 |
 | Home | Contact Us | FAQ | Search & Site Map | Link to Us |
 | Sign In | Join | Other 45 Sites in Network |
| HomeDiscussion GroupsElectronicsBasicsRepairDesignCADComponentsEquipmentElectrical Engineering ElectronicsKB.com Contact UsLink To UsSearch & Site Map |
Electronics Forum / CAD / March 2005Problems with SPICE models from vendors
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? > The LM324 model from TI works fine,but the one from National > Semiconductor is junk. [quoted text clipped - 11 lines] > > Can anyone help? 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 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. > > The LM324 model from TI works fine,but the one from National > > Semiconductor is junk. [quoted text clipped - 8 lines] > > 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. > > [quoted text clipped - 20 lines] > Helmut > Moderator of the LTspice user group > 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. 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: > Problem noted, and forwarded to the appropriate device-modeling > manager at Analog Devices. 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 >> 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 [quoted text clipped - 24 lines] >Best Regards, >Helmut 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. Hello Helmut: I got an email from a colleague informing of the problem and didn't see your response on the board. > 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 [quoted text clipped - 45 lines] > > Helmut > > Moderator of the LTspice user group > 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 [quoted text clipped - 57 lines] >>Helmut >>Moderator of the LTspice user group 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+00 Note 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). *********** >> The LM324 model from TI works fine,but the one from National >>Semiconductor is junk. [quoted text clipped - 32 lines] > Helmut > Moderator of the LTspice user group 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+00 Look at the poor results: large input currents, large Vos. Almost useless; certainly not representative of the part. >>> The LM324 model from TI works fine,but the one from National >>>Semiconductor is junk. [quoted text clipped - 69 lines] > Look at the poor results: large input currents, large Vos. Almost >useless; certainly not representative of the part. 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. 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 > >> The LM324 model from TI works fine,but the one from National > >>Semiconductor is junk. [quoted text clipped - 8 lines] > >>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. > >> [quoted text clipped - 22 lines] > > > 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 [quoted text clipped - 30 lines] > > Look at the poor results: large input currents, large Vos. Almost > useless; certainly not representative of the part. >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 [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. > 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 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 you're right Ib is actually 681nA but that's because the model reflects the first revision, it's dependant of the Bf, my guess is that no one created a second version of this model. > 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 [quoted text clipped - 114 lines] > >>useless; certainly not representative of the part. 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. >> 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 [quoted text clipped - 137 lines] > > Therefore 1+1=2 and Spice is whistling Dixie. What I found disturbing was that the bias currents were way in excess of MAX specification. ...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. [quoted text clipped - 11 lines] > > Can anyone help? 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. ----- Original Message ----- From: "Jim Thompson" <thegreatone@example.com> Newsgroups: sci.electronics.cad Sent: Friday, March 25, 2005 3:37 PM Subject: Re: Problems with SPICE models from vendors >> The LM324 model from TI works fine,but the one from National >>Semiconductor is junk. [quoted text clipped - 15 lines] > Problem noted, and forwarded to the appropriate device-modeling > manager at Analog Devices. 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 >----- Original Message ----- >From: "Jim Thompson" <thegreatone@example.com> [quoted text clipped - 30 lines] >Best Regards, >Helmut 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. >>----- Original Message ----- >>From: "Jim Thompson" <thegreatone@example.com> [quoted text clipped - 37 lines] > > ...Jim Thompson 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. > ----- Original Message ----- > From: "Jim Thompson" <thegreatone@example.com> [quoted text clipped - 30 lines] > Best Regards, > Helmut 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. >> ----- Original Message ----- >> From: "Jim Thompson" <thegreatone@example.com> [quoted text clipped - 35 lines] > And look at an earlier posting where i clearly show that the AD8614 > model gives large input currents and a large Vos. 