Why is the Schottky diode being used in control circuit?

I would need to know more about the function of the circuit to make an informed comment.

The two transistors are high voltage parts (250V and 500V).

What are the inductor connections and what is the working voltage on emitter of T104 ?

D108 is only rated for 40V reverse voltage.

I suspect that the diode is to protect T103 from negative voltages at TP131 - but without more information its only a guess. 

MK

The two transistors are high voltage parts (250V and 500V)- fuse & inductor path is max60V from Lead-acid battery. This a random selection. 100V part cab used.

What are the inductor connections and what is the working voltage on emitter of T104 ? -  ferrite bead used for High Impedance at high frequency (EMI/EMC) 

D108 is only rated for 40V reverse voltage. - D109, after 100k and 300k, 60V will drop...so they have used 40V schottky

I suspect that the diode is to protect T103 from negative voltages at TP131 - do we get -ve voltage in between?not sure, I thought it's only at product out (Connector/GND...).

Thanks for the efforts️.

Without Schottky it can produce very high voltage spikes during switching off. - you are refereing T103(npn)?. 

as we can see in the 2nd waveform (VC-Q1 - red)  there is high voltage spike...in-turn leading Vc-q2 (orange) -ve spike....

But any how this -ve spike will be suppressed by clamping diode right? so can we remove schottky?...

And can you please share the Simulation settings. If you can share the .asc file that would be great. 

Hi,

With Schottky - the current through the ferrite bead is minimal few micro ampere.
Without Schottky - the current is much more - it produce a current spike, that produce a spike voltage on the Q1 transistor during switching off.
This diode blocks the back current, which will stored in the induction during switching off, it separates Q1 from Q2.
refer what michaelkellet told - flyback diode

-->>> see also switched power supplies, such circuits looking similar.

copy this .docx file to your folder and rename the extension docx to .asc.

Best Regards

Gerald

--

Ok now its clear. Once again thanks for the support

Thank for the efforts and discussions️.

Hello Gerald,

I have replicated your model quite closely in LTSpice and it shows no sign of the huge spikes.

I used a Wurth ferrite bead:

MK

original ferrite bead in the original circuit, Murata BLM18KG101TH1D:

I've selected the Würth ferrite bead 74276051:

Well, may be your simulation have other setting in the software.

I just installed the software and worked with default settings, in the simulation settings.

Just drag and drop, I selected components that have "real" parameters, I did not use ideal components.

In the fused wire draws < 3A at 36V, not mA. This is the power rail.

The measurement circuit is just a small part of a bigger circuit.

You can ask the developers who inserted the Schottky. 

Could you post your .asc file for the simulation an I can try running it here. (I can't copy it as text the way you've posted it above.)

Here is mine:

Version 4.1
SHEET 1 880 692
WIRE -256 -208 -352 -208
WIRE 192 -208 -192 -208
WIRE 320 -208 192 -208
WIRE 192 -176 192 -208
WIRE 320 -112 320 -208
WIRE 192 -64 192 -96
WIRE 256 -64 192 -64
WIRE 192 -32 192 -64
WIRE 560 32 464 32
WIRE 320 64 320 -16
WIRE 464 80 464 32
WIRE 192 112 192 48
WIRE 192 176 192 112
WIRE -352 208 -352 -208
WIRE 320 208 320 144
WIRE 464 208 464 144
WIRE 464 208 320 208
WIRE 688 208 464 208
WIRE -32 224 -128 224
WIRE 80 224 48 224
WIRE 128 224 80 224
WIRE 80 256 80 224
WIRE 320 272 320 208
WIRE 688 272 688 208
WIRE 464 288 464 208
WIRE -128 304 -128 224
WIRE 560 304 560 32
WIRE -352 416 -352 288
WIRE -128 416 -128 384
WIRE -128 416 -352 416
WIRE 80 416 80 336
WIRE 80 416 -128 416
WIRE 192 416 192 272
WIRE 192 416 80 416
WIRE 240 416 192 416
WIRE 320 416 320 352
WIRE 320 416 240 416
WIRE 464 416 464 352
WIRE 464 416 320 416
WIRE 560 416 560 384
WIRE 560 416 464 416
WIRE 688 416 688 336
WIRE 688 416 560 416
WIRE 240 432 240 416
FLAG 240 432 0
FLAG 192 112 Q1_C
FLAG 688 208 OUT
SYMBOL npn 128 176 R0
SYMATTR InstName Q1
SYMATTR Value 2SC4061K
SYMBOL res 64 240 R0
SYMATTR InstName R1
SYMATTR Value 47k
SYMBOL res 64 208 R90
WINDOW 0 0 56 VBottom 2
WINDOW 3 32 56 VTop 2
SYMATTR InstName R2
SYMATTR Value 1k
SYMBOL voltage -128 288 R0
WINDOW 3 -165 160 Left 2
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR Value PULSE(0 3.3 .1 5u 5u 0.1 0.5 3)
SYMATTR InstName V1
SYMBOL voltage -352 192 R0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V2
SYMATTR Value 36
SYMBOL pnp 256 -16 M180
SYMATTR InstName Q2
SYMATTR Value 2SAR340P
SYMBOL res 176 -192 R0
SYMATTR InstName R3
SYMATTR Value 100k
SYMBOL res 176 -48 R0
SYMATTR InstName R4
SYMATTR Value 330k
SYMBOL res 304 48 R0
SYMATTR InstName R5
SYMATTR Value 180k
SYMBOL res 304 256 R0
SYMATTR InstName R6
SYMATTR Value 10.2k
SYMBOL diode 480 352 R180
WINDOW 0 24 64 Left 2
WINDOW 3 24 0 Left 2
SYMATTR InstName D2
SYMATTR Value 1N4148
SYMBOL diode 480 144 R180
WINDOW 0 24 64 Left 2
WINDOW 3 24 0 Left 2
SYMATTR InstName D3
SYMATTR Value 1N4148
SYMBOL voltage 560 288 R0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V3
SYMATTR Value 1.8
SYMBOL cap 672 272 R0
SYMATTR InstName C1
SYMATTR Value 0.47µ
SYMBOL FerriteBead -224 -208 R90
WINDOW 0 -16 0 VBottom 2
SYMATTR InstName L1
SYMATTR Value 600n
SYMATTR SpiceLine Ipk=0.3 Rser=0.219 Rpar=121 Cpar=279f mfg="Würth Elektronik" pn="782422101 WE-CBA 0402"
TEXT -96 -256 Left 2 !.tran 0 5 0

