paralleled inductors in cadence virtuoso

It's not Virtuoso that has a problem with this, it's Spectre (the simulator). See  RE: "the following branches form a loop of rigid branches"  where talk about this a bit. Since at DC, you have two shorts in parallel, there's no way to solve for the current flowing through each inductor numerically because the current flowing through each of the parallel inductors could be split in an infinite number of ways (so hence this is an ill-conditioned matrix to solve).

This is only an issue with ideal inductors though - once there's some series impedance that would prevent the problem.

Andrew

It's not Virtuoso that has a problem with this, it's Spectre (the simulator). See  RE: "the following branches form a loop of rigid branches"  where talk about this a bit. Since at DC, you have two shorts in parallel, there's no way to solve for the current flowing through each inductor numerically because the current flowing through each of the parallel inductors could be split in an infinite number of ways (so hence this is an ill-conditioned matrix to solve).

This is only an issue with ideal inductors though - once there's some series impedance that would prevent the problem.

Andrew

Thank you. But when I changed to transient simulation, the parallel connection of the two inductors still reported an error. Why?

I just want to verify that the ratio of the current value of the two inductors is equal to the inverse ratio of the inductance value.

Just like its dual circuit, the voltage of the capacitor is inversely proportional to the value of the capacitor (Spectre has successfully shown the simulation results).

Spectre can simulate one of these two dual circuits but not the other? This is really weird. In other words, is there any way I can simulate the theory that the ratio of the current value of two parallel inductors is equal to the inverse ratio of the inductance value?

The transient simulation starts with a DC analysis to find the initial starting point - and DC signals still effectively end up with the inductor shorted, so it has the same problem for the DC component.

Series capacitors are open circuit, and so there's no problem with solving that - the current through the capacitors is zero. The Vout node would be floating, and so that potentially would be ambiguous and lead to an infinite number of solutions, but spectre inserts a "gmin" impedance to ground (1e-12 Siemens, or 1e12 Ohms) from floating nodes which will mean that the Vout node in your series cap circuit becomes well-defined.

You can simply add a small resistance in series with the inductors. Given that it's not a good idea (for convergence reasons) to put very small resistances in the circuit with Spectre (this is all to do with solving Kirchoff's current law accurately as well as the normal convergence criteria), I used 1mOhm for the series resistance (in general it's unadvisable to use smaller resistors than this with Spectre). It then doesn't make sense to do your measurement at 1kHz, because the 1nH inductor will only have 6.28uOhms and so the currents would be dominated by the series resistors (which would be the same for both inductors). If I simulate with (say) 100MHz sine sources, then you can clearly see the effect (not really sure why you're trying to prove basic electrical theory with a simulator):

// spectre netlist for inductors in parallel with series resistance to avoid loop of rigid branches

Isin (n1 0) isource type=sine freq=100M ampl=6
R1 (n1 l7) resistor r=1m
L7 (l7 0) inductor l=5n
R8 (n1 l8) resistor r=1m
L8 (l8 0) inductor l=1n

save n1 L7:1 L8:1
tran tran stop=100n

Regards,

Andrew

Wow! You are so proficient in Spectre. Therefore, according to your statement, as long as the inductance is connected in parallel in Spectre (ideal inductance, no resistance), an error will be reported under any circumstances, right? Because I just started learning the virtuoso software suite. I feel that Spectre is very powerful and amazing, and I became interested in the operating principle of the simulation software. I just want to use it to verify some of the circuit theories I have learned, so as to find out how to use the software. Is this inappropriate? Thanks a million.

It's OK to do that - you just need to remember that circuit simulators use numerical methods (iterative solvers) to solve the circuit equations, and are optimised for real-life circuits rather than ideal components, so sometimes you need to make things slightly less than ideal to allow you to simulate them. Of course, in real life there never is a perfect inductor with zero DC impedance - and whilst you can do the maths analytically if you are using ideal components, the iterative solvers can't handle that so easily. We have to use numerical methods because it's not feasible to exactly solve a set of nonlinear simultaneous differential equations in practice.

Anyway, glad it helped!

Andrew

Many thanks for your kind and warm help.