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 >>>----- Original Message ----- >>>From: "Jim Thompson" <thegreatone@example.com> [quoted text clipped - 46 lines] > Best Regards, > Helmut I said that the AD8605 model does not work; at least for the old DOS TopSpice. Based on raw experience. Found the same model appears to work in Switchercad3 which i recently downloaded. See previous recent postings by me; there are nasty errors in a simple amplifier circuit using the AD8605. >> The LM324 model from TI works fine,but the one from National >>Semiconductor is junk. [quoted text clipped - 27 lines] > > ...Jim Thompson 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). > The LM324 model from TI works fine,but the one from National > Semiconductor is junk. [quoted text clipped - 12 lines] > > Can anyone help? Thanks! Using LTspice solved the problem. It also ensures that the model accurately mirrors the schematic. With the DOS TopSpice, transcription errors can cause problems (and did!). However, it *would* be of great use if: 1) one could easily edit wires (length, placement, number of corners and where corners are). 2) one could have a little window by a (chosen) node that gave the DC (or other value). 3) that the output, both text and graph could be directly saved. .PRINT and .SAVE just do not cut it here. 4) that the duplicate function would allow creation of more than one; sometimes you need 5 more of something... ************* I noticed that in some cases, setting ITL1 and/or ITL6 "small" can allow something to converge, where a setting of 200 or more can kill convergence. And he higher the value of ITL1 and/or ITL6, the worse the problem is. Why?? > Using LTspice solved the problem. > However, it *would* be of great use if: [snip] Just to add to the LTspice wish-list........ An automatic cross-reference between opamp and comparator part numbers and LT's own devices. eg, select "TL081" from the list, but get given the nearest LT device..... LTxxxx if an exact pin for pin equivalent, (LTxxxx) if it is a nearly but not quite equivalent. If given the part numbers I don't mind calling up LT devices as 'payment' for LTspice.  SignatureTony Williams. >> Using LTspice solved the problem. > [quoted text clipped - 10 lines] > pin for pin equivalent, (LTxxxx) if it is a > nearly but not quite equivalent. I suppose you want the moon on a stick as well. Kevin Aylward informationEXTRACT@anasoft.co.uk http://www.anasoft.co.uk SuperSpice, a very affordable Mixed-Mode Windows Simulator with Schematic Capture, Waveform Display, FFT's and Filter Design. > I suppose you want the moon on a stick as well. Hmm... Nice bit of selective editing. I'll just repeat the paragraph you cut out in order to make your snide little remark. "If given the part numbers I don't mind calling up LT devices as 'payment' for LTspice." SignatureTony Williams. >> I suppose you want the moon on a stick as well. > > Hmm... Nice bit of selective editing. > > I'll just repeat the paragraph you cut out > in order to make your snide little remark. It wasn't "snide". "Just to add to the LTspice wish-list" was what the comment was directed at. Snipping the following bit changed nothing. > "If given the part numbers I don't mind calling > up LT devices as 'payment' for LTspice." As a realist, I would never even contemplate a "wish" of what you suggested for a freebee product. I certainly use free software products, but my expectations of what I get for my money are rather limited. Any "little" feature, can end up being a massive amount of work. Kevin Aylward informationEXTRACT@anasoft.co.uk http://www.anasoft.co.uk SuperSpice, a very affordable Mixed-Mode Windows Simulator with Schematic Capture, Waveform Display, FFT's and Filter Design. >>>I suppose you want the moon on a stick as well. >> [quoted text clipped - 22 lines] > Windows Simulator with Schematic Capture, > Waveform Display, FFT's and Filter Design. ...don't snile when you can smarl? [snip] > As a realist, I would never even contemplate a "wish" of what you > suggested for a freebee product. I certainly use free software > products, but my expectations of what I get for my money are > rather limited. Any "little" feature, can end up being a massive > amount of work. You still don't see it. It's a suggestion that could be beneficial to LT. At rock bottom, LTspice is an aid to selling Linear Technology's products. The suggestion of a cross reference between other mfr's products and equivalent LT devices is intended to help LTspice to sell more LT devices. I repeat: If in LTspice I called up say a TL081, and got offered a similar LT device, then I would simulate with that and probably call up the LT device in the final BOM. That seems a fair way of 'paying' for what is an excellent free piece of software. SignatureTony Williams. > [snip] >> As a realist, I would never even contemplate a "wish" of what you [quoted text clipped - 18 lines] > in the final BOM. That seems a fair way of 'paying' > for what is an excellent free piece of software. Hello Tony, the benfit for LT would be low. LTspice tries to make "unique" opamps. Unique means they have one or more better specs than you get from standard parts. This may result in a higher price for such better parts. If people have the cheapest parts of the world (TL082) in mind, they can't afford anything more expensive. It's so simple to add any third party model. The only additional thing to do is adding a ".include" command line. You don't need a new symbol for every other opamp! 