MATLAB simulation of pulse forming networking using VINPFN

Thread Starter

frustratedgrape20

Joined Mar 3, 2020
19
Hi, I am trying to use a set of open source scripts called VINPFN to simulate a type 'B' pulse forming network. An enhanced dialog input box is concurrently required to input various parameters of the network. The scripts are available on mathworks.com and the links for them are listed below:

· download source for VINPFN: www.mathworks.com/matlabcentral/fileexchange/41738-vinpfn?
· download source for enhanced dialog input box: www.mathworks.com/matlabcentral/fileexchange/25862-inputsdlg-enhanced-input-dialog-box?s_tid=FX_rc1_behav

I have taken the liberty of combining the contents of both folders into a single folder in the attachment.

The user manual for VINPFN states that the command 'vinpfn' can be launched without any input arguments. However, upon launching the program, the following error messages were encountered:vinpfn error screenshot (1).jpgvinpfn error screenshot (2).jpg

I wasn't sure if the syntax was correct, but examples posted online seem to suggest so. I have also tried adding semicolons but they only added to the list of errors. Could anyone please show me what went wrong with the scripts?

Pardon me for my ignorance and thank you for your patience; this my 1ˢᵗ time using this program.
 

Attachments

WendellB

Joined Feb 14, 2020
22
Hi Frustratedgrape20

I do not use matlab so I cannot help you with that particular problem.
However, I am curious why you are trying to simulate a PFN and why you choose a type B topology?
Reason: I started my engineering career in the 50s design high voltage pulse capacitors and PFNs for pulsed radar systems. The type E PFN was what finally evolved from the work done at MIT. For more information you can find on line a free copy of a book entitled PULSE GENERATORS which is part of a series of 29 volumes called the MIT radiation laboratory series, published by MIT, This particular book is a design manual showing the development of pulsing methods, all methods, developed as a result of the work of Scientists at MIT during world war two.

You could use LTspice to set up and run a circuit showing a PFN pulsing a load. And there are other ways to set up a simulation of a PFN operating. If you want to continue this conversation then leave a message for me. Good luck.

Best regards

Wendell
 

Thread Starter

frustratedgrape20

Joined Mar 3, 2020
19
Hi Wendell,

The ultimate goal is to build a type 'E' PFN that matches a relatively high impedance LC network to a low impedance series RL load. Matching will be achieved using a 'coaxial cable' type pulse transformer as shown below:
pulse transformer ltspice1.jpg

The output of this pulse transformer is a single turn winding with an impedance ('Rs', 'Ls' in schematic) much lower than the load ('R', 'L' in the schematic) I intend to drive, i.e. Rs ≪ R and Ls ≪ L

In theory, if the characteristic impedance of the ladder network is matched to the load impedance, then an approximately rectangular current pulse should be observed through the load, like the one below:
ideal case ltspice2.jpg

Various research papers that I've downloaded on that subject mentioned the use of a user coded script called VINPFN that only contains scripts for 3 topologies - A, B & C. Since 'E' is type 'B' with mutual coupling between adjacent pulse forming inductors, I decided to give it a go. But I digress.

Anyway, I have used LTspice to simulate the required topology, and below is an image of the circuit, along with 2 schematics attached - 1 showing a simulation with ideal components and the other, with real components.updated circuit ltspice3.jpg

The circuit and the components were designed around the following criteria:
◊ mesh capacitance of 3 mF
◊ pulse width = 1.6 ms
◊ primary output current = 12.2 kA

A 7:2 step down pulse transformer was used and in theory, the current output into the R-L load should be in the ball park of 40 kA.

The inductor on the last stage of the PFN was used as the pulse transformer's primary winding, and the simulation yielded the following results:
♤ discharge time ≪ 1.6 ms (as required)
♤ discharge curve on the primary looked like an inductive spike
♤ maximum primary current was only 600 A
♤ maximum secondary current of ≪ 50 A

The component parasitics for each mesh's inductance and capacitance are included in 1 of the schematics attached.

Lastly, your work in PFNs and pulsed radar systems sounds interesting. Have you by any chance, happened to design capacitors with a high specific energy (> 2 J / cc)?
 

