Adding new transistors to LTspice???

G'day all.

I am wanting to build an image orthicon B&W television camera and have the complete circuit diagram for a 1960s transistorized image orthicon camera chain. Unfortunately the circuit has obsolete germanium transistors so I need to somehow substitute modern available silicon transistors in place of them and have been reading up some modification tips on substituting germaniums for silicons here http://www.hawestv.com/transistorize/germanium1.htm .

Anyhow cutting to the chase I need to be able to test sections of the camera's circuitry using the original germanium transistors in LTspice and then with silicon transistors along with the necessary modifications test the circuitry again to see if the results match the original design. However I haven't got the faintest idea in understanding the code values of the transistors eg.:
.MODEL 2N3393 NPN(IS=12.03E-15 ISE=8.195E-12 ISC=0 XTI=3 BF=154.1 BR=4.379 IKF=0.1072 IKR=0 XTB=1.5 VAF=37.37 VAR=12.5 VJE=0.65 VJC=0.65 RE=0.1 RC=1 RB=10 CJE=8.307E-12 CJC=5.777E-12 XCJC=0.75 FC=0.5 NF=1 NR=1 NE=1.971 NC=2 MJE=0.384 MJC=0.3199 TF=385.4E-12 TR=783.8E-12 ITF=0.17 VTF=3 XTF=8 EG=1.11 KF=1E-9 AF=1 VCEO=25 ICRATING=500M MFG=NSC)

All of those vales make absolutely no sense to me and do not even resemble anything of that transistor's given values on alltransistors.com http://alltransistors.com/transistor.php?transistor=3141 which are:

2N3393 Transistor Datasheet. Parameters and Characteristics.
Name: 2N3393
Material of transistor: Si
Polarity: npn
Maximum collector power dissipation (Pc): 200mW
Maximum collector-base voltage (Ucb): 25V
Maximum collector-emitter voltage (Uce): 25V
Maximum emitter-base voltage (Ueb): 5V
Maximum collector current (Ic max): 100mA
Maximum junction temperature (Tj): 125°C
Transition frequency (ft): 70MHz
Collector capacitance (Cc), Pf: 12
Forward current transfer ratio (hFE), min/max: 90/400
Manufacturer of 2N3393 transistor: GEN
Package of 2N3393 transistor: TO98-1
Application: Low Power, General Purpose

So I was wondering if anyone can help me on how to go about adding transistors and encoding the transistors specifications to that of LTspice's mumbo jumbo coding? Any advice would be much appreciated.

Lastly here's the list of transistors this camera contains:
2N337 X5 (can subsitute with 2N699 except IO safety circuit)
2N491 X3
2N699 X3
2N743 X1
2N1022 X2
2N1131 X2
2N1143 X12 (can substitute with 2N1301)
2N1274 X1
2N1308 X2
2N1415 X2
2N1546 X2
2N1565 X1
4N1908 X4
2N1997 X9
2N1999 X23
2N2000 X1 (can substitute with 2N1046)
2N2102 X2
2N2145 X1
2N2157A X4
2N2671 X28 (can substitute with 2N2084 & 2N1309)

hi,

Open the following file, using a text editor and paste the model details listed below, into the
C:\Program Files\LTC\LTspiceIV\lib\cmp\standard.bjt

Paste it at the top of the other transistor models in that file, Save the standard.bjt file.

Run LTspice and using F2 , select a 'npn' transistor an place the symbol on your circuit.

Right click on the transistor symbol and then 'pick new transistor button', your NEW transistor 2N3393 should appear, select it.

I have a asc file and image to help you test , AFTER you have added the new model.



.MODEL 2N3393 NPN(IS=12.03E-15 ISE=8.195E-12 ISC=0 XTI=3 BF=154.1 BR=4.379 IKF=0.1072 IKR=0 XTB=1.5 VAF=37.37 VAR=12.5 VJE=0.65 VJC=0.65 RE=0.1 RC=1 RB=10 CJE=8.307E-12 CJC=5.777E-12 XCJC=0.75 FC=0.5 NF=1 NR=1 NE=1.971 NC=2 MJE=0.384 MJC=0.3199 TF=385.4E-12 TR=783.8E-12 ITF=0.17 VTF=3 XTF=8 EG=1.11 KF=1E-9 AF=1 VCEO=25 ICRATING=500M MFG=NSC)

G'day. Thanks for helping but that wasn't quite the answer I was after nor that was the question I was actually asking. That particular transistor I am aware is already in the models list in standard.bjt and I actually cut and pasted the given code for that 2N3393 transistor from standard.bjt as an example showing what kind of mumbo jumbo coded parameters LTspice uses to specify transistor values instead of having a user friendly parameter settings for us to add new transistors such the data on transistors listed on alltransistors.com .