1. Add the "opamp2" symbol. 2. Rename it the model name(opamp2) in the schematic, e.g. opamp2 to TL082 . 3. Add this command line: .include model_file_name 4. Place the model_file in the directory where you have saved the schematic. Best Regards, Helmut PS: I am not an employee of LT if that matters. > Hello Tony, > the benfit for LT would be low. LTspice tries to make > "unique" opamps. Unique means they have one or more > better specs than you get from standard parts. Hmm... perhaps that is why the Linear View 3 CDROM (which I bought as a result of LTspice) also does not carry any cross references. > This may result in a higher price for such better parts. > If people have the cheapest parts of the world (TL082) > in mind, they can't afford anything more expensive. I chose a wrong example Helmut. I'm fortunate to be in a branch of electronics (avionics ATE), where being well within spec and bullet proof is far more important than the cost of an ic. So an LT part that models properly in LTspice (even at N times the price) is ok. [snip] > PS: I am not an employee of LT if that matters. I know. Thank you for your remarks. SignatureTony Williams. > [snip] >> As a realist, I would never even contemplate a "wish" of what you [quoted text clipped - 4 lines] > > You still don't see it. Oh? > It's a suggestion that could be beneficial to LT. It may well be, but its a return on investment. *How* beneficial would it be to LT? > At rock bottom, LTspice is an aid to selling Linear > Technology's products. The suggestion of a cross [quoted text clipped - 7 lines] > in the final BOM. That seems a fair way of 'paying' > for what is an excellent free piece of software. I also repeat "Any little feature, can end up being a massive amounts of work." I've been there dude, I am still there. Sure, lots of things may be "useful". Whether or not it makes any business sense to do so is another matter. LTSpice is still only an *indirect* way to generate revenue. Maybe it could be cost effective to add more bells and whistles, but the impression I got was still this "looking a gift horse in the mouth" sort of thing. I suppose you also want fries with that? Kevin Aylward informationEXTRACT@anasoft.co.uk http://www.anasoft.co.uk SuperSpice, a very affordable Mixed-Mode Windows Simulator with Schematic Capture, Waveform Display, FFT's and Filter Design. huge snip] > I've been there dude, I am still there. Sure, lots of things may > be "useful". Whether or not it makes any business sense to do so [quoted text clipped - 3 lines] > "looking a gift horse in the mouth" sort of thing. I suppose you > also want fries with that? You can of course conveniently ignore any of the other posts I have made praising/recommending LTspice. SignatureTony Williams. >I suppose you also want fries with that? Sure. That would be a good feature. But not too often. Got a good model for my cholesterol with/without? > [snip] > [quoted text clipped - 19 lines] > in the final BOM. That seems a fair way of 'paying' > for what is an excellent free piece of software. And it is not difficult to do, it just takes time. So one mfg's product could be used as a starter, and others can be added on as time permits. An excellent initial candidate for replacement look-up is Maxim, as the majority of what they advertise is vaporware, and un-buidable articles causes frustration and excellent candidates as customers for parts that !can! be obtained. >>> Using LTspice solved the problem. >> [quoted text clipped - 20 lines] > Windows Simulator with Schematic Capture, > Waveform Display, FFT's and Filter Design. That is not within the confines of SPICE in general, so talk to NASA... >> Using LTspice solved the problem. > [quoted text clipped - 14 lines] > If given the part numbers I don't mind calling > up LT devices as 'payment' for LTspice. Excellent additions. In using LTspice somemore, i add: The output be in the same *order* that one has in the .PRINT statement. |
Reply to this Message |
 Sign In
 Join
 My Latest Posts My Monitored Threads My Blog My Photo Gallery My Profile My Homepage Start New Thread Enable EMail Alerts Rate this Thread
|
©2009 Advenet LLC Privacy Policy - Terms of Use
This website includes both content owned or controlled by Advenet as well as content owned or controlled by third parties.