Keyboard Shortcuts
ctrl + shift + ? :
Show all keyboard shortcuts
ctrl + g :
Navigate to a group
ctrl + shift + f :
Find
ctrl + / :
Quick actions
esc to dismiss
Likes
- LTspice
- Messages
Search
Re: Opamp models from Texas Instruments
Sven,
The simulation ( transient analysis )with the AD8009It looks like the problem is in the model. I ran the model in PSpice 9.2.3, the most recent version of the target simulator of the model, and got the same results. Here is a netlist based on your circuit that you can run in either LTspice or PSpice. I removed the power source impedances because PSpice doesn't handle those as part of voltage sources. You'll have to pick a different opamp or contact TI about the error in the model. Good luck. * THS4271.asc R1 N001 0 100 R2 out N001 100 V1 N005 0 PULSE(0 1 0 0.1n 0.1n 10n 20n) V2 0 N003 5 V3 N002 0 5 R3 N004 N005 0.1 XU1 N004 N001 N002 N003 out THS4271 .tran 0 20n 0 .inc TI.lib .probe .end --Mike __________________________________ Do you Yahoo!? SBC Yahoo! DSL - Now only $29.95 per month! |
No files were attached
Hello,
my attached files did't appear, so I try to add then to this post. Thank you again for any help. Sven Hegewisch The library: AD8009 SPICE model Rev B SMR/ADI 8-21-97 * Copyright 1997 by Analog Devices, Inc. * Node assignments * non-inverting input * | inverting input * | | positive supply * | | | negative supply * | | | | output * | | | | | .SUBCKT AD8009 1 2 99 50 28 * input stage * q1 50 3 5 qp1 q2 99 5 4 qn1 q3 99 3 6 qn2 q4 50 6 4 qp2 i1 99 5 1.625e-3 i2 6 50 1.625e-3 cin1 1 98 2.6e-12 cin2 2 98 1e-12 v1 4 2 0 * input error sources * eos 3 1 poly(1) 20 98 2e-3 1 fbn 2 98 poly(1) vnoise3 50e-6 1e-3 fbp 1 98 poly(1) vnoise3 50e-6 1e-3 * slew limiting stage * fsl 98 16 v1 1 dsl1 98 16 d1 dsl2 16 98 d1 dsl3 16 17 d1 dsl4 17 16 d1 rsl 17 18 0.22 vsl 18 98 0 * gain stage * f1 98 7 vsl 2 rgain 7 98 2.5e5 cgain 7 98 1.25e-12 dcl1 7 8 d1 dcl2 9 7 d1 vcl1 99 8 1.83 vcl2 9 50 1.83 gcm 98 7 poly(2) 98 0 30 0 0 1e-5 1e-5 * second pole * epole 14 98 7 98 1 rpole 14 15 1 cpole 15 98 2e-10 * reference stage * eref 98 0 poly(2) 99 0 50 0 0 0.5 0.5 ecmref 30 0 poly(2) 1 0 2 0 0 0.5 0.5 * vnoise stage * rnoise1 19 98 4.6e-3 vnoise1 19 98 0 vnoise2 21 98 0.53 dnoise1 21 19 dn fnoise1 20 98 vnoise1 1 rnoise2 20 98 1 * inoise stage * rnoise3 22 98 8.18e-6 vnoise3 22 98 0 vnoise4 24 98 0.575 dnoise2 24 22 dn fnoise2 23 98 vnoise3 1 rnoise4 23 98 1 * buffer stage * gbuf 98 13 15 98 1e-2 rbuf 98 13 1e2 * output current reflected to supplies * fcurr 98 40 voc 1 vcur1 26 98 0 vcur2 98 27 0 dcur1 40 26 d1 dcur2 27 40 d1 * output stage * vo1 99 90 0 vo2 91 50 0 fout1 0 99 poly(2) vo1 vcur1 -9.27e-3 1 -1 fout2 50 0 poly(2) vo2 vcur2 -9.27e-3 1 -1 gout1 90 10 13 99 0.5 gout2 91 10 13 50 0.5 rout1 10 90 2 rout2 10 91 2 voc 10 28 0 rout3 28 98 1e6 dcl3 13 11 d1 dcl4 12 13 d1 vcl3 11 10 -0.445 vcl4 10 12 -0.445 .model qp1 pnp() .model qp2 pnp() .model qn1 npn() .model qn2 npn() .model d1 d() .model dn d(af=1 kf=1e-8) .ends * [Disclaimer] (C) Copyright Texas Instruments Incorporated 1999 All rights reserved * * THS4271 High Speed amplifier "macromodel" subcircuit * updated using Model Editor release 9.2 on 