What I want to know is when I want to add new transistors to the standard.bjt, how do I convert the transistor specifications like max collector-base voltage, max collector current etc. to the mumbo jumbo code LTspice uses such as ISE= ISC= BF= BR= etc.? I basically want to enter all those listed old germanium transistors into standard.bjt with the appropriate codes that represent those transistors' specifications so I can accurately reconstruct sections of the camera's circuits where the transistors are in LTspice, run the appropriate signals through them and look at the output signal, then after that replace the germanium with a silicon and the appropriate resistors to make the silicon do the job similarly to the germanium and test the output signal to see if it's the same so I know if it will work or not.

aussiebloke said:

G'day. Thanks for helping but that wasn't quite the answer I was after nor that was the question I was actually asking. That particular transistor I am aware is already in the models list in standard.bjt and I actually cut and pasted the given code for that 2N3393 transistor from standard.bjt as an example showing what kind of mumbo jumbo coded parameters LTspice uses to specify transistor values instead of having a user friendly parameter settings for us to add new transistors such the data on transistors listed on alltransistors.com .

What I want to know is when I want to add new transistors to the standard.bjt, how do I convert the transistor specifications like max collector-base voltage, max collector current etc. to the mumbo jumbo code LTspice uses such as ISE= ISC= BF= BR= etc.? I basically want to enter all those listed old germanium transistors into standard.bjt with the appropriate codes that represent those transistors' specifications so I can accurately reconstruct sections of the camera's circuits where the transistors are in LTspice, run the appropriate signals through them and look at the output signal, then after that replace the germanium with a silicon and the appropriate resistors to make the silicon do the job similarly to the germanium and test the output signal to see if it's the same so I know if it will work or not.

Click to expand...

That "mumbo jumbo code" consists of standard Spice parameters used in all Spice type programs, which allows accurate simulation of the transistor operation under a wide variety of operating conditions. The parameters in a data sheet tell only enough about the transistor for the designer to use it in a circuit but not enough to accurately simulate its operation. The data sheet parameters can be converted into the spice parameters with limited accuracy. See this for a program (SpiceMod, not free) that does just that.

So otherwise you could try to find some Spice parameters for similar germanium transistors and put them into LTSpice. The simulation won't be exact, but it should be close enough to tell you how the circuit operates. And there likely isn't that much difference between the circuit operation with germanium and with silicon, other then possibly having to adjust the base bias resistors to allow for the different Vbe.

SPICE parameters seem to bear no resemblance to their datasheet equivalent so you have my sympathy. Trust the mumbo jumbo and assume it is close to the datasheet performance of the part and the simulation should be accurate. Have a look at the link below for more information on importing 3rd party spice models. personally I do not import them into the standard library. If I ever have to reinstall LTSpice, I believe the standard library (hence all your models) gets deleted. I keep all the models in a separate directory

simonbramble said:

........................
personally I do not import them into the standard library. If I ever have to reinstall LTSpice, I believe the standard library (hence all your models) gets deleted. I keep all the models in a separate directory

Click to expand...

What I do, if I have to reinstall a program is to save all the libraries under a different name before the install. Then you can remove the new libraries and change the saved file names back to the original after the installation is complete and nothing is lost.

I am learning LTspice XVII.
Have placed a .model of npn MPSAO6 into /cmp.
I can select it and place it.
In the 'Pick New Transistor' boxes Vceo[V] and the Collector Current[A], is blank.
Existing items have this data.
What am I not doing?

Do you have Vceo and Collector Current values specified in you model statement?

alec_t said:

Do you have Vceo and Collector Current values specified in you model statement?

Click to expand...

