Hi Bryan, Welcome to EasyEDA. If you have been looking around the forums, I'm guessing you've found the EasyEDA Simulation eBook at: https://docs.google.com/document/u/1/d/1OWZVVFRAe_2NW3WratpkA_SGuHa5AcRow5ZRfvcoVTU/pub in particular: https://docs.google.com/document/u/1/d/1OWZVVFRAe_2NW3WratpkA_SGuHa5AcRow5ZRfvcoVTU/pub#h.43ky6rz What may also save a bit of hunting around is: https://easyeda.com/forum/topic/How_to_find_simulatable_parts_in_EasyEDA-1YgasK2kC The reason you are getting: `Error: unknown subckt: xq5 q8_1 xq4_3 r4_2 2n2222a npn` is because you have made a simple mistake. * The reason there is an error message about a subckt is because the model for a 2n2222a from ON Semi is a .model defined model and not a .subckt defined model. So all you have to do is to: 1. paste the **whole** of the model text into your schematic; 2. Set it to `text type = spice`; 3. Select the symbol; 4. Edit the bjt symbol name to be exactly the same as the name in the .model; 5. Press `I` and set the `Spice Prefix` to Q. 6. Done. *However, please note that there is a model for the 2N2222, 2N2904, 2N3904 and 2N3906 already in the library.* *I have also just put models for the Q2n2907a and Q2n2222a in there too so all you have to do is place the relevent symbol in the schematic and edit the name to match the model in the library.* *So, no other changes needed.* The reason it made no difference if you pasted the whole model statement or just the model line into the schematic is also because EasyEDA and ngspice was looking for a .subckt and not a .model definition. For any model, you have to paste the **whole** of the model definition (including, for copyright reasons, all the header information!) like this for example from: http://www.onsemi.com/pub_link/Collateral/2N2907A.LIB.TXT ************************************** * Model Generated by MODPEX * *Copyright(c) Symmetry Design Systems* * All Rights Reserved * * UNPUBLISHED LICENSED SOFTWARE * * Contains Proprietary Information * * Which is The Property of * * SYMMETRY OR ITS LICENSORS * *Commercial Use or Resale Restricted * * by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 Mar 1, 13 * MODEL FORMAT: PSpice .MODEL Q2n2907a pnp +IS=3.02341e-12 BF=523.064 NF=1.16335 VAF=44.2994 +IKF=0.591421 ISE=3.31443e-11 NE=1.9954 BR=4.8572 +NR=1.18959 VAR=1.33092 IKR=5.91421 ISC=3.31443e-11 +NC=3.81262 RB=2.76209 IRB=0.1 RBM=0.880912 +RE=0.0001 RC=0.857407 XTB=0.119647 XTI=1 +EG=1.05 CJE=3.934e-11 VJE=0.680693 MJE=0.379312 +TF=2.75919e-10 XTF=0.674951 VTF=54426.6 ITF=0.067962 +CJC=2.40198e-11 VJC=0.4 MJC=0.462796 XCJC=1 +FC=0.570446 CJS=0 VJS=0.75 MJS=0.5 +TR=1e-07 PTF=0 KF=0 AF=1 * Note that the model from OnSemi is named: `Q2n2907a` and not `2n2907a` * Somefurther notes about your sim. 1. Delete V1 and replace it with a spice Independent source as described in: https://easyeda.com/forum/topic/Selecting_Sources_in_EasyEDA-oASM4mEyQ 2. For simulations, unless there is a dedicated spice symbol for a device (see link above on how to find these), it's always best to use symbols directly from the EasyEDA Libs. 3. Slider of R16 pot needs to be connected somewhere. A simpler variable resistor symbol is also available in the EasYEDA Libs. :)

Also now added: mjl3281a mjl1302a to library.

Thank you so very much for your reply. Now it makes sense.