Ok, think I've figured it out ... even if you intend to associate your own model with a device, you have to choose a device that already has a model to start with.  Otherwise, it looks like it always gets (silently) ignored.

... although now I just keep getting a rather unhelpful message "ERROR: error" when I run a simulation.  The netlist looks OK to me visually, but it won't run...

For help in getting simulations to run smoothly, please refer to:

https://docs.easyeda.com/en/Simulation/Chapter1-Introduction/index.html

In your model:

.model 2SC3356 NPN(IS=6E-16 NF=0.98 ISE=32E-16 NE=1.93 BF=120 IKF=0.0.17 VAF=10 NR=0.991 ISC=0 NC=2 BR=12 IKR=0.17 VAR=3.9 RB=4.16 IRB=1.96E-04 RBM=3.6 RE=0.38 RC=2  XTB=0 EG=1.11 XTI=3 CJE=2.8E-12 VJE=1.3 MJE=0.5 TF=15E-12 XTF=6 VTF=10 ITF=0.2 PTF=0 CJC=1.1E-12 VJC=0.7 seiresMJC=0.55 XCJC=0.3 TR=1E-09 CJS=0 VJS=0.75 MJS=0 FC=0.5 Vceo=12 Icrating=100m mfg=cel)

if you delete:

Vceo=12 Icrating=100m mfg=cel

then your simulation will run.

This text at the end of the model is not part of the spice model syntax. It is a proprietary LTspice (and possibly Pspice) add-on which throws an error because it is not recognised by ngspice.