BUG: LTSpice calculates wrong inductor current

Hi Udo ,

I see. Will look into this.

mike

I don't see anything wrong with the result. Plotted I(L1) climbs to 24mA, following the same shape as Vcc.

In my simulation the final current is wrong for small inductor values.

I can't observe the same behavior, looks normal to me. Same with different solver and integration methods. This is with LTspice 26.0.2

Hi Udo , mtwieghr ,

mtwieghr said:

I can't observe the same behavior, looks normal to me. Same with different solver and integration methods. This is with LTspice 26.0.2

Interesting, I was able to reproduce the exact behavior that Udo  shows, in both 26.0.2 and in LTspice XVII. I wonder why mtwieghr is not seeing it?

mike

I just tried it on another machine and that shows the problem exactly the same as in Udo's screenshot. Both machines are running the same LTspice version, but different versions of windows (the machine which shows the problem is 11, the machine that shows no problem is 10). That doesn't prove the windows version is actually related to the issue though.... shrug.

Hi Udo , mtwieghr ,

mtwieghr said:

Both machines are running the same LTspice version, but different versions of windows (the machine which shows the problem is 11, the machine that shows no problem is 10).

Interesting. I will look at the Windows effect further.

In the meantime, I do have an answer to why you see the result at all, and yes, it is not a Windows problem, it is LTspice…

LTspice optimizes the simulation of parasitics, which usually results in a vanishingly small error when using typical circuit elements. e.g. Inductors with relatively low DCR. The trade-off, as you've found, is that the resulting error can be significant in some atypical designs, such as yours. In your case, you can workaround this problem by breaking out the parasitic resistance into a series resistor and assigning the default 1mΩ Rser in the inductor. You could also make Rser zero by putting in a "0", but we would advise against that for the sake of convergence.

mike

Hi Mike,

I tested with Win10 and Win11 and it makes no difference.

I sometimes use an inductor with a series resistor to simulate a resistor with parasitics. Unfortunately LTspice resistors do not have parasitics build in. In this use case the bug causes very serious errors. For examples if you change the 1n-1kOhm combination to 1p-1kOhm the error climbs to 24 Ampere!

It would be best to fix the problem at the root, but i can accept the solution with the external series resistor.

Udo

Hi Udo ,

Udo said:

It would be best to fix the problem at the root, but i can accept the solution with the external series resistor

Noted, and this change is being considered. This is a very old design decision that would take some time and testing to change; essentially ensuring it doesn't break existing designs.

mike

Hi Mike,

I did some more tests and the bug disappears if i added Rpar=1T, the value of Rpar does not matter as long as it is high enough.

This could provide a quick fix. 

Some more tests with capacitors and different Rser/Rpar show no problems.

Udo