Makign a circuit block in LTspice

[opampsmoker]

Hi,
Do you know how i can make the attached into a "box" with the three connections "coll", "here" and "gnd" ?
Basically, i want a single circuit block component which is as in the attached.

 

[rjenkinsgb]

A transistor with resistors includes is known as a "digital transistor".

This one has a SPICE model listed with it, you should be able to convert/import that in to ltspice etc.
**broken link removed**

 

[eTech]

Hi,
Do you know how i can make the attached into a "box" with the three connections "coll", "here" and "gnd" ?
Basically, i want a single circuit block component which is as in the attached.

First, rename the schematic file so the file name doesn't contain any spaces.

Then,

1. Define the nodes you want to be "pins" using a label with a "Port Type". The Port Type has no other significance other than where it is placed on the block symbol (which you can move later), and really doesn't matter whether the port type is input, output, or bidirectional .
Your label names:

here
coll

are ok, but should be changed to a "port type".

2. The ground label can be anything other than "gnd". A "gnd " label name will be converted to global node "0" and changed to a ground symbol. Use "Vee", or just "E", if you like, to keep it a separate node.

3. To automatically create a symbol.
Heirarchy-> Open this sheets symbol->Click "yes" when prompted.
A symbol will be created and displayed in the symbol editor. Close the symbol editor.
The symbol will be created in the same folder as the schematic.

4. To test the symbol.
Open a schematic in same folder as symbol.
Click the "select component" tool. There will be a browse pull down at the top.
Browse to the schematic folder, the symbol should appear in the lower pane.
Click the symbol then click OK. The symbol will be attached to the pointer.
Place the symbol on the schematic