11/05/02 at 13:11 * The Model Editor is a PSpice product. * * connections: non-inverting input * | inverting input * | | positive power supply * | | | negative power supply * | | | | output * | | | | | *$ .subckt THS4271 1 2 3 4 5 *Offset and CMRR Vos 1a 9 .005 Ios 1 2 .5u * upper Vic range limit drc1 16 17 dx drc2 16 18 dx Vcp 3 16 dc -0.4 * input stage rc1 17 11 176.8 rc2 18 12 176.8 L- 2 2a .8n q1 11 2a 13 qx1 L+ 1 1a .8n q2 12 9 14 qx1 re1 13 10 159.07 re2 14 10 159.07 Cdif 1 1c 0.8p Rcdf 1c 2 50 Ccm 2 2b 0.4p Rccm 2b 99 50 * lower Vic range limit d10 15 10 dx v10 15 4 dc 1.2 Iee 10 4 dc 3e-3 Icc 3 4 15m Rcc 3 4 2500 * gain stage and dominant pole Ga 21 99 value = {(limit(V(11,12),-.447,.447))*-35.6m} ra 21 99 158k ca 21 99 15.9E-12 * GAIN STAGE SWING LIMIT DPC 21 23 dx VPC 3 23 1.7 DNC 24 21 dx VNC 24 4 1.74 * zero ez 26 99 21 99 10 rz1 26 27 -900 cz 26 27 .2p rz2 27 99 -100 * phase shift stage gps 25 99 27 99 -100.0E-6 rps 25 99 10.0E3 cps 25 99 10E-15 Egnd 99 0 poly(2) 3 0 4 0 0 .5 .5 X_OP 25 99 3 4 5a THS4271_OP Ro 5a 5b .1 Lo 5b 5 .2n Rco 5c 99 10 Co 5 5c .8p .ends *$ * Output stage * connections: non-inverting input * | inverting input * | | positive power supply * | | | negative power supply * | | | | output * | | | | | .subckt THS4271_OP 1 2 3 4 5 * GAIN STAGE SWING LIMIT DOPC 1 38 dx VOPC 3 38 1. DONC 48 1 dx VONC 48 4 1. * UPPER DRIVE STAGE ROP 3 34 8.5 HLP2 34 33 VLP 30 VOP 33 32 0 HLP1 35 0 VOP 8 RLP 35 36 8 DLP 36 37 dx VLP 37 0 0 EOP 32 31 Poly(2) 2 1 3 4 -.8 1 .5 DOP 31 5 dx * LOWER DRIVE STAGE DON 5 41 dx EON 41 42 Poly(2) 1 2 3 4 -.8 1 .5 VON 42 43 0 HLN1 45 0 VON 15 RLN 45 46 8 DLN 46 47 dx VLN 47 0 0 HLN2 43 44 VLN 45 RON 44 4 12 .ends *$ *DIODE MODELS .model dx D(Is=800.00E-18) *$ .model qx1 NPN(Is=800.00E-18 Bf=272.73 af=0 kf=9e-22) *.model qx1 NPN(Is=800.00E-18 Bf=272.73 af=2 kf=8e-8) *$ Please note that the disclaimers and copyright notices are shorted! The circuit with AD8009: Version 4 SHEET 1 880 680 WIRE -320 176 -80 176 WIRE -80 80 -80 176 WIRE -80 176 0 176 WIRE 0 80 144 80 WIRE 144 80 144 192 WIRE 144 192 64 192 WIRE 144 192 240 192 WIRE 32 160 32 144 WIRE 32 352 32 336 WIRE 240 192 288 192 WIRE -80 208 0 208 WIRE -224 288 -224 208 WIRE -224 208 -160 208 WIRE 192 336 192 320 WIRE 192 432 192 416 WIRE 32 240 32 224 FLAG -320 256 0 FLAG -224 368 0 FLAG 32 432 0 FLAG 192 320 0 FLAG 240 192 out FLAG 32 144 v+ FLAG 192 432 v+ FLAG 32 240 v- FLAG 32 336 v- SYMBOL res -336 160 R0 SYMATTR InstName R1 SYMATTR Value 100 SYMBOL res 16 64 R90 WINDOW 0 0 56 VBottom 0 WINDOW 3 32 56 VTop 0 SYMATTR InstName R2 SYMATTR Value 100 SYMBOL voltage -224 272 R0 WINDOW 123 24 132 Left 0 WINDOW 39 0 0 Left 0 WINDOW 3 -402 89 Left 0 SYMATTR Value2 AC 0.1 SYMATTR Value PULSE(0 1 0 0.1n 0.1n 10n 20n 1) SYMATTR InstName V1 SYMBOL voltage 32 448 R180 WINDOW 0 24 104 Left 0 WINDOW 3 24 16 Left 0 WINDOW 123 0 0 Left 0 WINDOW 39 24 -12 Left 0 SYMATTR InstName V2 SYMATTR Value 5 SYMATTR SpiceLine Rser=0.1 SYMBOL voltage 192 432 R180 WINDOW 0 24 104 Left 0 WINDOW 3 24 16 Left 0 WINDOW 123 0 0 Left 0 WINDOW 39 24 76 Left 0 SYMATTR InstName V3 SYMATTR Value 5 SYMATTR SpiceLine Rser=0.1 SYMBOL res -64 192 R90 WINDOW 0 0 56 VBottom 0 WINDOW 