Keyboard Shortcuts
ctrl + shift + ? :
Показати всі комбінації клавіш
ctrl + g :
Не доступний для безкоштовних груп.
ctrl + shift + f :
Знайти
ctrl + / :
Сповіщення
esc to dismiss
Лайки
Пошук
Simple model for diffin-diffout amp
|
Apparajan
I have uploaded my model
Temp-->File-->>E_model_for_diffamp.asc It is a very simple model that models the differential and common mode loop gains. I have other more complicated models that model slew-rate, bandwidth, etc. However my most complicated model seems to be much simpler than what is commercially available? They also have a disclimer that they don't model offset, psrr, cmrr etc.? What gives... |
|
Apparajan
I am re-posting this since I din't get a boo or an aye or nay..
переключити цитоване повідомлення
Показати цитований текст
Cheers AG --- In LTspice@..., "Apparajan" <dg1@...> wrote:
|
|
Hi AG,
переключити цитоване повідомлення
Показати цитований текст
I would caution against using a simple E source based fully differential amp model. Usually G source with appropriate resistor results in a much better behaved model. I believe I suggested you download some ADC models. within that ADC collection are some fully differential CMOS opamp / OTA models. For a very simple model I would use .subckt ideal_differential_op_amp Vinm Vinp Outp VCM Outm R1 Outp N001 1 R2 N001 Outm 1 G1 N001 Outp Vinp Vinm 100MEG G2 Outm N001 Vinp Vinm 100MEG G3 0 N001 VCM N001 100MEG .ends ideal_differential_op_amp you can also include output caps to limit the bandwidth and change the resistor values to model the output impedance. I cant give you the exact models I use at work because they don't really belong to me. regards Robert --- In LTspice@..., "Apparajan" <dg1@...> wrote:
|
|
Hi AG,
переключити цитоване повідомлення
Показати цитований текст
I forgot to mention that there is an A-device OTA (single ended unfortunately) look LTspice\lib\sub folder at the UniversalOpamps2.sub file it is a text netlist file, with an example of how to use the OTA e.g. A1 2 1 0 0 0 0 out 0 OTA G={Avol/Rout} ref={Vos} linear Cout={Cout} + en={en} enk={enk} in={in} ink={ink} incm={incm} incmk={incmk} + Vhigh=1e308 Vlow=-1e308 Rout={Rout} R5 2 3 {2*Rin} noiseless R6 1 4 {2*Rin} noiseless R1 3 1 {2*Rin} noiseless R2 2 4 {2*Rin} noiseless .param Rout=.1 .param Cout={Avol/GBW/2/pi/Rout} .param Avol=1Meg GBW=10Meg Slew=10Meg ilimit=25m rail=0 Vos=0 .param en=0 enk=0 in=0 ink=0 incm=0 incmk=0 Rin=1G regards Robert --- In LTspice@..., "RobertTalty" <rtalty@...> wrote:
|
|
Ganesan
Thanks for the suggestions.. I will get back in a few days..
My more complicated models which I did not post are Gm and R based.. However my most complicated model seems to be much simpler than what is commercially available? They also have a disclaimer that they don't model offset, psrr, cmrr etc.? What gives.. This question still remains unanswered.. Cheers ag > > --- In LTspice@... <mailto:LTspice%40yahoogroups.com>, "Apparajan" <dg1@> wrote: > > > > > > I have uploaded my model > > > Temp-->File-->>E_model_for_diffamp.asc > > > It is a very simple model that models the differential and common mode loop gains. I have other more complicated models that model slew-rate, bandwidth, etc. However my most complicated model seems to be much simpler than what is commercially available? They also have a disclimer that they don't model offset, psrr, cmrr etc.? What gives... > > > |
|
I'm not sure I understand
переключити цитоване повідомлення
Показати цитований текст
How do you model offset? I model it by adding a DC source in series with the In+ or IN- gate. some value between 100uV and 10mV depending on the expected mismatch of the input pair. Model PSRR requires that you model the power supply, which a simple G/R model does not have, also the typical sources of non-ideal opamp performance that results in power supply variation transferring to the output signal neesd to be correctly modeled. simple things like the variations in current sources with power supply voltage, the correct model for this depends on weather you cascode the mirrors or not. Same thing with Cmrr? A differential G with perfect R load has infinite CMRR, modeling CMRR requires that you include errors that cause CMRR. in your model. This requires some knowledge of the Input pair type and the cascode bias levels. BTW most commercial device level spice models are very badly written. I mean VERY BADLY written. so they are unlikely to include these effects, heck Microchips opamp models usually don't even converge properly. The Microchip opamp spic models are very complex and attempt to model all types of errors and their Temp variations, but in the end these models cause convergence problems, so what is the point of a complex model that causes beginners convergence problems. Convergence can be hard for experienced spice users to solve, so it is the last thing that beginners need. So if you want to see some complex models go to Microchip and download some of their spice models. regards Robert --- In LTspice@..., Ganesan <dg1@...> wrote:
