Problem noted, and forwarded to the appropriate device-modeling manager at Analog Devices.
I, personally, have experienced some problems with ADI models. Reported same, and was told, "They work just fine here."
So don't hold your breath.
BTW, Sennewald is wrong when he says, "...generated by stupid programs or "roboters" and not by engineers."
They ARE generated by engineers, or should I say it as "engineers" ?:-)
...Jim Thompson
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC\'s and Discrete Systems | manus |
| Phoenix, Arizona Voice:(480)460-2350 | |
| E-mail Address at Website Fax:(480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |
I love to cook with wine. Sometimes I even put it in the food.
I simply passed on the posting to the ADI manager.
As previously noted, I, personally, have experienced issues with ADI models.
...Jim Thompson
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC\'s and Discrete Systems | manus |
| Phoenix, Arizona Voice:(480)460-2350 | |
| E-mail Address at Website Fax:(480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |
I love to cook with wine. Sometimes I even put it in the food.
The LM324 model from TI works fine,but the one from National Semiconductor is junk. I tried numerous Analog Devices models for various rail-to-rail opamps, and found that almost all i tried gave me the same kind of cryptic square root error. Those tried: AD8605, AD531, AD541, AD8552, and the AD8571; the only one tried that did work was for the AD8614. Now i would dearly like to have a set of models that were known to work (and more or less correctly), but i need to get a working AD8605 model. The sets i have came from the manufacturer created in the latter of
1992, and thus are not quite up-to-date. However, the model for the AD8605 was downloaded via the web just yesterday - implying the problem is not fixed.Can anyone help?
hello folks, just saw your message about my Spice models. I did the AD8605 model and would like to know what it is that you think isn't working. I would prefer to see the test circuit you're using and understand what you're trying to do. And if it really doesn't work, then I owe you a pizza of your choice.
Helmut Sennewald wrote:
opamps,
square
only one
to work
model.
of
But the AD8605 seems to NOT be one of them. Works AOK on PSpice.
Results conveyed to JA at ADI.
...Jim Thompson
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC\'s and Discrete Systems | manus |
| Phoenix, Arizona Voice:(480)460-2350 | |
| E-mail Address at Website Fax:(480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |
I love to cook with wine. Sometimes I even put it in the food.
"Robert Baer" schrieb im Newsbeitrag news:1PQ0e.3481$ snipped-for-privacy@newsread1.news.pas.earthlink.net...
Hello Robert, I don't believe that you really can judge the quality of these models as a beginner with SPICE simulations. I agree with you that most models have difficulties with convergence. Many of them are really over complicated and sometimes generated by stupid programs or "roboters" and not by engineers.
I assume that the listed models will work with some tweaking of the convergence parameters.
What simulator do you use? If it's LTspice then send me your files and I will make you a working example with your AD8605. I always want to see the schematic, because I know that people sometimes have errors in their circuit. One important thing is to have a DC path to ground(0).
Best Regards, Helmut Moderator of the LTspice user group
Hello Helmut: I got an email from a colleague informing of the problem and didn't see your response on the board.
snipped-for-privacy@gmail.com wrote:
cryptic
latter
just
convergence.
I have also checked it independently myself, on PSpice v10.3.
NO PROBLEM!
...Jim Thompson
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC\'s and Discrete Systems | manus |
| Phoenix, Arizona Voice:(480)460-2350 | |
| E-mail Address at Website Fax:(480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |
I love to cook with wine. Sometimes I even put it in the food.
Hmm useless huh? the AD8614 has 1mV of Vos and the model has 1mV, I just looked at it, so I don't know what you mean by not working. I think you may be overlooking some things here. Here's the Vos in the netlist... EOS 7 1 POLY(2) (73,98) (81,98) 1E-3 1 1
Robert Baer wrote:
opamps,
square
only one
to work
model.
of
convergence.
way
and
replace
and
poor
----- Original Message ----- From: "Jim Thompson" Newsgroups: sci.electronics.cad Sent: Friday, March 25, 2005 3:37 PM Subject: Re: Problems with SPICE models from vendors
Hello Jim, this wasn't necessary. This AD8605 model runs without any convergence problem in LTspice. So the model doesn't have any error. Yuu should withdraw your email to AD and apologize to the manager you have contacted for any inconvenience. :)
Best Regards, Helmut
For the rated VCC (+5V and up), I'm getting offset right at the typical of 1mV.
BUT the IB's are about double the MAX spec.
...Jim Thompson
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC\'s and Discrete Systems | manus |
| Phoenix, Arizona Voice:(480)460-2350 | |
| E-mail Address at Website Fax:(480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |
I love to cook with wine. Sometimes I even put it in the food.
[snip]
I just verified Baer's setup with PSpice. The IB's are running ~700nA, substantially larger than the MAX spec.
I simply visually scanned the data sheet, so I don't know... are we close enough to negative rail to cause the high IB?
...Jim Thompson
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC\'s and Discrete Systems | manus |
| Phoenix, Arizona Voice:(480)460-2350 | |
| E-mail Address at Website Fax:(480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |
I love to cook with wine. Sometimes I even put it in the food.
schrieb im Newsbeitrag news: snipped-for-privacy@l41g2000cwc.googlegroups.com...
Good morning Sir, I posted 2h40m ago that this model has no problem. Have you overlooked that or do you do you see postings only after many hours? Please use a better news reader. May news reader is uptodate within minutes.