3 32 56 VTop 0 SYMATTR InstName R3 SYMATTR Value 0.1 SYMBOL Opamps\\AD8009 32 128 R0 SYMATTR InstName U1 TEXT -226 506 Left 0 !.tran 0 20n 0 The circuit with THS4271: Version 4 SHEET 1 880 680 WIRE -320 176 -80 176 WIRE -80 80 -80 176 WIRE -80 176 0 176 WIRE 0 80 144 80 WIRE 144 80 144 192 WIRE 144 192 64 192 WIRE 144 192 240 192 WIRE 32 160 32 144 WIRE 32 352 32 336 WIRE 240 192 288 192 WIRE -80 208 0 208 WIRE -224 288 -224 208 WIRE -224 208 -160 208 WIRE 192 336 192 320 WIRE 192 432 192 416 WIRE 32 240 32 224 FLAG -320 256 0 FLAG -224 368 0 FLAG 32 432 0 FLAG 192 320 0 FLAG 240 192 out FLAG 32 144 v+ FLAG 192 432 v+ FLAG 32 240 v- FLAG 32 336 v- SYMBOL res -336 160 R0 SYMATTR InstName R1 SYMATTR Value 100 SYMBOL res 16 64 R90 WINDOW 0 0 56 VBottom 0 WINDOW 3 32 56 VTop 0 SYMATTR InstName R2 SYMATTR Value 100 SYMBOL voltage -224 272 R0 WINDOW 123 24 132 Left 0 WINDOW 39 0 0 Left 0 WINDOW 3 -402 89 Left 0 SYMATTR Value2 AC 0.1 SYMATTR Value PULSE(0 1 0 0.1n 0.1n 10n 20n 1) SYMATTR InstName V1 SYMBOL voltage 32 448 R180 WINDOW 0 24 104 Left 0 WINDOW 3 24 16 Left 0 WINDOW 123 0 0 Left 0 WINDOW 39 24 -12 Left 0 SYMATTR InstName V2 SYMATTR Value 5 SYMATTR SpiceLine Rser=.1 SYMBOL voltage 192 432 R180 WINDOW 0 24 104 Left 0 WINDOW 3 24 16 Left 0 WINDOW 123 0 0 Left 0 WINDOW 39 24 76 Left 0 SYMATTR InstName V3 SYMATTR Value 5 SYMATTR SpiceLine Rser=.1 SYMBOL res -64 192 R90 WINDOW 0 0 56 VBottom 0 WINDOW 3 32 56 VTop 0 SYMATTR InstName R3 SYMATTR Value 0.1 SYMBOL Opamps\\THS4271 32 128 R0 SYMATTR InstName U1 TEXT -226 506 Left 0 !.tran 0 20n 0 ________________________________________________________________________ Send free SMS using the Yahoo! Messenger. Go to |
Opamp models from Texas Instruments
Hello,
first let me than you for this nice program. I am rather new to simulation programs so I ran into some difficulties. I try to simulate a small circuit with two different opamps, the AD8009 from Analog Devices and the THS4271 from Texas Instruments. I downdloaded both models from the net and made a library with them which I put in the standard library folder. The simulation ( transient analysis )with the AD8009 works as expected. But the THS4271 produces just junk. After some 500 ps the output will be some Megavolts. The AC analysis on the other hand looks ok. After several days of try and still error I don't know what I am doing wrong. Every help will be appreciated. The circuits have the filenames THS4271t.asc and AD8009t.asc and the library has the name opa.lib. They are attached to this post. Thank you Sven Hegewisch ________________________________________________________________________ Send free SMS using the Yahoo! Messenger. Go to |
Re: Rotating components when placing in schematic
Howie, Brian (UK)
In Eagle (by CadSoft) I can rotate components by clicking the right Control R does it. Brian *** This email and any attachments are confidential to the intended recipient and may also be privileged. If you are not the intended recipient please delete it from your system and notify the sender. You should not copy it or use it for any purpose nor disclose or distribute its contents to any other person. *** |
Rotating components when placing in schematic
