Review this Goofy 555 Based SMPS Design

[Henry Kiefer]

| The ironic thing is LTSpice SwitchercadIII was probably made to sell
| LT controllers but I'm controlling with cheapo 555's instead.

In the next version of LTspice Mike seeks for the string 555 in open documents and if it finds, it executes del *.*

Oh I forgot to add /s

Have fun!
- Henry

 

[Henry Kiefer]

| On 21 Jan 2007 23:38:42 -0800, [email protected] wrote:
|
| >Dell used to roll their own Dc/DC converters with 555s. Well, the key
| >phrase is "used to."
|
| Do you know if it was hysteretic or PWM?
| I recall seeing an app note one time for turning the 555 into a PWM.
| D from BC

I guess I saw one in a Supertex SMPS app note.

- Henry

 

[Jim Thompson]

What advantage (apart from including a few resistors) do you
get by using the C555s, instead of a dual comparator?

It's a feel-good kind of thing ;-)

...Jim Thompson

 

[John Popelish]

I picked CMOS 555..just because it had that cool parallel processing
look to it.
Also.... it's one of the most ancient IC's and a text book item. Using
it in the cct. has an artistic quality.

What advantage (apart from including a few resistors) do you
get by using the C555s, instead of a dual comparator?

 

[D from BC]

What advantage (apart from including a few resistors) do you
get by using the C555s, instead of a dual comparator?

I had to pick one of the following methods:
* Schmitt inverter or schmitt gates
* Comparator with hysteresis control pin
* Positive feedback or feedback to a switch
* 2 comparators and a discrete SR latch
* CMOS 555

I had to pick something... I've never used the 555 this way before and
I liked the newness factor.
Besides..prop delay, I draw, Vs specs fit the app ok.

I posted about hysteresis methods some time ago. IIRC somebody bashed
the positive feedback method in favor of the SR method.

I haven't done a study to compare the methods for an
economic/performance fitting in my app.
It was one of those "works....good enough...move on...." decisions.
Also..it's hobby electronics...I can do artsy stuff like that

To really answer your question...
I dunno...
D from BC

 

[D from BC]

| The ironic thing is LTSpice SwitchercadIII was probably made to sell
| LT controllers but I'm controlling with cheapo 555's instead.

In the next version of LTspice Mike seeks for the string 555 in open documents and if it finds, it executes del *.*

Oh I forgot to add /s

Have fun!
- Henry

But I am using the LT op amps and might get suckered into using them..


D from BC

 

[John Popelish]

I had to pick one of the following methods:
* Schmitt inverter or schmitt gates
* Comparator with hysteresis control pin
* Positive feedback or feedback to a switch
* 2 comparators and a discrete SR latch
* CMOS 555

I had to pick something... I've never used the 555 this way before and
I liked the newness factor.
Besides..prop delay, I draw, Vs specs fit the app ok.

I posted about hysteresis methods some time ago. IIRC somebody bashed
the positive feedback method in favor of the SR method.

I haven't done a study to compare the methods for an
economic/performance fitting in my app.
It was one of those "works....good enough...move on...." decisions.
Also..it's hobby electronics...I can do artsy stuff like that

To really answer your question...
I dunno...

Fair enough. Shouldn't you add a third C555 to control
output voltage? Add a pulsed switch that adds enough load
to take the current above and below the current limit on a
regular basis, to see how well both voltage and current
regulation work.

BTW, you don't need the resistors on the 555 outputs.

 

[D from BC]

D from BC wrote: [snip]
It was one of those "works....good enough...move on...." decisions.
Also..it's hobby electronics...I can do artsy stuff like that

To really answer your question...
I dunno...

Fair enough. Shouldn't you add a third C555 to control
output voltage? Add a pulsed switch that adds enough load
to take the current above and below the current limit on a
regular basis, to see how well both voltage and current
regulation work.

BTW, you don't need the resistors on the 555 outputs.

