I'd like some subcircuit guidance

[Euler's_Identity]

What I'd like to be able to do is convert a subcircuit into a component model.  For example, I recently needed a 74hc193, a couple of them.  However, I found that Multisim v10.1's model has a small error, for (at least) the Borrow Output's pulse-width reduces to a sliver if anything is attached to the pin.  Therefore, I built the counter circuit using digital components (time consuming...) and copied it, as a "paste as subcircuit," into the design where I needed it.  I'm thinking there's a better way, a way to create components to store in my library somehow.  Granted, I could just make a "circuit" of subcircuits (a library of sorts type of file) and edit them (to open them in a new window) and copy them to "paste as subcircuit" whenever I needed them; that would be an option.  But that option doesn't seem to be, how shall I say, elegant.

Do any of you have any ideas how I can convert such subcircuits into component models in some more elegant manner?

[NavyJay]

I reuse my circuit components by grouping them into hierarchical blocks, which is identical to a subcircuit, but saves the circuit to its own file.  It won't show up in your library as a component, however.  You can just keep your blocks organized in a directory structure that makes sense to you.

The only way I am aware of to create your own component is to export the netlist and place it in your user library.  This is a little more time consuming and will lose all non-spice data such as part/wire placement, analysis instruments, etc.

-J

[Euler's_Identity]

Thanks for the tip. Way back when I used hierarchical blocks (HBs) for chips I'd make up which weren't available.  However, I seem to remember sending in a circuit to Multism once that contained HBs and being told I should use subcircuits instead, but I must admit I don't remember why.  Based on what you've said, the HB route seems reasonable.

[OStep]

Hi,

One good solution is to create a SPICE .subckt from your Multisim schematic and then create a Multisim component for the .subckt. At the moment, unfortunately, there's no wizard-like way to do this (this is being considered for future releases) so you'll have to do this manually. Here are the general steps

1. Leave on the schematic only the core model components (i.e remove any input sources, grounds)

2. Give the nets that will be your .subckt ports (and also your component ports) meaningful names. Note:  ports must be connected to either all digital or all analog components- you cannot have a mix.

3. Export your netlist

4. Wrap the netlist with ".subckt PARAMS" and ".ends" statements, where PARAMS is the standard format for .subckts. So, your final result should look something like

.subckt anyName node1 node2 node3 nodeN

****National Instruments SPICE to netlist routine

***blah blah blah

aU1 node1 88 modelsx

(more exported stuff here)

.ends

5. Create component using Component Wizard. Make sure to select the component type (Analog or Digital) according to the types of the ports

Message Edited by MaxNI on 03-02-2009 09:12 AM