problem simulation a pulse delay line

Thread Starter

yef smith

Joined Aug 2, 2020
810
Hello , i was given a schematics which is supposed to be pulse delay .
my pulse is 3.3V and 220nS wide, but instead of a pulse on the outside i get a huge overshoot .
I know that LC system is a differencial equation which can lead to overshoot but its supposed to be a pulse delay.
Where did i go wrong?
LTspice file is attached.
Thanks.

1711374198002.png
 

Attachments

Papabravo

Joined Feb 24, 2006
21,264
There is a HUGE mismatch between your source impedance and your load impedance. In 2nd order systems overshoot happens because there is little to no damping.

ETA:
  1. You might want to note on the schematic that you are using real components with parasitic properties including series resistance and parallel resistance.
  2. Changing the series resistance of the source doesn't help much.
  3. AC analysis shows considerable peaking between 1 & 2 MHz.
I don't think the source impedance is the problem, but rather the peaking of the AC response between 1 & 2 MHz,
1711377648887.png
 

Attachments

Last edited:

Papabravo

Joined Feb 24, 2006
21,264
Even if I give you a 6th order Butterworth filter with ideal components and a corner frequency of 4MHz., which knocks down the peaking, there are still problems.
1711380830454.png
At least the overshoot is of a smaller magnitude. For ANY appreciable source impedance, the input pulse becomes wildly distorted from the multiple reflections going back and forth.
1711381224416.png
 

Attachments

Thread Starter

yef smith

Joined Aug 2, 2020
810
Hello , first I am confused regarding the source at post 4, how do I properly represent my 33220A signal generator as a source in the simulation ?
 

Thread Starter

yef smith

Joined Aug 2, 2020
810
What is the theory behind doing this pulse delay?
I see that if I put a square pulse threw LC then it will be ruined . What is the logic of keeping the shape and controlling the delay?
I need a 300ns delay .
Thanks .
 

Papabravo

Joined Feb 24, 2006
21,264
Hello , first I am confused regarding the source at post 4, how do I properly represent my 33220A signal generator as a source in the simulation ?
For starters you can represent it as a voltage source with some internal resistance. As a general-purpose signal generator, it might have an output impedance of 50Ω in which case you could use that as the internal resistance of the voltage source.
 

Papabravo

Joined Feb 24, 2006
21,264
What is the theory behind doing this pulse delay?
I see that if I put a square pulse threw LC then it will be ruined . What is the logic of keeping the shape and controlling the delay?
I need a 300ns delay .
Thanks .
Any pulse that you put through anything that looks like a low-pass filter is going to affect the shape of the pulse. Why did you think your original circuit was going to pass the pulse without changing the shape? Seems like you should know better.
 

Thread Starter

yef smith

Joined Aug 2, 2020
810
Yes of course , it will be filtered .
what is the theory behind this type of structure so I will know what delay I would have and the shape will be not ruined as possible ?
Thanks .
 

Thread Starter

yef smith

Joined Aug 2, 2020
810
The important thing to me is the basic theory.
I know how to design chabyshev filters in the frequency domain but I have three terms
1.phase delay
2.group delay
3.time delay

I want know how mathematically given the AC transfer function can we get the time delay the pulse will go threw .
Is there some example I could se the logic of the link between them ?
Thanks .
 

Papabravo

Joined Feb 24, 2006
21,264
The type of structure in your original post is a passive lowpass filter with 3 LC sections. You can design such a filter with the capacitor as the first component – as you did, or you can put the inductor first, but the L & C values will be different. The characteristics of various filter types can be tabulated, but I'm not familiar with one that does a pure time delay without affecting the pulse shape.

Consider that your pulse has rise and fall times of 1 nanosecond. Using the standard approximation of

\( BW\;=\;0.35\cdot t_r\;=\cfrac{0.35}{1 \times 10^{-9}}\;=\;350\text{ MHz.} \)

Anything you do with a lower corner frequency is going to distort the pulse.

You might want to consider using a transmission line to achieve the desired delay. I don't know if you have available a practical method of using a transmission line.
 
Last edited:

Papabravo

Joined Feb 24, 2006
21,264
Hello , the key if you could show me the link between transmutation line response and the time delay I get ?
Thanks .
You select a candidate for a transmission line and you get from the datasheet the velocity of propagation. You terminate it properly, send a pulse down the line and see how long it takes. As a rule of thumb, you can start with an estimate of 0.7c, figure out the length and see what happens. The rule of thumb estimate is 1 ft./nanosecond. A better estimate might be:

\( 0.7c\;=\;0.7(299,792,458\text{ m/s})\;=\;209,854,720\text{ m/s} \)

\( 209,854,720\text{ m/s}\times 300\text{ ns.}\;\approx\;62.956\text{ m}\;\approx\;206.55\text{ ft} \)

A commonly available coaxial cable is RG58/U which has the following properties:

The RG58/U cable exhibits capacitance of approximately 28.8 pF/ft (94.73 pF/m), signal attenuation of around 11.7 dB/100 ft at 400 MHz (signal attenuation of the cable depending on the frequency) and has a velocity of propagation of 66%
ETA: Using our estimate of 63 meters of cable we note the following:

\( C_{TOTAL}\;=\;94.73\text{ pf/m}\times 63\text{meters}\;\approx\;5.9\text{ nF} \)
\( L_{TOTAL}\;=\;Z^2C_{TOTAL}\;=\;50^2(5.9\text{ nF})\;\approx\;14.76\text{ µH} \)
\( \tau_{d}\;=\;\sqrt{L_{TOTAL}C_{TOTAL}}\;=\;\sqrt{14.76\text{µH}\times 5.9\text{ nF}}\;\approx\;295\text{ ns} \)
 
Last edited:

Thread Starter

yef smith

Joined Aug 2, 2020
810
Hello Papabravo,based on transmission line theory i have the formula for phase velocity.
In transmission line the phase velocity is by L and C of per length.
But in my model of lumped elements how do i know what is the total L and total C?
Thanks.

1711604722437.png
1711603304552.png
1711603329866.png

1711603238194.png
 

Papabravo

Joined Feb 24, 2006
21,264
Using capacitance per unit length times some length and characteristic impedance to approximate the total inductance of the proposed length. Using those numbers you approximate the expected delay. This would be for an ideal lossless transmission line. You build it, measure it, and adjust it because ideal lossless transmission lines do not exist. Furthermore I'm not sure it is worthwhile to try for a more accurate estimation, but you are welcome to make the attempt.
 

Thread Starter

yef smith

Joined Aug 2, 2020
810
Hello Papabrabo,How did you design the BW of the filter?
Each section doesnt have the load impedance 2000Ohm.
it will create discontinuety.
How did you reccomend to design the filter so it will match the load?
currently i dont see each section having 2K characteristic impedance.
Thanks

1711828915659.png
1711828800283.png
 

Papabravo

Joined Feb 24, 2006
21,264
The standard Butterworth technique is to start with prototype low pass filter normalized for 1 rad/sec. You get the starting values for the L & C components and then you frequency scale them and adjust for the source and output impedance. I've never heard of have resistive loads between the sections.

For the 6th order with RS and RL = 1Ω
C1 = 0.517638
L1 = 1.4142136
C2 = 1.9318516
L2 = 1.9318516
C3 = 1.4142136
L3 = 0.517638

There are also online calculators that will do the legwork for you like this one:
Butterworth Pi LC Low Pass Filter Calculator (calculatoredge.com)

1711832716586.png
 
Top