telyn_de
Hello,
my name is Michael and I'm designing stage control systems for theaters, opera houses etc. I've been using LTSpice only for a few days by now (after been completely unsatisfied with CircuitMaker 5 schematic editor). Now my question: Is there any easy way (other than clicking the Rotate Button) to rotate components when placing ? In Eagle (by CadSoft) I can rotate components by clicking the right mouse button before placing. Would be a nice feature in LTSpice, too. Greeting from Germany Michael |
Re: What does 'Fatal Error: doAnalyses: Iteration limit reached' mean?
Massimo,
Please can you report some additional information about the alternateThe alternate solver uses a sparse matrix package that accumulates much less internal round-off error. The new sparse solver uses (what I call) a vertical solution method. It runs at about half the simulation speed but 1000x more accurately as far as the matrix solution goes in the test cases that caused the investigation. For practical circuits, there's no need for it. But some opamp macro models use unphysical components that lead to a difficult-to-solve linearized circuit matrix. I found three ways to solve the problem, but only released the method to use a more accurate sparse matrix solver that has less round- off error because (i) it was of the most general use and (ii) it's the hardest for other SPICE programs to duplicate. This also gives a nice diagnostic that allows one to check if numerical round-off is an issue by switching between solvers. I think it's an interesting, very high-power means to solve the problem and I don't know of any other SPICE in academia or commerce that uses this vertical solution technology. Intellectual property concerns don't allow me to feel comfortable revealing the theory behind the implementation, but you should find the operation to be exactly as I describe. Besides the sparse matrix solver, there is no other intended difference between the two SPICE solvers in the current release. There's basically two copies of LTspice in the executable because the new matrix solver is not compatible with the old one so a copy of LTspice had to be modified to work with it. Anyway, I recommend only using the normal solver unless you run into singular matrix issues. The normal solver usually will be just as accurate as the alternate solver since round- off error in the sparse matrix is rarely the limiting factor to the accuracy of your circuit's solution. If you develop macro models for others to use in possibly other simulators, I definately recommend that you use the normal solver, or could end up with a model that only LTspice can solve. But of course I appreciate people testing both solvers and reporting any un-intended differences between them. It was a huge reorganization of the code to have two versions of LTspice in the same executable. I find the feedback I get from this, other groups, and individually extremely valuable to the quality of the program. --Mike __________________________________ Do you Yahoo!? SBC Yahoo! DSL - Now only $29.95 per month! |
Re: What does 'Fatal Error: doAnalyses: Iteration limit reached' mean?
