csx18@seq1.keele.ac.uk (C.M. Yearsley) (02/13/91)
I've just started using SPICE and would greatly appreciate any
standard subcircuits people could point me to. Specifically I
need to simulate a TL072 op-amp, among other things. I'm using
version 2G5 if that makes any difference.
--
----------------------------------------------------------------------------
Chris Yearsley JANET: csx18@uk.ac.keele.seq1
USENET: csx18@seq1.keele.ac.ukmcovingt@athena.cs.uga.edu (Michael A. Covington) (02/13/91)
Texas Instruments gives out, for free or for a low price, a set of SPICE models of op-amps including the TL072.
terryb.bbs@shark.cs.fau.edu (terry bohning) (02/13/91)
mcovingt@athena.cs.uga.edu (Michael A. Covington) writes: > Texas Instruments gives out, for free or for a low price, a set > of SPICE models of op-amps including the TL072. PMI (Precision Monolithics Inc.) does also. Theirs are free.
teodor@acsu.buffalo.edu (Dan C. Teodor) (02/13/91)
In article <881@keele.keele.ac.uk> you write: >I've just started using SPICE and would greatly appreciate any >standard subcircuits people could point me to. Specifically I >need to simulate a TL072 op-amp, among other things. I'm using >version 2G5 if that makes any difference. > Here's what I do. It's kind of messy but it works. First label either the non-inverting or inverting input to the op-amp as ground (ie. as node 0). Then leave the non-inverting and inverting input terminals disconnected on one end (ie. connect to the rest of the network nodes but leave them "dangling" on the other end). Then, model the op-amp as a voltage dependent voltage source with a potential of the op-amp's gain times the potential at the non-ground node that was left "dangling". I normally use a value to somewhere between 10,000 and 50,000 for the gain. Of course all of the above assumes an ideal op-amp with no bias current running through it's inputs. If you want to model a "realer" one see what the bias current of your op-amp is and calculate it's Thevenin equivalent resistance across the inputs (ie. R(th)=V/I). This is usually given in an op-amp's specs and no calculation is necessary. Once you know this equivalent resistance (usually about 1 Megaohm) just connect a resistor of this value across those "dangling" terminals and model as before. It all works out very nicely and it doesn't get any more accurate than that. Good luck. I'll try and give you some samples if this confuses the shit out of you. Dan C. Teodor teodor@sun.acsu.buffalo.edu v083pzgu@ubvms.cc.buffalo.edu P.S. I'm sorry to post this in this fashion but the return address on that message bounced. But this pretty much general info.
kahhan@bnr.ca (02/13/91)
In article <881@keele.keele.ac.uk> csx18@seq1.keele.ac.uk (C.M. Yearsley) writes: >I've just started using SPICE and would greatly appreciate any >standard subcircuits people could point me to. Specifically I >need to simulate a TL072 op-amp, among other things. I'm using >version 2G5 if that makes any difference. > >-- Chris, Check with Texas Instruments. They offer a disk with SPICE models of many OP-AMPs that they make. Other manufacturers offer free disks as well. Sure beats the heck out of using PARTS and keying in data from a spec sheet yourself (and it's probably more accurate). -- ---------------------------------------------------------------------------------- Larry Kahhan - NRA, NRA-ILA, CSG, GOA, GSSA | The opinions expressed here do | not necessarily represent the | views of the management of BNR ----------------------------------------------------------------------------------
stigvi@Lise.Unit.NO (Stig Vidar Hovland) (02/14/91)
In article <1991Feb13.124247.22948@bnr.ca>, kahhan@bnr.ca writes: |> Check with Texas Instruments. They offer a disk with SPICE models of many OP-AMPs |> that they make. Other manufacturers offer free disks as well. Sure beats the |> heck out of using PARTS and keying in data from a spec sheet yourself (and it's |> probably more accurate). |> If anyone have one of these free disks, can you please email me a copy of it. Stig Vidar Hovland - stigvi@lise.unit.no
goodloe@b11.ingr.com (Tony Goodloe) (02/20/91)
in article <881@keele.keele.ac.uk>, csx18@seq1.keele.ac.uk (C.M. Yearsley) says: > > I've just started using SPICE and would greatly appreciate any > standard subcircuits people could point me to. Specifically I > need to simulate a TL072 op-amp, among other things. I'm using > version 2G5 if that makes any difference. > > -- > ---------------------------------------------------------------------------- > Chris Yearsley JANET: csx18@uk.ac.keele.seq1 > USENET: csx18@seq1.keele.ac.uk Here is a model from TI. They have a DOS disk full of them, along with a data book. Get in touch with them at: Texas Instruments Inc. Literature Response Center P.O. Box 809066 Dallas 75380-9066 The name of the box and disk is "Linear Circuits - Operational Amplifier Macromodels" * TL072 operational amplifier "macromodel" subcircuit * created using Parts release 4.01 on 06/16/89 at 13:08 * (REV N/A) * connections: non-inverting input * | inverting input * | | positive power supply * | | | negative power supply * | | | | output * | | | | | .subckt TL072 1 2 3 4 5 * c1 11 12 3.498E-12 c2 6 7 15.00E-12 dc 5 53 dx de 54 5 dx dlp 90 91 dx dln 92 90 dx dp 4 3 dx egnd 99 0 poly(2) (3,0) (4,0) 0 .5 .5 fb 7 99 poly(5) vb vc ve vlp vln 0 4.715E6 -5E6 5E6 5E6 -5E6 ga 6 0 11 12 282.8E-6 gcm 0 6 10 99 8.942E-9 iss 3 10 dc 195.0E-6 hlim 90 0 vlim 1K j1 11 2 10 jx j2 12 1 10 jx r2 6 9 100.0E3 rd1 4 11 3.536E3 rd2 4 12 3.536E3 ro1 8 5 150 ro2 7 99 150 rp 3 4 2.143E3 rss 10 99 1.026E6 vb 9 0 dc 0 vc 3 53 dc 2.200 ve 54 4 dc 2.200 vlim 7 8 dc 0 vlp 91 0 dc 25 vln 0 92 dc 25 .model dx D(Is=800.0E-18) .model jx PJF(Is=15.00E-12 Beta=270.1E-6 Vto=-1) .ends