Continue to Site

Welcome to our site!

Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.

  • Welcome to our site! Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.

Help to get lowest parasitic inductance/capacitance

Status
Not open for further replies.

Futterama

Member
Hi forum,

I'm building an isolated DC/DC converter using the LT3999 push-pull driver and a Würth 749196301 SMPS transformer:
https://www.linear.com/product/LT3999
https://katalog.we-online.de/pbs/datasheet/749196301.pdf

I would like to connect the IC and transformer with lowest possible parasitic inductance/capacitance, but I need some advise for this.

Look at the attached drawing. The LT3999 is alternately switching the two pins to GND. The transformer is built as the red symbols indicate. The pink lines are the necessary connections between pins. The direct connection between two transformer pins is connected to the positive input supply.

So how should the PCB traces be routed to minimise parasitic inductance/capacitance? I have 2 PCB layers at my disposal. I'm thinking the currents should run is opposite directions on each side of the PCB to minimise inductance, but I just can't wrap my head around this.

Thanks.

Best regards,
Martin
 

Attachments

  • drawing.jpg
    drawing.jpg
    53.3 KB · Views: 192
To minimize capacitance use as short traces as possible. (For critical requirements you can remove any ground or power planes beneath the traces, but that shouldn't be required here).

To minimize inductance use a wide trace. You can also run the two traces to the transformer over the Vin trace (or Vin power plane) to further minimize inductance.
 
crutschow, thanks for your reply.

Ok, use wide traces, got it. Regarding running the two traces from LT3999 to transformer, does is matter where the current is flowing from and to? I mean, if the supply voltage was connected to a Vin power plane, does it matter if it is connected to the right of the transformer, so current will flow towards the LT3999, or if it is connected near the LT3999, so current is flowing away from the LT3999 towards the transformer?
 
Ok, use wide traces, got it. Regarding running the two traces from LT3999 to transformer, does is matter where the current is flowing from and to? I mean, if the supply voltage was connected to a Vin power plane, does it matter if it is connected to the right of the transformer, so current will flow towards the LT3999, or if it is connected near the LT3999, so current is flowing away from the LT3999 towards the transformer?
Not sure I understand your question. :confused: What to you mean "towards" or "away". The current direction is determined by the polarity not location.
But normally, current direction should not make a difference.
 
I'm just thinking of the path the electrons will travel. In order to have low inductance, they will have to pass close in their path one way and the other. Imagine a battery connected to a load with a long cable. If the wires in the cable, are close together, the inductance is low, if the wires in the cable are further apart, the inductance is higher. This is due to the electrons travel from battery to load in one wire, and from load to battery in the other wire, creating opposite electric fields along their paths. So what I have to make sure, is that the electrons will travel in each direction, in 2 different conductors, placed close together. Right?

Well, maybe this all happens automatically with a power plane since the current will take the path with least inductance, according to a paper I read once.
 
Yes, a power plane just acts like a very wide conductor.
The current will follow the lowest resistance/inductance path from one point to the other.
The magnetic field from the current in a trace above the plane will tend to focus the plane return current to be underneath the trace so as to minimize trace inductance.
 
Low inductance is achieved by having a small enclosed area of the signal path, signal out and return. You keep things short or together because L is proportional to enclosed area. But keeping things together increases capacitive coupling between the two traces, think of two capacitor plates, the closer they are together the greater the capacitance. So what tends to reduce inductance tends to increase capacitance except for shortness, which reduces both.
 
I'm just thinking of the path the electrons will travel. In order to have low inductance, they will have to pass close in their path one way and the other. Imagine a battery connected to a load with a long cable. If the wires in the cable, are close together, the inductance is low, if the wires in the cable are further apart, the inductance is higher. This is due to the electrons travel from battery to load in one wire, and from load to battery in the other wire, creating opposite electric fields along their paths. So what I have to make sure, is that the electrons will travel in each direction, in 2 different conductors, placed close together. Right?

Well, maybe this all happens automatically with a power plane since the current will take the path with least inductance, according to a paper I read once.

Hi,

Inductance increases with length, ie inductors in series add.
Current takes the path of least resistance, and for short time periods takes the path of least inductance. Over longer time periods inductance doesnt matter only the resistance.
Wires in parallel with the total current split equally between them all reduces skin effect which reduces AC resistance. For circuit traces this might not be as bad as with thick wires.
 
Thank you all, I will move the IC as close to the transformer terminals as possible and use much wider traces than I did previously and make sure there is a power plane return path below the traces.

I can get the IC almost in under the transformer or I can move the transformer to the other side of the board, I'll see what works best. Luckily I can make double sided PCB at home so prototyping is fast and cheap, even though the LT3999 is very small in 3x3mm DFN-10 package and it takes patience to solder by hand without soldermask ;)
 
I just want to follow up. I moved the IC closer to the transformer and used much wider traces and also made them more symmetrical to each other. The inductance dropped from 140nH to 80nH which I think is pretty good and I'm totally happy with it.

Thanks guys!
 
Status
Not open for further replies.

Latest threads

New Articles From Microcontroller Tips

Back
Top