This is a constant current type power supply.
I probably have to add voltage feedback in case the output voltage
gets crazy with no load. But not with another 555. Probably a
zener/resistor to U2.

I'll be doing "jumpy" load regulation tests later on.. For now, it's
good for a static resistive load.
I did catch some literature about CPU's being powered up with
hysteresis type controllers. Fast response to loading?

You probably saw the jpeg...The PDF has a mouse over note that
mentions the 555 out resistors. I have to include those resistors in
LTSpice to see the waveforms... It's cool to see the mode change from
input current regulation to output current regulation.

I'm currently checking to see how sluggish of an op amp I can use in
the high side cct. I can't get the LT1784 to sim for some reason..
This is to reduce Q1 dissipation.
D from BC

 

[John Popelish]

This is a constant current type power supply.
I probably have to add voltage feedback in case the output voltage
gets crazy with no load. But not with another 555. Probably a
zener/resistor to U2.

I'll be doing "jumpy" load regulation tests later on.. For now, it's
good for a static resistive load.
I did catch some literature about CPU's being powered up with
hysteresis type controllers. Fast response to loading?

You probably saw the jpeg...The PDF has a mouse over note that
mentions the 555 out resistors. I have to include those resistors in
LTSpice to see the waveforms... It's cool to see the mode change from
input current regulation to output current regulation.

(snip)

No. I have been playing with the simulation in LTspice.
After I eliminated the 555 output resistors, I watched the
two 555s trade off control by displaying the current into
each discharge pin.

 

[D from BC]

No. I have been playing with the simulation in LTspice.
After I eliminated the 555 output resistors, I watched the
two 555s trade off control by displaying the current into
each discharge pin.

I'm new to this prog..At first I clicked like crazy on the output pins
and nothing..So I placed the resistors... Might be some left over
habit from Circuitmaker 2000 where pins often need to be connected.
I checked with just drawing a piece of wire at the pin in LTSpice...
Then I got the signal..
D from BC

 

[John Popelish]

I'm new to this prog..At first I clicked like crazy on the output pins
and nothing..So I placed the resistors... Might be some left over
habit from Circuitmaker 2000 where pins often need to be connected.
I checked with just drawing a piece of wire at the pin in LTSpice...
Then I got the signal..

When you put the curser directly over the pin, a clamp on
current probe, with an arrow through it that shows the
direction of a positive current should appear. Left click
there, and a current trace should appear on the graph. This
is especially handy if you are also graphing large voltage
swings from other nodes, that make the low voltage pin trace
very small. The current trace gets its own scale factor, on
the right side of the graph.

 

[Henry Kiefer]

| On Mon, 22 Jan 2007 12:20:50 +0100, "Henry Kiefer"
|
| >| The ironic thing is LTSpice SwitchercadIII was probably made to sell
| >| LT controllers but I'm controlling with cheapo 555's instead.
| >
| >In the next version of LTspice Mike seeks for the string 555 in open documents and if it finds, it executes del *.*
| >
| >Oh I forgot to add /s
| >
| >Have fun!
| >- Henry
|
| But I am using the LT op amps and might get suckered into using them..
|

Double check that no LT op amp type number includes 555 !

- Henry

 

[D from BC]

Maybe you might know....

I'm trying to replace U1 with a lower a GBW op amp. This is to lower
Q1 dissipation.
Trying LT6221.

I'm absolutely stumped...
There's some sort of breakdown effect but the timing is random in
LTspice.
Looks like very narrow HV "clicks" at the 555 U3 trigger input.

Is this for real? It doesn't happen with the 80Mhz GBW LT1800 op amp.

Notes:
1)Inductor parallel capacitance is estimated at 3pF. Added filter..Not
it...
2) Using latest LTC.lib file from LT.
3) Tried LT1784, LT6237 ..same effect
4) Schematic on
http://www.members.shaw.ca/chainsaw/SED/556BasedCuk.pdf

D from BC

 

[John Popelish]

Maybe you might know....