Attachments

Last edited:

WendellB

Joined Feb 14, 2020
22
Hi Frustratedgrape20,

In answer to your question about high energy storage caps. I know what you mean but have not designed any. Usually very high energy is accomplished by voltage stresssing the caps way above normal rating for usually they have to run for a very short time Material like Kapton and reconstituted mica (Mica wih a binder) can be stressed very high both in voltage stress and heat stress.

My experience was designing PFN's and their capacitors and we stressed them at about 500 volts per mil of insulation. Most DC caps in the same time frame were stressed at 1000 vdc per mil. Some even at 1200 dc volts per mil. but for pulse work we used a stress of 500v/mil and would vary it depending on the actual life that we would guarantee.

looking at your LTspice circuits I cannot really figure out what your goals are yet. your connecting to the end of a transmission line with a transformer winding. That alone would prevent the build up of voltage (360vdc) on the PFN capacitors.

I have attached two LTspice circuits. (1) Shows a conventional way of forming a pulse using a PFN which is to simply apply a DC source voltage to the line at as slow rate. When the caps are all charged up then you short the input coil of the PFN to ground. With the bottom side of all the capacitors (one node) connected to the load current flows down the transmission line and through the load starting at time =0 . When the signal reaches the far end of the transmission line it returns in the opposite polarity and when it reaches the beginning coil of the PFN it stops the existing current from flowing. So if the switch is a Thyratron tube that tubes current ceases and the pulse is terminated.

Another PFN circuit is attached and shows another way to generate the EXACT same pulse. You simply place the load resistor in series with an uncharged PFN meaning the capacitors are not charged up. Then apply a voltage to the PFN with the load connected to the lead common to all the capacitors. The will produce a pulse across the load which is exactly the same as you see when you discharge conventionally using a charged PFN.

I designed to a pulse width of 1000us and a load impedance of 1 ohm to connect to the values easier.

Also the effect of a real inductance figure should a pulse transformer be used to couple to a load.

hope this helps.

Best regards, Wendell
 

Attachments

Thread Starter

frustratedgrape20

Joined Mar 3, 2020
19
Hi Wendell,

Regarding energy dense capacitors, what did you mean by voltage stressing them? Based on what I gathered from the internet, it seems that you might be referring to the application of a very high voltage across the film (close to its dielectric breakdown). But I don't understand how this would increase the voltage rating of said capacitor. Could you explain to me how that would work?

Thanks for the simulation files. I have tried with my own circuit as well and while I could obtain a nice flat top pulse for any value of mesh capacitance, complications arise when component parasitics e.g. ESR and ESL are factored in.

My goal is to deliver the energy of all 20 capacitors (≈3.7 kJ) into a RL load of average ESR of 2.35 mΩ and average ESL of 1.75 µH within 1.0 ms, and preferably with a flat top current. In this endeavor, component parasitics have to be factored in and that's where the challenge lies. The pulse transformer seen in the previous circuit was meant to match the characteristic impedance + capacitor bank ESR to the (much smaller) ESR of the load.

I have attached a copy of:
(1) my circuit;

(2) the conventional PFN discharge circuit you designed without parasitics for which I used my own capacitance (3 mF);
↑ ↑ ↑ ↑ ↑ ↑ ↑ ↑ ↑
(3) the schematic directly above but with parasitics

While the effects of parasitics are inescapable, do you think they will impact the discharge curve as significantly as simulation files (2) and (3) suggest? Oh, and I have added in a spice directive in all simulation files that initializes the parameters of the components (including parasitic quantities) to simplify data entry.

Thank you again for looking through the files.
 

Attachments

Last edited:

WendellB

Joined Feb 14, 2020
22
Hi Frustratedgrape20,

First I will answer your first question. The physical size of a wound capacitor, the kind you would use in your PFN, is inversely proportional the the stress you subject the dielectric material to. By stress we mean the volts per mil of dielectric thickness that you apply to the insulating mater between the capacitor plates of the capacitor winding. If you stress higher, then the amount of dielectric material becomes less and the capacitor will be smaller.

As for your project. I have included real parasits, as you call them. For capacitors they are actually specifications the vendor guarantees. For coils, yes the resistance has to be calculated and for this case it has to be the the resistance due to skin and proximity effect for a wound coil.