Dear Mike,
toggle quoted message
Show quoted text
Please can you report some additional information about the alternate solver? Which are the main differences between the two solvers? Is it possible to understand why you have added this new solver? Are there some limitations in the old one? Which are the circuits in which the new solvers is more accurate? Thanks Massimo Panama Mike wrote: I wrote: --
''~`` ( o o ) +------------------.oooO--(_)--Oooo.------------------+ | | | e-mail: gaspari@... | | | | ICQ # = 166939207 | | | | PGP fingerprint16: | | 76 80 F2 F9 8D 70 F3 D1 42 2B CD 80 29 49 CB 25 | | | | .oooO | | ( ) Oooo. | +---------------------\ (----( )--------------------+ \_) ) / (_/ |
Re: Symbol Creation
Steve Steckler
Thanks Mike Panama Mike wrote: Steve, Do you Yahoo!? - Now only $29.95 per month! |
Re: Symbol Creation
Steve,
Just an observation of a very minor issue that LT is probablyThank you very much for reporting this. The fix will be availible when the next minor update is released. --Mike __________________________________ Do you Yahoo!? SBC Yahoo! DSL - Now only $29.95 per month! |
Re: Models for BB INA111AP
D Chisholm
I have models for the INA111 from an old Burr-Brown databook (pre-Texas Instruments). They seem to have produced 3 versions: a Basic model, called ".SUBCKT INA111/BB"; an "Enhanced" model, called ".SUBCKT INA111E/BB"; and another enhanced model called ".SUBCKT INA111Z/BB". About 30K bytes (over 500 lines) altogether for the 3. These are probably the same models you will get from TI, but I assembled them into a single file & posted to this group under the "Files>Lib>Sub" heading.
toggle quoted message
Show quoted text
p.s. - You might still find the whole collection of Burr-Brown models at <ftp://nyquist.ee.ualberta.ca/pub/cookbook/spice/> or some other site that actually archives files, rather than linking to the manufacturer's current web pages. Hao Fu wrote: Hi, |
Re: Models for BB INA111AP
--- In LTspice@..., "Hao Fu" <fuhao@y...> wrote:
Hi,Hello Hao, there is a SPICE model on the TI website. Nobody would do the work on it a second time. genericPartNumber=INA111 genericPartNumber=INA111&pfsection=models The only thing you need now is a symbol for LTSPICE. Take care to number the value of "Netlist order" according to the parameter order in the subcircuit definition of the model file. Now some hints about file organization depending on the value of "SpiceModel" in the symbol file. If you reference the "SpiceModel" with a file name without path, then this model file has to be either in the LTSPICE "...\Lib\Sub" directory or in the working directory of your schematic file(*.asc). If you specify a drectory path too("xyz\abc.mod"), then it has to be in "...\Lib\xyz\abc.mod". I have added the INA111 symbol, model and a test circuit under this group's File->Lib directory. You could read additionally my last posting about the INA103 model and probably some of my earlier postings which also explain how to make symbol files. Overall it was not clear for me whether you have wanted to use the TI- model or you try to make a model from the data sheet. I hope I could help you. Best Regards Helmut |
Re: Models for BB INA111AP
Jonathan Kirwan
On Sun, 15 Jun 2003 07:52:24 -0000, you wrote:
