1. LTspice
  2. Теми

Input filter + LT3845A Middlebrook Question

 

Hi all,
 
I am a little stumped on how to appropriately model the combination of an input filter and converter power stage for use in determining whether the Middlebrook criteria are met.
 
Here is my best attempt at a simulation; I have made a Comment for what I plotted that I think would be used to determine Middlebrook compliance:
 
I based how I set up this simulation on this paper (which is of course based on Middlebrook's):
Specifically, Figures 4 and 8 were my guide.
 
Any help is greatly appreciated,
-M
 

On Thu, Dec 12, 2024 at 03:37 PM, May wrote:
  • The command ".lib OptiMOS5_100V_LTSpice.lib" is not needed, and anyway that file is missing so the line needs to be deleted.
  • The signals TG1, TG2, BG1, and BG2 are not driven by anything.  I don't think your circuit could do anything useful when the MOSFET Gates are un-driven and floating.  At the least, I think they ought to be tied high or low, don't you?
 
Andy
 
 

I noticed some non-standard nomenclature, but you were lucky because it seems to work:
 
Some of your capacitors have "x2" or "x4" or "x6" parameters, apparently as multipliers.  As far as I know, this is improper.  The standard SPICE syntax for scaling a capacitor is "m=<value>".  Therefore, one should write "m=4" not "x4".  LTspice seems to understand how to translate your "x4" into "m=4" in the expanded netlist - but this is UNDOCUMENTED.  Because it is not documented, you may consider yourself lucky that it works, and understand that it might not work next week or next year.

Also, is it proper to ground both ends of the common-mode choke, L4 pins 5 and 6?  Admittedly it may have no effect on this simulation.
 
Andy
 
 

One other thing -
 
Where is the LT3845A?
 
It appears to be missing from your simulation.
 
Andy
 
 

I think the "x2" notation is mentioned in some post on the Analog Devices website: link, but is not in the LTspice docs.

It is probably easier to do two simulations to confirm Middlebrook criteria. 1, for the output impedance of the input filter, and 2, for the input impedance of the DC/DC converter.

To measure the output impedance, simply connect the AC source you have in parallel with the output of the filter (bus_filt_i to GND). Then you can just plot V(bus_filt_i)/I(V3) to get the output impedance in ohms.
As for the input impedance of the converter, that can be simulated, or estimated based on equation 12 in your linked paper.

If you want to do a combined simulation you are going to need to do a time transient simulation (with the missing DC/DC converter), not an AC sweep.

Eric Sims

(and it's a small world... tell Matt V I say "Hi")

On Thu, Dec 12, 2024 at 3:08 PM Andy I via groups.io <AI.egrps+io=gmail.com@groups.io> wrote:
I noticed some non-standard nomenclature, but you were lucky because it seems to work:
 
Some of your capacitors have "x2" or "x4" or "x6" parameters, apparently as multipliers.  As far as I know, this is improper.  The standard SPICE syntax for scaling a capacitor is "m=<value>".  Therefore, one should write "m=4" not "x4".  LTspice seems to understand how to translate your "x4" into "m=4" in the expanded netlist - but this is UNDOCUMENTED.  Because it is not documented, you may consider yourself lucky that it works, and understand that it might not work next week or next year.

Also, is it proper to ground both ends of the common-mode choke, L4 pins 5 and 6?  Admittedly it may have no effect on this simulation.
 
Andy
 

1 - 5 з 5