Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Toroidal Drive analysis using ltspice.

Dragnovith

Newbie level 5
Joined
Apr 17, 2021
Messages
8
Helped
0
Reputation
0
Reaction score
0
Trophy points
1
Activity points
70
Hello, I am designing this circuit to feed a coil. I had never worked with a flip flop in the ltspice and I am having difficulties.

The 3 kHz square wave generated by the first stage of the circuit needs to be divided by a ratio of 2 and become 1.5 kHz. But I've tried everything and nothing makes the flipflop work.

Then I need to turn the voltage into a current. Is it better to use the photo circuit or the Ground Load Voltage to Current Converter?

circuit.jpeg

thanks!
 

Attachments

  • coil_feed.rar
    973 bytes · Views: 2

KlausST

Super Moderator
Staff member
Joined
Apr 17, 2014
Messages
19,717
Helped
4,343
Reputation
8,695
Reaction score
4,304
Trophy points
1,393
Activity points
130,522
Hi,

Your U3 has:
* high differential input voltage (saturated)
* output at the rails (saturated)
This is not how an OPAMP is operated, this is how a comparator is meant to work.
While the LT1013 is not critical with this (many other Opamps may not operate correctly this way) you have ti live with it's drawbacks, like slow slew rate, delay due to saturation, maybe even latch up.
My recommendation: Treat/use an Opamp and comparator respectively like they are meant to work.

The sane applies to U2. It has "quasi" digital input and output.--> use a comparator.
I don't know what you expect it to do. It is used like an "analog unity gain buffer". You signal is not abalog. I guess it makes the digital signal worse than it was before.
For signal shaping: --> Use a comparator.

Sadly your flipflop shows no power supply, thus it's impossible to see the valid input voltage range.
Generally the input voltage should be within it's supply voltage rails (only a little overvoltage allowed)
--> A real FF may be destroied the way you treat it.
There is no part number, so I'm not sure about it'input levels. I guess 0V/5V. You are way beyond.
Then according naming you
* activate "PRE" and you
* activate "CLR"
What's the use of it?
--> I'd rather not_activate them by connecting them to GND.

U1 --> same as U2. You treat an analog part like a digital part

U4 .. at least connected as an analog amplifier. It will amplify the input voltage by a gain of +2.
I guess the input voltage is 0V / 5V, thus the output may amplified to become 0V / 10V.
But the input stage may be temporarily saturated by the too high dV/dt.

I can't see how and where you want to convert voltage into current.
Which voltage?
Which current?
--> The easiest way to convert voltage to current is a simple resistor.

I guess you need to give sime more infirmation for us to understand what (and how) you want to achieve.

Klaus
 

FvM

Super Moderator
Staff member
Joined
Jan 22, 2008
Messages
48,396
Helped
14,251
Reputation
28,763
Reaction score
12,937
Trophy points
1,393
Location
Bochum, Germany
Activity points
280,075
As already stated, the LTspice generic FF has positive CLR and PRE inputs, they must be connected to ground or simply unconnected to make the FF operate.

A floating coil can be connected in series with R4 as indicated below to get current drive. For grounded load use a Howland current source.
Sadly your flipflop shows no power supply, thus it's impossible to see the valid input voltage range.
Default supply of generic logic devices is 1V. Read in LTspice help "A. Special Functions" how to change it. There's no limitation of input voltage, just a mid-supply threshold voltage.

Of course you need to think about input voltage range when designing real hardware, not yet addressed in the thread.


1619941974093.png
 

KlausST

Super Moderator
Staff member
Joined
Apr 17, 2014
Messages
19,717
Helped
4,343
Reputation
8,695
Reaction score
4,304
Trophy points
1,393
Activity points
130,522
Default supply of generic logic devices is 1V. Read in LTspice help "A. Special Functions" how to change it. There's no limitation of input voltage, just a mid-supply threshold voltage.
Yes...I'm not that experienced with LTspice. I just generally wanted to point out that some parts of a simulation differs with reality.

Addressed to the simulation tools and their developers:

So often - especially unexperienced electronic designers - simulate a circuit ... and expect it to work in reality as if in simulation.
The example above shows that this is not the case.
Sadly not. And often it is hard to find. For sure reading the "help" may answer some questions.

My opinion: If it has power supplies that need to be connected (as in reality) it is more "visible" what's the input voltage limit, and where's the swutching threshold.
I don't understand why simulation tools try to simulate "real circuits" ... but then differ in most basics like power supply or clock input...