It seems that this device is not among the existing examples inI'm no expert on this, but it would seem that your needs would depend on which model you can accept. There are three Ebers-Moll models I'm familiar with, but the help file for LTSpice only mentions "the Ebers-Moll." I guess it just depends on which parameters you want to specify. EM1 has an injection version, a transport version, and a nonlinear hybrid-pi version. They use the forward beta (Bf), reverse beta (Br), saturation current (Is, which is usually just a hypothetical value designed to minimize errors against a realistic curve of behavior), the nominal temperature (Tnom), and the energy gap (Eg.) The energy gap is used to modify Is over temperature. For these parameters, you just need to look at a curve trace which shows the collector current vs the collector-emitter voltage for a fixed base-current drive. Select the Bf value found on the desired I(B) curve at the point where I(C) and V(CE) are at the values you intend to operate the transistor. Use the DC value, not the AC value. Br can just be set to 1, if you aren't going to operate it that way or else you can try and find a curve with the emitter and collector leads interchanged and pick off the right value for Br. Is is more complex. You can use a numerical method for this, if you capture some complete curves. But it is often just set to arbitrary values like 1E-16 or else measured by considering a simple relationship when the transistor is in the normal, active region and zero-biased base-collector junction. In this case, you use the standard Ebers-Moll equation, I(C)=I(S)*(e^((q*V(BE))/(k*T))-1), and solve for I(S) (Is.) Eg is typically 1.11eV for silicon but its often obtained by curve-fitting Is. This would probably take some effort on your part, as the required information isn't usually present on a data sheet for this. You might also steal it from some similar transistor or else ignored if you assume you will operate the transistor at the specified Is value. EM2 uses EM1's parameters and adds the emitter ohmic resistance (Re), the collector ohmic resistance (Rc), the base ohmic resistance (Rb), the zero-bias emitter-base junction capacitance (CJEO or CJE) and barrier potential and gradient factor, the zero-bias collector-base junction capacitance (CJCO or CJC) and barrier potential and gradient factor, the forward transit time (Tf), the reverse transit time (Tr), and the substrate capacitance (Csub). I think you'd need a curve tracer, capacitance bridge, power supply, pulse generator, and a small signal measurement system at a minimum. I don't think all these can be fetched from a typical data sheet. EM3 adds more, and so does Gummel-Poon. It gets really hairy at this point. My guess is that a data sheet is good for EM1, and even that is only without really getting a good bead on Eg unless you determine it by fiat. But like I said, I've only played around with this a little bit with just a couple of unmarked transistors, for the fun of it. I don't have good experience at this. I'll be reading to see if someone can wisely point out some good techniques for better modeling from data sheet curves. Best of luck, Jon |
Models for BB INA111AP
Hi,
It seems that this device is not among the existing examples in LTspice. This device is primarily used for medical instrumentation and data acquisition. Can someone tell me what it takes to make a custom model for it? What is the minimum number of parameters from its data sheet that should be taken into account? Thanks, Hao |
Re: Oscillator
Al Williams
--- In LTspice@..., "Helmut Sennewald"
<helmutsennewald@y...> wrote: --- In LTspice@..., "Al Williams" <alw@a...> wrote:simulator.I put the ASC file in the Files section. The simulation time isHello Al, Accidentally by far not all paramaters can be controlled from thetoo. Thanks! I'm not sure where this file came from. I thought it was installed as part of LTSpice, but maybe I got it somewhere else. It isn't mine :-) I was simply trying to see if I could simulate it. |
