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: 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. |
Re: Spice model for 2SD2006, .......
manduur2000
Hi Jon,
toggle quoted message
Show quoted text
thanks for your help, Guenter --- In LTspice@..., Jonathan Kirwan <jkirwan@e...> wrote:
I found this: |
Re: Oscillator
--- In LTspice@..., "Al Williams" <alw@a...> wrote:
I was playing with pierce.asc -- as far as I can remember, this wasHello Al, please post your circuit *.asc file and the subcircuit models if any used. I have simulated crystal oscillators in the past and they did run at the crystal frequency. Be aware of very long startup times. Best Regards Helmut |
Oscillator
Al Williams
I was playing with pierce.asc -- as far as I can remember, this was
a sample provided with the program (I think). Doing a transient analysis on it shows that it oscillates at 21.114 MHz. Why is that? The quasi-crystal has L=.1, Rs=600, Cs=1.75fF, Cp=5pF. The series resonance should be 1/(2pi*sqrt(L*Cs)) Parallel resonance should be 1/2pi*sqrt(L*Cx)) where Cx=(Cs*Cp)/(Cs+Cp) So Cx=1.749fF (almost no difference from Cs) and Fs=12.031MHz Fp=12.033MHz External components might pull the crystal, but not to that extent. So is this a spice problem where other components are moving the resonant frequency even though in real life it would not? Or am I missing something obvious? What am I doing wrong? Regards, Al Williams |
Re: Spice model for 2SD2006, .......
D Chisholm
Fairchild will email a PSPICE model file for the TIP110. Request it here:
toggle quoted message
Show quoted text
<> Or try: .SUBCKT TIP110 1 2 3 * TERMINALS: C B E * Darlington NPN Q1 1 2 4 QPWR .1 Q2 1 4 3 QPWR R1 2 4 8K R2 4 3 60 D1 3 1 DSUB .MODEL QPWR NPN (IS=2.4P NF=1 BF=142 VAF=139 IKF=2.4 ISE=168P NE=2 BR=4 NR=1 VAR=20 IKR=3.6 RE=.45 RB=1.8 RC=.18 XTB=1.5 CJE=382P VJE=.74 MJE=.45 CJC=48.7P VJC=1.1 MJC=.24 TF=85.3N TR=3.68U) .MODEL DSUB D (IS=2.4P N=1 RS=.45 BV=60 IBV=.001 CJO=48.7P TT=3.68U) .ENDS .MODEL Q2SC2655 NPN (IS=203F NF=1 BF=195 VAF=127 IKF=1.2 ISE=104P NE=2 BR=4 NR=1 VAR=20 IKR=1.8 RE=35.7M RB=.143 RC=14.3M XTB=1.5 CJE=220P VJE=1.1 MJE=.5 CJC=71P VJC=.3 MJC=.3 TF=1.59N TR=1.1U) manduur2000 wrote: Hello, |
Re: Spice model for 2SD2006, .......
Jonathan Kirwan
On Sat, 14 Jun 2003 14:48:52 -0000, you wrote:
where can I find the spice model?s for these transistors:I found this: .MODEL 2SC2655 NPN( + IS=8.8111E-15 + BF=164 + VAF=100 + IKF=6.3687 + XTB=1.5 + ISE=68.197E-15 + NE=1.4705 + BR=10.573 + VAR=100 + IKR=91.376E-3 + ISC=26.265E-12 + NC=2.0018 + NK=.4398 + RC=47.627E-3 + CJE=2.0000E-12 + CJC=72.874E-12 + MJC=.33333 + TF=437.89E-12 + XTF=10 + VTF=10 + ITF=1 + TR=190.47E-9) The others I don't have handy. Jon |
Symbol Creation
leckerts
This is not a complaint, since we're all happy to have this tool!
Just an observation of a very minor issue that LT is probably aware of - When creating an IC symbol (I was drawing a 64-pin LQFP)and when inserting pins which are vertically oriented, there are occasionally trailing graphics when these pins are placed. I notice it usually happens after 6 or 7 vertically oriented pins have been placed. Keep up the great work! Steve |
Re: request -- Help On INA 103 and using vendor spice models
Thank you very much Helmut for u time.
I am sorry that took too long. I was able to use INA 103 and learning more. Still having problems in simulation .AC ....but more after i try more.. Thanks once again regards ranga rajan Besr RegardsG100 .SUBCKT INA103 1 2 3 4 5 8 9 10 109 110 11 12 105111
|
Re: What does 'Fatal Error: doAnalyses: Iteration limit reached' mean?
I wrote:
...The fix is not yet in the general releaseThis MOS3 fix and the alternate solver with the new sparse matrix package is now in the general release. This makes the above mentioned url obsolete and no longer available. Version 2.03h implements a major reorganization of most of the underlying code. Please report any problems you might encounter as soon as you can. --Mike __________________________________ Do you Yahoo!? Yahoo! Calendar - Free online calendar with sync to Outlook(TM). |
to navigate to use esc to dismiss