I've been trying to design a PSU for a HifiBerry DAC+.
Since the feed point is (in fact) a decent regulator, I'm just trying to get the high frequency trash cleaned up, so I'm using a CRCRC circuit.
I was going OK with a simple SINE voltage source. Noise was down at -120Db at 1KHz. Voltage had minor ripple, but at low freq - that's what regulators handle really well.
But since I was concerned about the nasty wave forms that diodes can (I'm told) generate, I changed the input side of my circuit to have a SINE source representing the secondary of a transformer, and a bridge rectifier.
This simulates fine and reasonably under .tran, but under .ac the noise is now down at -540Db. Which is a little too good to be credible. Something's wrong.
I upgrade my LTSpice-under-Wine-Under-Ubuntu from IV to XVII (oops, version drift) with the same result.
I've attached my crazy sim run, and the asc file. Can anyone see what dumb-*** newb mistake I've made?
BugBear
Since the feed point is (in fact) a decent regulator, I'm just trying to get the high frequency trash cleaned up, so I'm using a CRCRC circuit.
I was going OK with a simple SINE voltage source. Noise was down at -120Db at 1KHz. Voltage had minor ripple, but at low freq - that's what regulators handle really well.
But since I was concerned about the nasty wave forms that diodes can (I'm told) generate, I changed the input side of my circuit to have a SINE source representing the secondary of a transformer, and a bridge rectifier.
This simulates fine and reasonably under .tran, but under .ac the noise is now down at -540Db. Which is a little too good to be credible. Something's wrong.
I upgrade my LTSpice-under-Wine-Under-Ubuntu from IV to XVII (oops, version drift) with the same result.
I've attached my crazy sim run, and the asc file. Can anyone see what dumb-*** newb mistake I've made?
BugBear
Attachments
Does that mean that (in effect) the signal isn't getting past the rectifier at all, and all I'm seeing on the output is noise?
I could understand that.
I shall go and look up what that means (since I don't know)
Thank you!
BugBear
Yes, actually you are only seeing calculation artifacts / resolution limits, not any type of noise (.AC analysis is noise-free). Your DC operation point is 0V, the diodes don't conduct at all. The scale value for an AC source is just that, a scale value. You can use 1uV or 100MegaV, it just scales the display. No actual voltage is presented to the circuit.
.opt plotwinsize=0 switches off the file size compression of the output data used for display. Think sort of MP3 vs WAV.
For the new LTspice version it might not be needed to locate this statement in the sim file directly, I don't know, and I will never upgrade from IV...
Last edited:
Looks like you made a couple of rookie mistakes.
1. Forgot to select a diode model. Your simulation schematic shows that you used a diode called "D" ... which is an ideal diode and decidedly not available in the real world. I suggest you choose diode 1N4004 for simulation studies
2. Connected AC stimulus incorrectly. To get the answer you want, replace the input by two voltage sources connected in series. The first one is (7.5V DC, 0V AC) and the second one is (0V DC, 1V AC). This will let you get the answer you want in .AC analysis
2. Connected AC stimulus incorrectly. To get the answer you want, replace the input by two voltage sources connected in series. The first one is (7.5V DC, 0V AC) and the second one is (0V DC, 1V AC). This will let you get the answer you want in .AC analysis
Thank you. Does this mean I (in fact) need slightly different models for different simulations?
Is there an easy way to manage this, other then (re)editing the model for the two sims?
(I've changed the diodes as recommended; I wasn't planning to worry about component selection until I had the sims running OK; there seemed little point).
BugBear
Yikes, you're right. I've been using it for so long that I forgot I had downloaded it.
For those who want to simulate an 1N4004, Diodes Inc makes a SPICE model available on this web page -- look for the phrase "SPICE model". Or for those who just want to simulate with a real world 1 amp diode and find out whether 1kHz on the AC mains is (or is not) attenuated by 540dB, you can use the presupplied diode model of
- ES1D, or
- 1SR154-400
Here's what I get in AC analysis, assuming ESR = 50 milliohms and ESL = 5 nanohenrys.
The ultra low frequency response at the left edge of the plot is less than 0 dB, thanks to the voltage dropped across the two 1.5 ohm series resistors in the CRCRC filter. They form a voltage divider with the load resistor, guaranteeing that Vout < Vin.
_
The ultra low frequency response at the left edge of the plot is less than 0 dB, thanks to the voltage dropped across the two 1.5 ohm series resistors in the CRCRC filter. They form a voltage divider with the load resistor, guaranteeing that Vout < Vin.
_
Attachments
Expanding the selection window and clicking on the column label should sort the list in order. I know it works for 'type' when I'm hunting zeners.
That's very much what I'm after; I'm trying to avoid feeding the Regulator the sort of (audio freq) stuff it can't filter out itself.
BugBear
The spec sheet doesn't even bother giving a figure at 1Khz, but it's 70dB at 10KHz.
ADP150 Datasheet and Product Info | Analog Devices
BugBear
- Status
- This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.