Re: Oscillator
--- In LTspice@..., "Al Williams" <alw@a...> wrote:
I put the ASC file in the Files section. The simulation time isHello Al, I modified your oscillator circuit and added also some comments. It is very important to have well defined settings for the simulator. Accidentally by far not all paramaters can be controlled from the schematic or the netlist. This is a very bad drawback of LTSPICE. I would appreciate to have commands for all simulator settings. Setup the Simulator: The points 1 to 4 are the most important actions. 1. Control Panel->Spice->Reset to Default 2. Control Panel->Hacks->Reset to Default 3. Control Panel Hacks->Supply a min. inductor damping->click off 4. Don't use integration method Gear. It tends to let die the oscillation of this crystal oscillator. 5. Start your simulations with a lower Q of the crystal to reduce turnaround time during development of your circuit. Later you can increase Q and simulation time. My new schematic file is in the Files->Examples->Educational Menu too. By the way, this is not the best type of one transistor oscillator for 12Mhz. There are better suited circuits. Best Regards Helmut Pierce_12Mhz_r.asc: You have to repair the two broken long lines with a text editor. .TEXT 728 324 ..... .TEXT 728 524 ..... You can find this file in the Files->Examples->Educational folder too. Version 4 SHEET 1 2020 1396 WIRE 1248 752 1280 752 WIRE 1344 752 1376 752 WIRE 1136 656 1136 752 WIRE 1328 1040 1136 1040 WIRE 1136 752 1136 1040 WIRE 1392 992 1392 960 WIRE 1392 960 1472 960 WIRE 1920 1232 1920 1344 WIRE 1920 1344 1568 1344 WIRE 1408 1344 1408 1376 WIRE 1440 1200 1440 1232 WIRE 1440 1344 1408 1344 WIRE 1344 1344 1408 1344 WIRE 1440 1136 1440 1104 WIRE 1440 1104 1392 1104 WIRE 1392 1104 1392 1088 WIRE 1344 1344 1136 1344 WIRE 800 960 800 1088 WIRE 640 1344 800 1344 WIRE 800 1344 944 1344 WIRE 944 960 800 960 WIRE 688 960 640 960 WIRE 640 960 640 1056 WIRE 800 1152 800 1344 WIRE 640 1136 640 1344 WIRE 944 1056 944 960 WIRE 944 1344 944 1248 WIRE 944 1136 944 1152 WIRE 1136 1040 1136 1136 WIRE 944 1152 944 1168 WIRE 1344 1216 1344 1344 WIRE 1344 1136 1344 1104 WIRE 1344 1104 1392 1104 WIRE 1232 656 1136 656 WIRE 1472 656 1296 656 WIRE 1136 752 1168 752 WIRE 1456 752 1472 752 WIRE 1472 752 1472 656 WIRE 800 960 768 960 WIRE 1232 960 944 960 WIRE 1312 960 1392 960 WIRE 1344 1056 1328 1056 WIRE 1328 1056 1328 1040 WIRE 1568 992 1568 960 WIRE 1568 960 1472 960 WIRE 1568 1056 1568 1104 WIRE 1568 1344 1440 1344 WIRE 1568 1216 1568 1344 WIRE 1568 1104 1568 1152 WIRE 1920 1104 1568 1104 WIRE 1920 1104 1920 1152 WIRE 1136 1200 1136 1344 WIRE 1136 1344 944 1344 WIRE 992 1152 992 1040 WIRE 992 1152 944 1152 WIRE 992 1040 1136 1040 WIRE 1472 960 1472 752 WIRE 1440 1312 1440 1344 FLAG 1408 1376 GND FLAG 1920 1104 Output SYMBOL voltage 640 1040 R0 SYMATTR InstName V1 SYMATTR Value 12 SYMBOL res 784 944 R90 WINDOW 0 0 56 VBottom 0 WINDOW 3 32 56 VTop 0 SYMATTR InstName R1 SYMATTR Value 100 SYMBOL res 960 1152 R180 WINDOW 0 36 76 Left 0 WINDOW 3 36 40 Left 0 SYMATTR InstName R2 SYMATTR Value 10k SYMBOL res 960 1264 R180 WINDOW 0 36 76 Left 0 WINDOW 3 36 40 Left 0 SYMATTR InstName R3 SYMATTR Value 10k SYMBOL cap 784 1088 R0 SYMATTR InstName C1 SYMATTR Value 100n SYMBOL cap 1120 1136 R0 WINDOW 3 25 60 Left 0 SYMATTR InstName C2 SYMATTR Value 33p SYMBOL res 1904 1136 R0 SYMATTR InstName R4 SYMATTR