# Using SPICE to model dV/dt filter for inverter motor drives

I am starting to learn LTSPICE to create model where I can test various passive filter topologies for inverter drives where the output PWM has very short rise times and high switching frequency.

I have managed to create a model which accurately models the voltage reflection using a PULSE source and a lossless line model.

NETLIST as follows:

V1 N001 0 PULSE(0 20 0.1u 0.1u 0.01n 0.3u 1ms) Rser=50
T1 N001 0 N002 0 Td=0.25US Z0=50
T2 N002 0 N003 0 Td=0.25US Z0=50
R1 N003 0 100
.tran 0 1.8us 0 0.1n
.backanno
.end


Figure:

Result:

Green: Voltage pulse from source Blue: Measurement between lossless lines Red: Measurement at cable end (motor terminals)

It is seen that the pulse has a travel time from the source to the motor, and that the motor terminal voltage is higher than the source voltage due to the voltage reflection and impedance mismatch (50 vs 100 ohm). The second pulse in the x-axis is the pulse returning to the source.

# Now, the problem:

When I add filter components, the voltage essentially drops to zero after the filter. This is what I have implemented: I expected that this would damp the overvoltage. The values are extracted from an IEEE paper (A. von Juanne, "Design considerations for an inverter output filter to mitigate the effects of long motor leads in ASD applications")

The resulting voltage measurements look like this: where the green trend still is the source voltage pulse.

The voltage is much lower at the receiving end that what I expected and I hope that someone with better experience than me have some tips to create a model for this scenario.

# UPDATE

I got it to work as expected after being more careful with the parameters and components.

The updated netlist:

V1 N001 0 PULSE(0 648 10u 0.025u 0.01n 1.2u 5us 0) Rser=0
R1 N003 0 1MEG
L1 N001 N002 0.2m
R2 N002 N004 190
C1 N004 0 0.075µ
O1 N002 0 N003 0 PL1
.tran 0 501u 0 1n
.model PL1 LTRA(len=30 R=6m L=0.36u C=0.01n)
.backanno
.end


Updated schematic:

Updated result: From LTSPICE

From original IEEE paper

After exporting the data values and letting LaTeX present the same result

(PS: Dont mind the blue dashed line and 20 % tick, that was just testing)

• You're sending a 1 micro second pulse which the filter averages by squashing and elongating. This seems perfectly normal. What might you have been expecting? Free energy for life? – Andy aka Nov 14 '15 at 15:36
• Well, I was actually hoping to save the world with free energy. But on a more serious note, I fixed the problem and also added a lossy line model. Now the experimental results from the IEEE paper matches the simulation results i have obtained. – fluxmodel Nov 14 '15 at 15:40
• Well don't hang about on this problem too long, our world needs your efforts. – Andy aka Nov 14 '15 at 15:48
• Well, since you solved, you could explain how in your own answer and perhaps get more upvotes for that. Also, on the topic of learning LTspice: you could add net/label names so then you'd have less explaining to do regarding the voltages you're plotting. – Fizz Nov 14 '15 at 18:26
• @fluxmodel You can post answers to your own question in this kind of circumstances. Post your update/solution as an answer and accept that answer. – Nick Alexeev Nov 16 '15 at 4:31