Please check <https://easyeda.com/Doc/Tutorial/spiceSimulation.htm#3.Froma%C2%A0spicedirectiveinaschematic> out

* If you are trying to find a transistor just to draw in a schematic then all you have to do it place a symbol for it from EasyEDA Libs (bjt, mosfet, darlington, jfet, IGBT etc) and then double-click on the name text and edit that to whatever you want. * If you are trying to find a simulation model for a transistor or find a transistor that has a simulation model attached then please refer to the whole of the section that Dillon suggested in the EasyEDA Tutorial: <https://easyeda.com/Doc/Tutorial/spiceSimulation.html#h.62i6bydbsl9u> The following examples may help illustrate what the tutorial is describing: <https://easyeda.com/file_view_Playing-with-model-parameters_Ev5rpnJG2.htm> <https://easyeda.com/file_view_LM108-test-jig_htnFzR9OI.htm> <https://easyeda.com/file_view_How-to-simulate-a-spice-netlist-directly-in-EasyEDA_53WewqI0i.htm> <https://easyeda.com/file_view_Moving-coil-cartridge-phono-preamp_u8EWQ8qjB.htm> <https://easyeda.com/file_view_Simulation-schematic-for-Bob-Pease-s-High-Impedance-Active-Scope-Probe_F3fOMmWUt.htm> <https://easyeda.com/file_view_TL081-based-10W-amplifier_axXV74ECA.htm> <https://easyeda.com/project_view_Class-A-2SK1058-MOSFET-Amplifier_B1VP7oiAS.htm> <https://easyeda.com/project_view_Current-source-devices_EFztNHZhy.htm> <https://easyeda.com/project_view_CMOS-Inverter_wICUctL3l.htm> * To use a .subckt in a schematic symbol that is expecting to call a .model (for example to use the EasyEDA mosfet symbols with 3rd party .subckt definitions): > In a schematic, if a symbol has a Spice prefix of 'M' then it calls up a model in the form of a .model definition. > If you want to use a different spice model with that symbol but the new model is in the form of a .subckt definition then the symbol Spice prefix must be changed to 'X'. To do this: a) Click on the schematic symbol to highlight it. b) Then: > Super Menu > Miscellaneous > Edit Symbol... or (easier): > Press the I Hotkey. c) Change the 'Spice prefix' from 'M' to 'X' d) Click OK. Done. This might look hard but just set up a very simple test jig and try it a few times!

how can i choose the value of BETA for bjt?

The nearest parameter to Beta in a BJT spice model is `BF`. However, if you want to accurately model the effect of Beta variation in transistors of the same type you also need to vary all the other model parameters. This is because Beta variation is not an isolated physical parameter, it arises from a combination of other device physical parameter variations. This is why device modelling at the device and IC fab level uses fully characterised device model sets. Unfortunately these model sets are not usually available for discrete devices. There are *some* models available - such as for the BC846A and BC846B hfe range devices below - and these illustrate the kind of parameter variations that include but are by no means limited to, the basic `BF` parameter variation. For more information about device modelling, please see (3) in: https://easyeda.com/andyfierman/Welcome_to_EasyEDA-31e1288f882e49e582699b8eb7fe9b1f **This is a model for a BC846A:** ************************************** * Model Generated by MODPEX * *Copyright(c) Symmetry Design Systems* * All Rights Reserved * * UNPUBLISHED LICENSED SOFTWARE * * Contains Proprietary Information * * Which is The Property of * * SYMMETRY OR ITS LICENSORS * *Commercial Use or Resale Restricted * * by Symmetry License Agreement * ************************************** * Model generated on Sep 13, 12 * MODEL FORMAT: SPICE3 .MODEL bc846alt1g npn +IS=8.36175e-14 **BF=276.385** NF=1.07221 VAF=10 +IKF=0.0266381 ISE=1.97552e-13 NE=1.47405 BR=2.94391 +NR=1.1187 VAR=5.64674 IKR=0.266381 ISC=1.97552e-13 +NC=1.26493 RB=4.74759 IRB=2.00988 RBM=0.665574 +RE=0.0002 RC=0.001 XTB=0.267171 XTI=4 +EG=1.07225 CJE=7.6759e-12 VJE=0.402735 MJE=0.298569 +TF=5.78244e-10 XTF=2.80886 VTF=20.6808 ITF=0.0813242 +CJC=4.08707e-12 VJC=0.95 MJC=0.342311 XCJC=0.8 +FC=0.8 CJS=0 VJS=0.75 MJS=0.5 +TR=1e-07 PTF=0 KF=0 AF=1 **This is a model for a BC846B:** ************************************** * Model Generated by MODPEX * *Copyright(c) Symmetry Design Systems* * All Rights Reserved * * UNPUBLISHED LICENSED SOFTWARE * * Contains Proprietary Information * * Which is The Property of * * SYMMETRY OR ITS LICENSORS * *Commercial Use or Resale Restricted * * by Symmetry License Agreement * ************************************** * Model generated on Oct 7, 08 * MODEL FORMAT: SPICE3 .MODEL bc846bdw1t1g npn +IS=6.21868e-15 **BF=313.939** NF=0.978615 VAF=808.652 +IKF=0.0670247 ISE=6.72945e-10 NE=4 BR=31.3939 +NR=1.03954 VAR=311.824 IKR=0.670247 ISC=5.02001e-14 +NC=1.10677 RB=45.553 IRB=0.1 RBM=0.1 +RE=0.18181 RC=0.909048 XTB=1.26632 XTI=1.16217 +EG=1.206 CJE=7.31938e-12 VJE=0.479294 MJE=0.236218 +TF=6.54085e-10 XTF=1000 VTF=8791.04 ITF=12.3428 +CJC=1.97395e-12 VJC=0.95 MJC=0.33914 XCJC=1 +FC=0.8 CJS=0 VJS=0.75 MJS=0.5 +TR=1e-07 PTF=0 KF=0 AF=1