Running the attached program you will see that I have used ESR and ESL figures for the caps that are real specifications. For the coil you would have to design it to meet the ESR shown, it it is raised to a higher value then that shown, yes, the pulse shape will
begin to droop during the pulse output and of course the coil loss will increase. On the LTspice schematic I voiced my opinion that
I think the coil value along with the ESR value of the coil is difficult if not impossible to meet in practice due to the extremely low
PFN impedance. Raising that impedance at some point would make the design far more realizable and the capacitors would be much smaller and cheaper.

Best regards

Wendell
 

Attachments

WendellB

Joined Feb 14, 2020
22
1583687956264.png

Hi Frustratedgrape20

Above is a T model of a the tapped solenoidal coil to the right. Also included is the equation for calculating the inductance of any solenoid provided the length is greater than the diameter. it is Wheelers formula modified to use coil diameter and length.

Looking at the T circuit, it is the exact equivalent of the solenoid to the right which is two coupled coils, However the model has three coils all uncoupled. But notice that the inductor drawn vertically has a negative value equal to the inductance LM times the coefficient of coupling which is usually 0.15 for an E type PFN. Mutual inductance LM is simply the square root of the quantity L1 TIMES L2. Since it is a negative value it can and does buck the positive inductive value of inductance created by the lead inuctance in series with the capacitor connected to that tap and the capacitors ESL value. In fact. If you had a noticably large capacitor ESL you could design the solenoid making the coefficient of coupling quite high to buck the capacitors ESL. This means that the dimension D becomes larger.

Best regards

Wendell
 

Thread Starter

frustratedgrape20

Joined Mar 3, 2020
19
Hi Wendell,

Thanks for the diagram and for the latest simulation file. The thing about this PFN is that it will be used to drive a railgun. The electrical model of the railgun load is a varying resistance and inductance, and for now it is assumed that both quantities are constant. The maximum resistance and inductance of the load is 4.7 mΩ and 2.43 µH. Therefore, I am trying to design the PFN such that the source impedance (characteristic + lumped ESR) = railgun load resistance (4.7mΩ only, inductance ignored)

As for the coils, I will be winding them using a 2mm (12 AWG) magnet wires, and I used Wheeler's formula for short inductors to calculate the required inductance. If the inductances are far apart, then proximity effects can be neglected (I think). Also, I calculated the electrical specific action to melt for each mesh inductor (less than 6 kA for 1 ms based on the latest simulation file) and temperature rise seems to be acceptably small.

How would you suggest matching a PFN source impedance of 13 mΩ to a railgun load of 4.7 mΩ?

As we speak, I am currently recalculating mesh inductance using Wheeler's formula to get a better approximation:

asdfasdf.jpg

source: www.qsl.net/zl1an/Downloads/Inductance_Problem.pdf
 
Last edited:

Thread Starter

frustratedgrape20

Joined Mar 3, 2020
19
Wendell,

As of now, I have in mind the following methods for matching impedances:

1. using a pulse transformer (primary & secondary are wound in a similar manner as a coaxial cable's construction to maximize coupling)
2. using a sufficiently large & short coaxial cable (negates the effect of inductance in pulse transformers)
3. adopting a type 'C' PFN design to reduce source's ESR (paralleled LC meshes), but angling the inductors such that they are mutually coupled
 

WendellB

Joined Feb 14, 2020
22
Hi

Your formula is obviously more accurate, so use it. As for matching the PFN to the load. Then design or purchase a pulse transformer that can handle the peak and average power and with enough primary inductance to prevent too much pulse top voltage droop. If you really want to design very accurate air core inductances then purchase the book. called:
"INDUCTANCE CALCULATIONS" by Frederick W. Grover. This book is the upgraded and corrected book that was originally
published by the American Bureau of Standards I am not sure but then it was call Circular 555 or something like that.

In any event If you design air core coils then you must have this publication. The formula accuracy will astound you. It also focuses on mutual inductance calculations as well.

Another great book was written by Dr. Michoel P. Perry. called "LOW FREQUENCY ELECTROMAGNETIC DESIGN" and it addresses
all aspects of air coil inductors. not just their inductance but skin and proximity losses as well. He worked at GE and for them he designed huge inductors like 6 feet long and 4 feet in diameter for voice communication circuits on high voltage power lines. He work is excellent.

Best regards

Wendell
 
Top