NPN 100mA 50V Complex Digital Transistors (Bias Resistor Built-in Transistors)
Two DTC114T in one chip.
Package: SOT-363
Parts witch are quite similar:
10kOhm bias resistor: EMH4 / UMH4N / IMH4A
4,7kOhm bias resistor: EMH3 / UMH3N / IMH3A
Panasonic DMC56406 (4,7kOhm)
A number of problems with this one:
Schematic:
Bad scale (unfortunatly common even in core parts) which is a pain to fix but should be done. Basically you need to change the internal scale so the view box coords are 100 times the size in inches to make a px = 1 thou. The worst of this is that at least Inkscape will rescale it mostly but doesn’t change the stroke-widths so you have to do them with a text editor (or a yet to be written python script 
which I can feel coming on).
Whatever part you cloned from may have had bendable legs again as the terminalIds were a group (and got deleted when I ungrouped it). Replaced them with 10 thou by 10 thou rectangles at the ends of the pins. I resized schematic so the pins are on .1 centers to match many (but not all) other parts. In general smaller is better so you can get as much as possible on a single schematic page. At the end regrouped it all and added layerId schematic (without that svg export of the part breaks). Your internal pin numbers are in correct as well (as you can see in the sketch below). Breadboard doesn’t match schematic or PCB. Flipped the entire thing horizontally so pin 1i is on the left as is standard.
PCB:
Rescaled again. The current pads are too large according to the footprint recommendation in the data sheet, so I adjusted them down to the maximum recommended size and changed the pin numbers to be correct (i.e. connector0pad is pin 1 of the package then up in sequence).
fpz file:
changed connector types from pad to the more standard male
for all pins. Re sequenced the connectors to start a 0 for pin 1 and proceed up in order for neatness. Changed the pin name to pin x (where x is 1 to 6) depending on connector position so hovering over the pad in breadboard gets pin 1 Emitter 1 rather than the (incorrect) C1 Collector1 from your part which doesn’t tell you what pin number it is. Rather than post the part this time, I’m posting a sketch which illustrates some of the problems (the new part can be exported from the temp parts bin in the sketch). Note that in your part schematic is offset .05 in from the grid and the wire connects to the middle of the pin. That is caused by the terminalId being a group, without a terminalId frtizing defaults to the middle of the element defining a pin and aligns that point on connector0 to the grid. As well you can see from the numbers of the connectors connected to the pins in breadboard, that the numbering in schematic and pcb is different when all three should be the same. J3 for instance is pin1 in breadboard but pin 6 in both schematic and pcb.
UMH4_Sketch.fzz (25.4 KB)
Peter