I am working with 74LVC541A SPICE model (found under documentation) with the Microcap simulator at the link below using:
The model in the above link doesn't allow me to see visually the connections in the LVC. How can I visually see what is being connected in the SPICE model?
Doing this on a part like this is not super useful, as the designers most likely only replicated the functionality of the part and not the actual transistors.
If you are trying to do this in microcap, you'll have to do it manually.
You can do this in LT spice to some extent, Here are some instructions:
Schematic Builder to automate the first steps below.
Before you start, make working copy of the netlist and then clean it up by doing any reordering of lines or shortening of node/net names that will make them easier to work with. For example, nets with names like "n023" and "n001" can usually be safely shortened to "n23" and "n1" (sometimes I do this in a word processor with find and replace). Also, it is a good idea to move all comments to the end of the working netlist (if not delete them altogether).
At this point, I like to import the netlist into LTspice, either directly onto the schematic (if the netlist is short) or into a separate LTspice netlist window.
Now go through the netlist line by line and place a component of the corresponding type on the schematic (arrange these in rows by component type such that you build up rows of all the same type). It is important to do this in exactly the same order as the net- list because this will greatly ease cross checking when you think you have finished. (Also, all of the SPICE text, such as model statements, etc. should be copied and pasted in at the end.)
As you place each component, edit its reference designator to agree with the corresponding netlist reference designator.
As you place each component, place a net-label/node-name directly on each pin of the component (of course, these should agree with their names in the netlist, too). Don't bother with wires yet as these will just be trouble to move around later.
Once all the components are placed, view the SPICE Netlist (it's a drop-down menu item) and verify that it agrees exactly with the original netlist (it will, if you followed these instructions carefully). Correct any errors as needed until agreement is perfect. This "schematic" should actually be able to run at this point.
(This above section is what is automated by the SchBuilder.)
