LTC1485 component in LTspice

Question

I am simulating a model in LTspice and I Need to add the LTC1485 IC in the model. Unfortunately I could not find it in the LTspice library can anyone help me get this component model?

Many thanks

Answer 1

There does not appear to be a SPICE model available from Linear, nor an model of an equivalent part (*75176) from other vendors. This is not unusual, bus transceivers are typically modelled in an IBIS environment (focusing on digital behaviour) rather than SPICE.

However, because there are IBIS models available from both ADI and TI for their equivalent part, as Andy pointed out, you have a couple options:

• use an IBIS simulation environment, like Hyperlynx.
• use a SPICE simulation environment which supports using IBIS models directly, like Microcap.
• use a third-party tool (search "ibis to spice converter" in your search engine of choice) to transform the IBIS model into a SPICE model (this is often finicky, dependent on version, and can lead to poor modelling).

In this case, you may want to rethink your need for a SPICE simulation of this particular part.

Finally, if all you care about is the effect of the transceiver input on the rest of your circuit, you can also try and approximate the equivalent circuit of the input pins (ignoring the actual transceiver behaviour and output). Typically, an input pin is most easily modelled as a parallel R and C (in this case, R is stated in the datasheet, and C can be approximated from the package, but should be negligible at the speeds involved).

Also remember that simulation only takes you so far. If you require such a high degree of detail that you must have models of absolutely everything in the circuit, you may be looking at/for minutiae that may or may not be artifacts of the simulation. That's when the simulation cannot help anymore and a prototype is needed.

Answer 2

If you just need to model the functionality of the LTC1485, you might be able to do this with the diffshmtbuf and diffschmitt devices found in the LTspice\lib\sym\digital folder. (you can find these under the parts menu)

If you look under help in ltspice (and type schmitt), you can find information about the digital parts in the special functions section.

With these parts you can control the hysteresis voltage, high and low voltage, capacitance, rise an fall times, output capacitance and input impedance.

The Schmitt trigger devices have similar output characteristics as the gates. Their trip points are specified with instance parameters Vt and Vh. The low trip point is Vt-Vh and the high trip point is Vt+Vh.

The gates and Schmitt trigger devices supply no timestep information to the simulation engine by default. That is, they don't look when they are about to change state and make sure there's a timestep close to either side of the state change. The instance parameter tripdt can be set to stipulate a maximum timestep size the simulator takes across state changes.