I'm trying to replace U1 with a lower a GBW op amp. This is to lower
Q1 dissipation.
Trying LT6221.

I'm absolutely stumped...
There's some sort of breakdown effect but the timing is random in
LTspice.
Looks like very narrow HV "clicks" at the 555 U3 trigger input.

Is this for real? It doesn't happen with the 80Mhz GBW LT1800 op amp.

Notes:
1)Inductor parallel capacitance is estimated at 3pF. Added filter..Not
it...
2) Using latest LTC.lib file from LT.
3) Tried LT1784, LT6237 ..same effect
4) Schematic on
http://www.members.shaw.ca/chainsaw/SED/556BasedCuk.pdf

I don't think it is real, though you might want to eliminate
the minimum time step in the tran setup and add a small
capacitor across D1 (I used a .1u). That seems to get rid
of the problem on this end.

You might do your experiments with the UniversalOpamp2 at
the far end of the opamp list. It has completely
programmable gain bandwidth, slew rate and phase margin so
you can really find out where the limit is. Then you just
have to find an opamp that exceeds the minimum performance.

 

[D from BC]

Maybe you might know....

I'm trying to replace U1 with a lower a GBW op amp. This is to lower
Q1 dissipation.
Trying LT6221.

[snip]

I don't think it is real, though you might want to eliminate
the minimum time step in the tran setup and add a small
capacitor across D1 (I used a .1u). That seems to get rid
of the problem on this end.

You might do your experiments with the UniversalOpamp2 at
the far end of the opamp list. It has completely
programmable gain bandwidth, slew rate and phase margin so
you can really find out where the limit is. Then you just
have to find an opamp that exceeds the minimum performance.

I got the fake "clicks" from the high side cct greatly reduced but not
eliminated. Will ignore .....Something is probably different at my
end.
Great! I'll use that user defined opamp model... Thanks.

I'll be posting a new schematic when I get the following done:
1) HV linear regulator
2) Parts optimized for low power with respect to mos drive power
dissipation.
3) Adding failsafe parts and bypassing

D from BC

 

[[email protected]]

buck converter based around an HC14 (which is now my preferred PWM
contoller)

Cheers
Terry

I wasn't involved in the study. As you probably know, most IC companies
open up products to see who is using what. So more correctly I was
told Dell was using 555 circuits.

There are so many things that can go wrong in DC/DC design that I can't
ever see not using a real controller chip. Start up and undervoltage
lockout can be a real headache.

 

[D from BC]

This 555 based smps is a design challenge + LTSpice learning
project...so I'm not sure if my question below is steering away from
the "spirit" of sci.electronics.design..

I got the Zetex spice library... zmodels.lib.
I copied and renamed a PMOS symbol file..That looks ok.

Now for the syntax editing?

I get this message in LTSpice:
Error on line 2 : m1 0 n003 n002 n002 zmodels.lib zvp2120g
Unable to find definition of model - default assumed

The Zetex library section:

*ZETEX ZVP2120G Spice Model v1.0 Last Revised 10/8/05
*
..SUBCKT ZVP2120G 3 4 5
* D G S
M1 13 20 5 5 Pmod1
RG 4 2 100
RIN 2 5 1E9
RL 3 5 1.2E8
RD 3 13 Rmod1 22
C1 2 5 55E-12
**C2 3 2 15E-12
D1 3 5 Dmod1
D2 3 17 Dmod2
Egs1 2 17 2 5 1
Egt1 2 20 5 21 1
Vgt1 5 22 1
Igt1 5 21 1
Rgt 21 22 Rmod2 1
..MODEL Pmod1 PMOS VTO=-2.8 RS=2 IS=1E-15 KP=0.17
+CBD=60E-12 PB=1 LAMBDA=6E-3
..MODEL Dmod1 D IS=5E-12 RS=2 BV=220
..MODEL Dmod2 D CJO=70e-12 IS=1e-30 N=10
..MODEL Rmod1 RES (TC1=4.5e-3 TC2=4E-5)
..MODEL Rmod2 RES (TC1=-2.5e-3 TC2=3e-6)
..ENDS ZVP2120G
*
*$

It's probably a dum question, but I'm afraid to burn too much time
researching spice syntax differences..
How do I edit the ZVP2120 subckt so I can sim this Zetex PMOS?
Links?

