm resistor) it looks pretty good. My original circuit (R2=1K, L1=56n) was terrible. I'll try it in real life next. Thanks. John
Reply by ●December 15, 20112011-12-15
John Larkin wrote: [SPICE netlist]> > I'm trying to get the most linear ramp at OUT, from +1 to +3 volts in > 16 ns. AD8014 was probably a bad choice, and the best feedback > resistor value is way below the 1K that ADI suggests for a follower. > > I had to use .lib instead of .include to make LT Spice happy. The > default pin order was ok. > > If the opamp model is accurate (namely, it doesn't oscillate with the > 249 ohm resistor) it looks pretty good. My original circuit (R2=1K, > L1=56n) was terrible. I'll try it in real life next. >Doesn't look bad at all. For snappier corners you have to pick an amp with a lot more bandwidth. Like this little dude: http://www.ti.com/lit/ds/symlink/ths4303.pdf However, the AD8014 is a CFB and they really do not like this configuration with just Rf and a cap from IN- to ground. Might put them close to oscillation even if SPICE says they are ok. -- Regards, Joerg http://www.analogconsultants.com/
Reply by ●December 15, 20112011-12-15
Joerg a �crit :> John Larkin wrote: > > [SPICE netlist] > >> I'm trying to get the most linear ramp at OUT, from +1 to +3 volts in >> 16 ns. AD8014 was probably a bad choice, and the best feedback >> resistor value is way below the 1K that ADI suggests for a follower. >> >> I had to use .lib instead of .include to make LT Spice happy. The >> default pin order was ok. >> >> If the opamp model is accurate (namely, it doesn't oscillate with the >> 249 ohm resistor) it looks pretty good. My original circuit (R2=1K, >> L1=56n) was terrible. I'll try it in real life next. >> > > Doesn't look bad at all. For snappier corners you have to pick an amp > with a lot more bandwidth. Like this little dude: > > http://www.ti.com/lit/ds/symlink/ths4303.pdf > > However, the AD8014 is a CFB and they really do not like this > configuration with just Rf and a cap from IN- to ground. Might put them > close to oscillation even if SPICE says they are ok. >Ahem, CFB opamp, for the same FB resistor, do tolerate more parasitics than VFB opamps. Because the additional parasitic pole frequency is Rfb Cp for the VFB and is Rin Cp for the CFB opamp, with Rin being roughly between 50R and 100R. What CFB opamps don't like much is parasitic inductance in series with their minus input. -- Thanks, Fred.