MK

sorry, uploading the .asc file is not allowed.

I uploaded above the .docx file to Humaninsane postings.

Please download this docx file and rename the extension from .docx to asc.

I use the newest version of LTSpice. Please update it or download it.

geralds said:

I uploaded above the .docx file to Humaninsane postings.

I know that's what you tried to do but the rendering of that upload is incomplete and if it is downloaded MS Word can't decode it. The easy way to this is to just paste the text into a post.

Thanks.

MK

WARNING - LONG REPLY BUT WITH A HAPPY ENDING

Found I could download as a .pdf and translate that.

But - no overshoots:

Same overshoot result if I press reset to defaults and run again.

Updated to latest version.

And huge overshoot on Q1 collector is visible.

No picture of it here - see Geralds plots above.

But we know this is false because there is no big overshoot on the 36V power rail:

Let's remove the inductor:

Now we have a design with NO INDUCTANCE but we still get the 200V spike.

Analog seem to have broken LTSpice.

let's prove that:

There you are - no inductance and we get the nonsense spike.

This is so disappointing - LTSpice has been great for ages and now they have broken it.

The spike varies if you change the transistor model to npn2 or the type of device but it doesn't go away.

So let's find out what's wrong,

........................ several abortive tests I won't bore you with.

Here is a clue - only one rising edge is spikey, and less than they were, but all I've done is change the quiet intervals between edges.

Lets make a wild guess and set the minimum time step to 1us (its at the default setting of whatever it decides right now)

Suddenly it looks sensible.

And if the min time step is set then Gerald's original model works OK as well.

So all they have changed/broken is how the auto time step works - I preferred the older version.

So the take away from this - never trust a simulator - the hierarchy of truth is:

Lies

Damn lies

Statistics

SImulators

AI

But we have learnt that we don't need a diode in the collector circuit of Q1.

MK

MK

WARNING - LONG REPLY BUT WITH A HAPPY ENDING

Found I could download as a .pdf and translate that.

But - no overshoots:

Same overshoot result if I press reset to defaults and run again.

Updated to latest version.

And huge overshoot on Q1 collector is visible.

No picture of it here - see Geralds plots above.

But we know this is false because there is no big overshoot on the 36V power rail:

Let's remove the inductor:

Now we have a design with NO INDUCTANCE but we still get the 200V spike.

Analog seem to have broken LTSpice.

let's prove that:

There you are - no inductance and we get the nonsense spike.

This is so disappointing - LTSpice has been great for ages and now they have broken it.

The spike varies if you change the transistor model to npn2 or the type of device but it doesn't go away.

So let's find out what's wrong,

........................ several abortive tests I won't bore you with.

Here is a clue - only one rising edge is spikey, and less than they were, but all I've done is change the quiet intervals between edges.

Lets make a wild guess and set the minimum time step to 1us (its at the default setting of whatever it decides right now)

Suddenly it looks sensible.

And if the min time step is set then Gerald's original model works OK as well.

So all they have changed/broken is how the auto time step works - I preferred the older version.

So the take away from this - never trust a simulator - the hierarchy of truth is:

Lies

Damn lies

Statistics

SImulators

AI

But we have learnt that we don't need a diode in the collector circuit of Q1.

MK

MK