D from BC

 

[Jim Thompson]

This 555 based smps is a design challenge + LTSpice learning
project...so I'm not sure if my question below is steering away from
the "spirit" of sci.electronics.design..

I got the Zetex spice library... zmodels.lib.
I copied and renamed a PMOS symbol file..That looks ok.

Now for the syntax editing?

I get this message in LTSpice:
Error on line 2 : m1 0 n003 n002 n002 zmodels.lib zvp2120g
Unable to find definition of model - default assumed

I'm only a casual user of LTSpice, but I'd guess it's a device call
issue....

The ZVP2120G is defined via a _SUBCKT_

Thus it must be called in the netlist:

XM1 0 N003 N002 N002 ZVP2120G ; NOTE the "X"

and you need the library...

..LIB Drive\Path\zmodels.lib

I've not seen calling the library in the same line as the device.

The Zetex library section:

*ZETEX ZVP2120G Spice Model v1.0 Last Revised 10/8/05
*
.SUBCKT ZVP2120G 3 4 5
* D G S
M1 13 20 5 5 Pmod1
RG 4 2 100
RIN 2 5 1E9
RL 3 5 1.2E8
RD 3 13 Rmod1 22
C1 2 5 55E-12
**C2 3 2 15E-12
D1 3 5 Dmod1
D2 3 17 Dmod2
Egs1 2 17 2 5 1
Egt1 2 20 5 21 1
Vgt1 5 22 1
Igt1 5 21 1
Rgt 21 22 Rmod2 1
.MODEL Pmod1 PMOS VTO=-2.8 RS=2 IS=1E-15 KP=0.17
+CBD=60E-12 PB=1 LAMBDA=6E-3
.MODEL Dmod1 D IS=5E-12 RS=2 BV=220
.MODEL Dmod2 D CJO=70e-12 IS=1e-30 N=10
.MODEL Rmod1 RES (TC1=4.5e-3 TC2=4E-5)
.MODEL Rmod2 RES (TC1=-2.5e-3 TC2=3e-6)
.ENDS ZVP2120G
*
*$

It's probably a dum question, but I'm afraid to burn too much time
researching spice syntax differences..
How do I edit the ZVP2120 subckt so I can sim this Zetex PMOS?
Links?

D from BC

...Jim Thompson

 

[D from BC]

Here's a possibly obscure problem...

I found the Zetex high side current monitor IC...
What I can't figure out is how can I get offset current control?
....Preferably, without splitting the current path from the Iout pin
with a constant current source. It's gotta be a high side adjustment.
Expressed by math: Iout = Vsense*1.2/Rshunt - (Ioffset?)
Or expressed: Iout = ACcurrent - DCcurrent(offset)

No internal schematic on the data sheet.
http://www.zetex.com/3.0/pdf/zxct1011.pdf


Or should I just drop that idea and stick with the op amp/transistor
feedback combo ? R8 offsets Ir4 current by about 0.6mA.
As seen on:
http://www.members.shaw.ca/chainsaw/SED/556Cuk.pdf

If I go with the Zetex IC; I'll use a cascode cct so as not to
overvolt the IC.
D from BC

 

[Genome]

Here's a possibly obscure problem...

I found the Zetex high side current monitor IC...

D from BC

Just in case.......

In a CUK converter the average switch current is the input current.(?) You
might try a source sense resistor followed by an integrating op-amp stage to
reconstruct a facsimile of the input current. Then you won't need high side
sensing.

DNA