Klaus

 

Dragnovith

Newbie level 5
Joined
Apr 17, 2021
Messages
8
Helped
0
Reputation
0
Reaction score
0
Trophy points
1
Activity points
70
While the LT1013 is not critical with this (many other Opamps may not operate correctly this way) you have ti live with it's drawbacks, like slow slew rate, delay due to saturation, maybe even latch up.
I replaced the opamp with LT16323 which has 45V / µs and and the square wave was perfect.
Default supply of generic logic devices is 1V. Read in LTspice help "A. Special Functions" how to change it. There's no limitation of input voltage, just a mid-supply threshold voltage.
I read this, but I don't understand if this is a parameter that changes within the DFLOP settings.
I guess you need to give sime more infirmation for us to understand what (and how) you want to achieve.
This circuit will then arrive at a push-pull follower and then feed a coil that I have yet to define what the inductance will be (but I believe about 55mH).
I have to excite a coil to sum up.
But as I am having difficulties in some parts, I am going in stages.
Which current?
About 50mA

I already defined what the circuit has to do, but now I am having difficulties to implement it. As I go on I post here. I believe it will be better for those who read.
 

KlausST

Super Moderator
Staff member
Joined
Apr 17, 2014
Messages
19,717
Helped
4,343
Reputation
8,695
Reaction score
4,304
Trophy points
1,393
Activity points
130,522
Hi,

I guess you mean LT1632 .... it still is an Opamp, while it should be a comparator.

Klaus
 

Dragnovith

Newbie level 5
Joined
Apr 17, 2021
Messages
8
Helped
0
Reputation
0
Reaction score
0
Trophy points
1
Activity points
70
Hello, I am designing this circuit to power the toroidal coil. But the final answer that goes through the 55mH inductor is being quite strange.
1620494686414.png

To excite the core, a square wave oscillator was built, then it goes through a dfliflop to have the frequency divided and a voltage-to-current converter (I am not getting the current to 500mA, however simple it may be.) . Finally, the circuit arrives in a push pull follower to have enough capacity to excite the coil with this current. I know that buffers are not good for much there, but it is more by default.
Output of Osscilator and DFLIFLOP
1620494749164.png

Output of push-pull follower and current across inductor
1620494844732.png

1620494862336.png


I would like to see the saturation behavior as in the image below .
1620494992747.png
 

FvM

Super Moderator
Staff member
Joined
Jan 22, 2008
Messages
48,396
Helped
14,251
Reputation
28,763
Reaction score
12,937
Trophy points
1,393
Location
Bochum, Germany
Activity points
280,075
Your circuit drives DC voltage to the coil, intentionally?

If you want to see saturation, you should use a saturated core model.
 

dick_freebird

Advanced Member level 5
Joined
Mar 4, 2008
Messages
7,285
Helped
2,127
Reputation
4,259
Reaction score
1,983
Trophy points
1,393
Location
USA
Activity points
58,436
If you want to "see" saturation then your inductor
model would have to (a) emulate it at all and (b)
have its params set for reasonableness.

Coupled inductor modeling is something that
varies a lot between simulators. You may find
vendor models but these aren't necessarily
going to work in every simulator.
 

Dragnovith

Newbie level 5
Joined
Apr 17, 2021
Messages
8
Helped
0
Reputation
0
Reaction score
0
Trophy points
1
Activity points
70
Coupled inductor modeling is something that
varies a lot between simulators. You may find
vendor models but these aren't necessarily
going to work in every simulator
If you want to see saturation, you should use a saturated core model.
So, would I have to get a tool outside of ltspice to see this? Like the quickfield simulation tool?
 

FvM

Super Moderator
Staff member
Joined
Jan 22, 2008
Messages
48,396
Helped
14,251
Reputation
28,763
Reaction score
12,937
Trophy points
1,393
Location
Bochum, Germany
Activity points
280,075
LTspice provides two saturated core models and can create different models by using behavioral descriptions, e.g. B/H tables.

FEM tools like Quickfield or FEMM can be used to derive effective permeability and B/H function for complex core geometries. For simple geometries like toroid they can be simply read from the core datasheet.
 

Easy peasy

Advanced Member level 5
Joined
Aug 15, 2015
Messages
3,043
Helped
1,116
Reputation
2,232
Reaction score
1,155
Trophy points
113
Location
Melbourne
Activity points
16,831
You really should have diodes across Q1, Q2, also R6 is neg feedback - whereas it seems you want some positive hysteresis,

unless you really want 1V high at R5 = 1V low at the o/p
 

Dragnovith

Newbie level 5
Joined
Apr 17, 2021
Messages
8
Helped
0
Reputation
0
Reaction score
0
Trophy points
1
Activity points
70
Okay, I advanced on the circuit. But now I need to make a sensing circuit for the coil fed by the circuit, would you have any suggestions on how to do this?
I am taking this work as a reference.
1620659893809.png
 

Easy peasy

Advanced Member level 5
Joined
Aug 15, 2015
Messages
3,043
Helped
1,116
Reputation
2,232
Reaction score
1,155
Trophy points
113
Location
Melbourne
Activity points
16,831
because it is a parallel LC ckt, if you load the sense coil - you will in fact pull down the natural resonant freq of the LC tank - this is covered in any good text book. Thus if the temp varies significantly the inherent natural Fo will vary due to the changing R of the wdg.
 

LaTeX Commands Quick-Menu:

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top