Errors in pin assignment for a SPICE file in Altium

There are two faults here:

1. A single-unit SPICE model can't be attached to a dual symbol in Altium. It's a limitation of the platform, but it is easily addressed by making a two-section Part. Each section gets its own instance. (You can simply not place the second instance and ignore the Part warning, rather than placing it and strapping it as unused.)

2. The SPICE definition itself is wrong. I don't know how this happened, if LTSpice uses a different .SUBCKT definition or what, but the PARAMS: keyword is missing, between the list of nodes and the list of parameters.

This might be corrected as so:

.SUBCKT 74HC123 A B CLR CGND RC Q QN VCC VGND PARAMS: vcc1={vcc} speed1={speed} tripdt1={tripdt} 

Note that the vcc, speed and tripdt parameters have to be set globally (Design/Simulate/Mixed Sim, or Setup Mixed-Signal Simulation; Analyses Setup, Global Parameters). SPICE statements cannot be strewn about the schematic unlike most simulators.

The problem compounds, however. You also need to find substitutes for ALL the logic elements, which use the LTSpice propietary logic primitive. For example:

A21 0 N010 0 N011 0 0 N009 0 OR tripdt={tripdt1} td={td5} 

Seems to be an OR gate, presumably between N010 and N011 (inputs) and N009 (output). Note that equivalent timing parameters must be entered as well.

Altium uses a modified XSPICE engine, so these can perhaps be substituted with primitives from that platform.

Example:

^{Source: F.L. Cox, W.B. Kuhn, H.W. Li, J.P. Murray, S.D. Tynor, and M.J. Willis, Xspice User's Manual, Georgia Institute of Technology, Computer Science and Information Technology Laboratory (Dec. 1992); p.141.}

The bracketed list specifies a vector of input nodes. See the above reference, and LTSpice help for more information.[1] You may also be interested in porting elements to SimCode: https://techdocs.altium.com/display/AMSE/Digital+SimCode+Reference

Current versions of Altium may support more variants of syntax; I don't have an up-to-date version to compare. The above is correct through AD18, period-appropriate to the question.

[1] A correct link, but not very useful given its present content. Evidently this wiki is not well curated. This seems the more useful page: https://ltwiki.org/index.php?title=Undocumented_LTspice#A-Devices

The model only has these inputs, which is only one section of the inputs for the T-flip flop. Your model has two, your sub circuit only has one.

.SUBCKT 74HC123 A B CLR CGND RC Q QN VCC VGND

Typically spice files don't have dual parts inside of them, because they can be duplicated outside of the part. The code will need to be duplicated for both halves of the part.

There are a few options to correct this: 1) duplicate the library file and write a new one that has two of the 74HC123 sub circuits.
2) Change the graphical part to only have one flop not two. (which you probably don't want to do to mach the real world schematic)
3) This might be solvable in the netlist by doing something like this (but I have not tried it)

The SN74123 appears to be a dual monostable. However, the sim model looks to be just for a single instance.

The schematic indicates that you are interested in the operation of just one instance as well.

To get this to work, do not try to map the pins of the unused (2nd) instance (I've always had trouble with Altium and multi-part components with sim). Just map the pins for part A.

Your Model Kind statement should end up with just 9 parameters (as listed in the circuit sim file:

@DESIGNATOR %1 %2 %3 %4 %5 %6 %7 %8 %9 @MODEL

with %1 corrsesponding with "A", %2 to "B", and so on:

.SUBCKT 74HC123 A B CLR CGND RC Q QN VCC VGND

For example, here's a declaration for Part A of a dual Amp:

---

I am not familiar with the significance of the rest of the model statement in the sim file:

vcc1={vcc} speed1={speed} tripdt1={tripdt}

perhaps you will need to define these values as global parameters in your sim setup? Or maybe you can define them as constants in the model line? I don't know. Try and find out...