Value 50 SYMBOL ind 1264 736 R90 WINDOW 0 5 56 VBottom 0 WINDOW 3 32 56 VTop 0 SYMATTR InstName L0 SYMATTR Value {L0} SYMBOL cap 1344 736 R90 WINDOW 0 0 32 VBottom 0 WINDOW 3 32 32 VTop 0 SYMATTR InstName C0 SYMATTR Value {C0} SYMBOL cap 1296 640 R90 WINDOW 0 0 32 VBottom 0 WINDOW 3 32 32 VTop 0 SYMATTR InstName Cp SYMATTR Value 5p SYMBOL res 1472 736 R90 WINDOW 0 0 56 VBottom 0 WINDOW 3 32 56 VTop 0 SYMATTR InstName R0 SYMATTR Value {R0} SYMBOL cap 1424 1136 R0 SYMATTR InstName C7 SYMATTR Value 10n SYMBOL res 1328 1120 R0 SYMATTR InstName R6 SYMATTR Value 1k SYMBOL res 1216 976 R270 WINDOW 0 32 56 VTop 0 WINDOW 3 0 56 VBottom 0 SYMATTR InstName R7 SYMATTR Value 1k SYMBOL cap 1552 992 R0 SYMATTR InstName C9 SYMATTR Value 33p SYMBOL cap 1552 1152 R0 SYMATTR InstName C10 SYMATTR Value 2.2n SYMBOL res 1424 1216 R0 SYMATTR InstName R8 SYMATTR Value 1 SYMBOL npn 1328 992 R0 SYMATTR InstName Q1 SYMATTR Value 2N2369 TEXT 736 736 Left 0 !.tran 0 3m 0 0.005u TEXT 736 768 Left 0 !.IC I(L0)=1e-24 TEXT 728 384 Left 0 ;Setup the Simulator:\n1. Control Panel->Spice- Reset to Default\n2. Control Panel->Hacks->Reset to Default\n3.Control Panel Hacks->Supply a min. inductor damping->click off\n4. Don't use integartion method Gear. It tends to let die the oscillation.\n5. Start your simulations with a lower Q of the crystal to reduce startup simulation time. TEXT 728 584 Left 0 !.PARAM f0=12e6\n.PARAM Q=50000\n.PARAM R0=60 \n.PARAM L0={Q*R0/(2*pi*f0)}\n.PARAM C0={1/(2*pi*f0*Q*R0)} |
Re: Pierce Oscillator
Al Williams
That's strange. On my screen the Cs is 1.75fF not 250f and a .1H Ls.
I wonder if I have some file out of sync. --- In LTspice@..., "leckerts" <leckerts@y...> wrote: Al,capacitor.
|
Pierce Oscillator
leckerts
Al,
I just looked at the Pierce oscillator under the Educational directory. It has a 0.001 Henry series inductor and a 0.25 pF series capacitor. 2/(2pi sqrt(.001 x .25x10-12)) = 10.07 MHz. When I simulated the circuit I noticed that the output circuit doubles the frequency of the oscillator. So twice 10.07 would be 20.14 MHz which is pretty close. Steve |
Oscillators
leckerts
Gentlemen,
I have simulated a lot oscillators in my day. I've used Cadence's Spectre as well as LTSpice. Oscillators tend to be difficult to simulate because of several factors. Very often, at higher frequencies, you need to change the maximum time step or they won't work at all. Also, you can usually speed up the startup of a crystal oscillator by an order of magnitude by shocking the crystal resonator with a pulsed current source. I noticed that it seems that the maximum RAW file size of the LT simulator has been increased which is important for oscillator simulations. It used to complain if the simulation went too long and the file went over some limit. Steve Sr. Engineering Manager (Ex and looking) TLSI Inc. |
Re: Oscillator
Al Williams
I put the ASC file in the Files section. The simulation time is
quite long, but it seemed to stablize around 30uS or so. Al W. --- In LTspice@..., "Helmut Sennewald" <helmutsennewald@y...> wrote: --- In LTspice@..., "Al Williams" <alw@a...> wrote:wasI was playing with pierce.asc -- as far as I can remember, this 21.114a sample provided with the program (I think). extent.MHz. Why is that? The quasi-crystal has L=.1, Rs=600, Cs=1.75fF, ISo is this a spice problem where other components are moving the anymissing something obvious?Hello Al, used. I have simulated crystal oscillators in the past and theydid run at the crystal frequency. Be aware of very long startup times. |
to navigate to use esc to dismiss