Thanks for reply.
No V or I values:
Got this model from LTwiki
.MODEL MPSA06 npn
IS=6.03149f BF=559.138 NF=0.841146 VAF=996.086 IKF=0.187838 ISE=1e-08
NE=3.53096 BR=43.984 NR=0.893292 VAR=1.45264 IKR=1e-05
ISC=3.06474e-11 NC=3.98114 RB=0.01 IRB=0.269152 RBM=0.01 RE=1e-05
RC=0.000928752 XTB=1.17305 XTI=1 EG=1.05 CJE=5.54912e-11 VJE=0.577764
MJE=0.313139 TF=5.4629e-10 XTF=23.7458 VTF=7.07849 ITF=4.69733
CJC=1.76218e-11 VJC=0.4 MJC=0.285166 XCJC=0.902334 FC=0.732277
TR=1e-07

You can look up the Vceo and Collector Current values specified in the datasheet and paste them into the model statement, but note that LTspice will ignore these values in a simulation.

alec_t said:

You can look up the Vceo and Collector Current values specified in the datasheet and paste them into the model statement, but note that LTspice will ignore these values in a simulation.

Click to expand...

Thanks for info.
Have observed values in other .models. Have done what you said. All good.
Cheers

ericgibbs said:

hi,

Open the following file, using a text editor and paste the model details listed below, into the
C:\Program Files\LTC\LTspiceIV\lib\cmp\standard.bjt

Paste it at the top of the other transistor models in that file, Save the standard.bjt file.

Run LTspice and using F2 , select a 'npn' transistor an place the symbol on your circuit.

Right click on the transistor symbol and then 'pick new transistor button', your NEW transistor 2N3393 should appear, select it.

I have a asc file and image to help you test , AFTER you have added the new model.



.MODEL 2N3393 NPN(IS=12.03E-15 ISE=8.195E-12 ISC=0 XTI=3 BF=154.1 BR=4.379 IKF=0.1072 IKR=0 XTB=1.5 VAF=37.37 VAR=12.5 VJE=0.65 VJC=0.65 RE=0.1 RC=1 RB=10 CJE=8.307E-12 CJC=5.777E-12 XCJC=0.75 FC=0.5 NF=1 NR=1 NE=1.971 NC=2 MJE=0.384 MJC=0.3199 TF=385.4E-12 TR=783.8E-12 ITF=0.17 VTF=3 XTF=8 EG=1.11 KF=1E-9 AF=1 VCEO=25 ICRATING=500M MFG=NSC)

Click to expand...

Hi Eric,

Hopefully you are still here after all these years! )

I have a similar problem - wanting to add a JFET model from Cordell Audio's site to the list in LTspice XVII.

I have found the LTspice "standard.jft" file (in C:\Program Files\LTC\LTspiceIV\lib\cmp\) ... but I can't see how to open it - so I can paste my JFET model into it???

Are you able to advise?


Thanks,
Andy

I think you can edit that file with a txt editor. Note pad or word pad, one works better but I don't remember. Not on a Windows computer right now so I can't test it.

ronsimpson said:

I think you can edit that file with a txt editor. Note pad or word pad, one works better but I don't remember. Not on a Windows computer right now so I can't test it.

Click to expand...

Thanks, Ron - that's what I thought.

So I:
* highlighted the file 'standard.jft',
* pressed 'Ctrl/C'
* opened Note Pad, then
* pressed 'Ctr/V'

... and nothing happened!

Andy

Right-click on the filename. That will give a drop-down list headed 'Open with...'. Select Notepad from the list to open the file..

Some people use a sim program to see if their design will work. But the sim has only "typical" spec's, not the important minimums and maximums (especially hFE) that are needed in the design so that every passing part works.

Where can you buy "typical" parts? You get whatever they have and the person buying before you might have got all the "good" parts so you get the minimums. Maybe the last production run produced all minimums or all maximums?

some models (transistors and vacuum tubes primarily) have some of the spice parameters derived from operating curves for the devices such as Ice/Ibe and Ipk/Vgk curves, so the process for making a model of a transistor or tube isn't a matter of plugging in static values from the data sheet. with transistors, the beta is usually inversely proportional (and not linearly either) to the collector current, so at a particular static condition, the beta might be 200, and that's the value put into the data sheet, and the beta is only 10 or less near saturation, and you need to refer to the beta vs Ic chart in the data sheet to know what the actual beta is going to be at any given operating point. the chart data is what is needed for a spice model, because the beta of that transistor isn't always 200.

there is software out there that's used for creating models, but it requires a lot of data points to be entered.