multisim spice model help

I'm not sure what your question means:

Did you draw a specific symbol, or place values in a transformer that was generated by multisim?

If you drew your own, are you asking where to find terminals to place in your symbol so that you can connect to it (that will be specific to the way the schematic package of multisim works), or how to connect the transformer once you have done that?

As multisim is a schematic-based system, all that you should need to do is place your symbol in a schematic and connect it up.

If you are concerned about the internal node numbers that multisim has created, these are arbitrary - nodes within the subcircuit that have the same number are connected together (I've checked on the connection, and that is fine - only the coupling coefficients look suspicious - I don't know this specific transformer, but I would not usually expect the coupling between the single winding and the step-down turns to be the same as the coupling between the step-down turns themselves).

If you are asking how to hand-wire into SPICE using node numbers, again all you need to know is that the order of nodes inside the subcircuit definition corresponds to those used outside, and that node-names (numbers) written within a subcircuit are isoolated from the same numbers written outside it - the connection is by using the syntax.

If you use the transformer in a circuit, the end line will appear as (the $ sign can vary between simulators):

X$ts_pq4_48_1 a b c d e ts_pq4_48
the names or numbers a, b, c, d , e will correspond to 1, 2, 3, 4, 5 inside the transforemer, and should be the same as the nets you wish to connect to those pins of the transformer.

thank you for your reply. the example in my first post is a transformer model from multisim9. it is a 5 pin transformer. i need to make a 6 pin fransformer that uses 2 pins on the input, and 2 pins each for 2 outputs. 120v in 10v out on each of the 2 sets for a total of 20vac. i know that the 1, 2, 3, 4, 5 of the example correlate to the external pins, but were do the nodes 11, 31, 41 etc come from?

thank you

Ken

They are created by the people who built the transformer model to allow them to connect resistance in series with each of the coils. Take L1 as an example. Logically it connects between pin 1 and pin 2, but then it would be a zero-resistance coil - this is physically unrealistic - but even if that was unimportant for the practical operation of the transformer, it would cause a divide-by-zero error in the simulator if you were to drive pins 1 and 2 from a Voltage source. So the modellers connect a resistor in series between one terminal of L1 and pin 1. They chose to name the pin of L1 as net# 11. So now Rs is connected between pin 1 and net 11, and L1 is connected between net 11 and pin 2. (Pins (or terminals) of a subcircuit are just the specific internal nets that are brought out directly to the outside world).

P.S. I recommend reading up on SPICE in any case. The SPICE3 users manual (the Exeter web copy was linked by JohnDG) is not bad. Larry Nagel's Ph.D thesys, which was the SPICE2 manual, is possibly even better. Andrei Vladimirescu's "The SPICE book" is the best reference book that I've found, and worth the money if you are going to use SPICE for real.

thank you

i've already started on the exeter users manual that was linked. and at the present i am just a curious hobbiest in this matter. but the simulator intriques me. so i am playing with it. i was getting the impression that the nodes were just picked numbers.

thank you your time in answering my question.

now that i look back on the sample. it makes perfect sense the way you explained it.

thanks again.

Go to the following link and look under Basic SPICE Parameter, it explains the basic syntax for this model.

http://zone.ni.com/devzone/cda/tut/p/id/5413

The above model is a 5 terminal model with two pins on the primary side and three pins on the secondary side. The resistors Rs1, Rl2 and Rl3 are the transformer internal resistance. L1 is the primary inductor, L2 and L3 are secondary inductors and they connect to each other at node 5. The K values are coupling coefficient base on the following formula:

K=M/sqr(Ls*Lp) where M is the mutual coefficient.

If you look at the following statement:

K12 L1 L2 9.88-01

It tells you the couple coefficient between L1 and L2 is 9.881-01.

The nodes number can be anything you want as long as it is within the .subckt statement you don't have to worry about duplicate node outside of the component.

If you want to make a 6 pin model with three pins on each side, the model will look something like this:

.subckt 6_pins_transformer 1 2 3 4 5 6

L1 1 2 1

L2 2 3 1

L3 4 5 1

L4 5 61

K1 L1 L3 1

K2 L1 L4 1

K3 L2 L3 1

K4 L2 L4 1

.end

Once you understand the above model, you can create any transfomer model. The next step is to know how to create a custom component in Multisim, the following link will show you how:

http://zone.ni.com/devzone/cda/tut/p/id/3173

Good links - thanks