|
|
Ganesan
Thanks.. I model offset by dial ling some mismatch, so it includes
переключити цитоване повідомлення
Показати цитований текст
temperature effects.. I can understand Microchip having poor models.. But TI, LTC and ADI have way too complex models for the job they seem to do. I thought these models are simple representations of the real device intended to give the board level designer something to simulate his circuit with.. The way these commercial models are, it looks like they took the schematic from the chip design engineer and did a poor job of obscuring proprietary information. cheers AG ===================================================================================================================== On 9/14/2011 9:52 AM, RobertTalty wrote:
|
|
You may want to look at Intersil's AN1556. See:
переключити цитоване повідомлення
Показати цитований текст
<http://www.intersil.com/data/an/an1556.pdf> The author makes this claim about his method "Finally, Accurate SPICE Models I can Understand and Modify to Fit my Simulation Needs. The authors model "enables the user to simulate important AC and DC parameters of an amplifier. AC parameters incorporated into the model are: 1/f and flat-band noise, slew rate, CMRR, gain and phase. The DC parameters are V_OS , I_OS , total supply current and output voltage swing." Limitations of the model are: "25 Deg C only, no temperature dependence No current noise capability Does not provide supply current as a function of load current" Howard On 9/14/2011 6:54 AM, Ganesan wrote:
Thanks for the suggestions.. I will get back in a few days.. |
|
Ganesan
Thanks.. Much obliged.
переключити цитоване повідомлення
Показати цитований текст
Cheers A. Ganesan On 9/14/2011 4:04 PM, Howard Hansen wrote:
|
|
Hi AG,
переключити цитоване повідомлення
Показати цитований текст
You may want to read through a series of articles by Kendall see post# 30118 I know that he wrote a test suite for opamp models that tried to include PSRR / CMRR etc. I think this was about 2007 time frame. However everything that he is writing about is for regular single ended opamps. PSRR and CMRR in Fully differential opamps is very different to PSRR in single ended opamps. Most simulations, even with input pair mismatch, will show very very low PSRR for a fully differential opamps. The PSRR of the first stage becomes CMRR of the following stage, so if you just measure one stage fully diff out, you get almost infinite PSRR. Unfortunately the system PSRR for a fully diff system is often worse than a regular opamp (especially at low frequencies) because mismatch and asymmetry cause PSRR in fully diff opamps and this is hard to model properly. Most fully differential opamps have about 60db to 70dB PSRR that is fairly constant for most of the frequency band, this is VERY different from the PSRR of a regular opamp. You might want to play around with some PSRR measurements for fully differential opamp filters / PGA stages etc and get an idea about how Power supply variation / noise actually translates (over frequency) to an output error. The process is not that simple. regards Robert --- In LTspice@..., Ganesan <dg1@...> wrote:
|
|
Ganesan
Thanks.. I usually count on only 40 db from differential stuff or 1%
переключити цитоване повідомлення
Показати цитований текст
matching.. 0.1% is achievable with a lot of attention to layout When I get time I will read his postings in detail. It reinforces my thesis that simpler models will suffice.. Why the unnecessary device level complexity..? Cheers AG On 9/14/2011 10:07 PM, RobertTalty wrote:
|
|
ehydra
Indeed, and that is the reason why I just use the datasheet and the universalopamp symbol to get rid of the problems. Most times the universalopamp makes a better job.
переключити цитоване повідомлення
Показати цитований текст
- Henry -- ehydra.dyndns.info RobertTalty schrieb: The Microchip opamp spic models are very complex and attempt to model all types of errors and their Temp variations, but in the end these models cause convergence problems, so what is the point of a complex model that causes beginners convergence problems. Convergence can be hard for experienced spice users to solve, so it is the last thing that beginners need. |
Повідомлення
Більше
Додаткові параметри
Більше
to navigate to use esc to dismiss