Best Regards, Helmut
My posting from 2h40m ago:
Hello Jim, this wasn't necessary. This AD8605 model runs without any convergence problem in LTspice. So the model doesn't have any error. Yuu should withdraw your email to AD and apologize to the manager you have contacted for any inconvenience. :)
Best Regards, Helmut
Well, in a sense you are correct in labellling be as a beginner; i rarely use SPICE, but that useage has covered over 30 years. When one models a simple voltage follower, with the NI input half way between the poser supplies for the op-amp, one expects it to work, and not give a cryptic square root error. Furthermore, replacing the model used to a different one (eg replace the call from the AD8605 to the AD8614 (and changing *nothing* else) and have it work begs the question: what is wrong with the AD8605 model? The same can be said about the models for the LM324; the TI model works and the NatSemi does not.
And speaking of bad models that DO "work", the AD8614 is rather poor (from the .OUT file):
.OPTIONS ACCT LIST NODE OPTS NUMDGT=6 RELTOL=0.00001 NOPAGE .TEMP 27 .LIB ANLG_DEV.LIB ; most rail-to-rail opamps die with error .DC VBAT 4.499 4.501 0.001 VBAT 01 00 DC 4.5 VSET 10 00 0.209171 VIN 05 00 0.018051 R2 05 07 18.4K R3 10 08 18.4K R4 09 07 100K * NI I OUT XAMP2 08 07 01 00 09 AD8614/AD .PRINT DC V(05) V(07) V(08) V(09) .PLOT DC V(05) V(07) V(08) V(09) .SAVE
V(5) V(7) V(8) V(9)
1.80510E-02 2.22746E-01 2.21746E-01 1.26487E+00Look at the poor results: large input currents, large Vos. Almost useless; certainly not representative of the part.
I appreciate that you passed on the comments. Please see my slightly earlier response, showing problems with the AD8614 (high input currents and high Vos).
Please tell me why it does not work (and others mentioned) and that the model for the AD8614 does work. I am using a DOS version of TopSpice. And look at an earlier posting where i clearly show that the AD8614 model gives large input currents and a large Vos.
Here is a partial of the .OUT for the AD8614 which "works": .OPTIONS ACCT LIST NODE OPTS NUMDGT=6 RELTOL=0.00001 NOPAGE .TEMP 27 .LIB ANLG_DEV.LIB ; most rail-to-rail opamps die with square root error .DC VBAT 4.499 4.501 0.001 VBAT 01 00 DC 4.5 VSET 10 00 0.209171 VIN 05 00 0.018051 R2 05 07 18.4K R3 10 08 18.4K R4 09 07 100K * NI I OUT XAMP2 08 07 01 00 09 AD8614/AD ;AD8605 U2 .PRINT DC V(05) V(07) V(08) V(09) .PLOT DC V(05) V(07) V(08) V(09) .SAVE
V(5) V(7) V(8) V(9)
1.80510E-02 2.22746E-01 2.21746E-01 1.26487E+00Note the large input currents and large Vos. Will see if i can run my DOS TopSpice when online...
*********** Well, the error message is only on the screen, and it is hard to read. If i interpreted it correctly, it states "run time error M6201: MATH-sqrt: DOMAIN error". I hope this information is of some use. Meanwhile, maybe i can figure out how to download LTspice (if it is not gigantic, as i am on POTS).
***********schrieb im Newsbeitrag news: snipped-for-privacy@f14g2000cwb.googlegroups.com...
Hello zidane,
Robert was especially disappointed about the bias current. It is modeled with about 700nA. The datasheet shows max. Ib=400nA. It's a valid question why Ib is modelled not with the typical values. The later curves in the datasheet show Ib=300nA. I am talking about Ib when Vin is near the supply rails. Maybe you can enlighten us about the bias current.
I agree with your typical Vos of 1mV.
Best Regards, Helmut
Hello Robert, please tell me who said that the Ad8605 model doesn't work? Maybe TopSpice has problems with this opamp whereas other SPICE variants don't have a problem with the AD8605. The different SPICE versions on the market are far off from the original SPICE program code.
Best Regards, Helmut
Ok, i am convinced that the AD8614 was a lousy choice - but it was the only rail-to-rail model that worked at that time. I have downloaded SwitcherCAD3 and have part of my circuit working using the AD8605 model. So it is clear that there is something about those non-working-for-TopSpice models that goof it up, but is allowed in the more modern SPICE programs. That said, the results i get are WRONG - essentially it is saying that 1+1 is not 2. I could attach the .ASC file, but it is fairly large (about 4K), and tell you what the node voltages SC3 gives. Let me do it the quick way; SC3 sez: N003 at 0.295mV; R2=18.2K from N003 to N007 at 0.188481V; op amp NI at N006, I at N007, output at N008, V- at gnd, v+ at 4.5V; feedback R4=100K from N006 to N007; N006 at 0.188571V; I(R2)=I(R4)=10.3399uA; N008=0.376666V.
But do the calcs by hand; I(R2) = (0.188481V-0.000295V)/(18.2K) =
0.0103398mA. Drop across 100k then is 1.03398V; add to voltage at N007 for calc(N008)=1.222461V.Therefore 1+1=2 and Spice is whistling Dixie.
ElectronDepot website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.