LM2575 switching regulator - ideal inductor and COUT sizes

Community PCB Design
1

Hi all,

I’m developing a PCB in Cadsoft Eagle as seen in the brd and sch files as per the links below:

Eagle schematic file: https://sites.google.com/site/bgedsadat … ects=0&d=1

Eagle board file: https://sites.google.com/site/bgedsadat … ects=0&d=1

See the following links for screenshots of the schematic and the boards respectively:

Schematic screenshot:

Board screenshot:

My issue is with feedback I received from my board house regarding the sizes of my inductor and Cout being too small in relation to the switching frequency of my LM2575 switching regulator which as per page 7 of the datasheet is 52 kHz.

For the switching regulator subcircuit design I carefully utilised the design procedure as per pages 13 to 18 of the LM2575 datasheet.

Based on the provided design guidance within this pages the stand out selection factors in relation to picking an inductor are:

The inductor is rated for operation with a current rating (Irating) of 1.15 x Iload whereby I load in my case is 0.4A hence Irating equals 0.46A.
The inductor is rated to operate with the LM2575 switching frequency of 52kHz.

The pages also provide inductor part numbers from three different manufacturers. Selection of the part number is based on the inductor value which in turn is based on the desired LM2575 Vout, maximum input voltage into the LM2575 and Iload. In my case my desired LM2575 Vout is 5V, my maximum input voltage is +24V and my Iload is 0.4A hence the inductor value as per the figure 28 on the LM2575 datasheet is 680uH which as per table 2 on page 16 of the LM2575 datasheet means the following inductors can be used: 67127050 from Schott, PE-52629 from Pulse Eng and RL1950 from Renco.

1st question: What exactly is wrong with the size of my current inductor selection as per my .sch and .brd files or atatched screenshots? I’m using an inductor of package 0805 as per the eagle package.
2nd question: Does anyone have any idea where I can find the Cadsoft Eagle library files for any of the three inductors? I feel one of these three should be of the right size in relation to the feedback from my boardhouse.

As for the selection of Cout, the design guidance within pages 13 - 18 doesn’t mention anything regarding the size of the Cout capcaitor to be used. In my design as per my attachments, I’m utilising a standard 0805 capacitor which I have used all across my schematic.

3rd question: Any idea which Cout capacitor size I should be selecting?

Note: I would like to stick to using the LM2575 as I’ve gone quite far with integrating it within my design plus the availability of its Cadsoft Eagle library file.

I appreciate any assistance.

Regards,

TokTok.

2

The attached zip file contains a library that has the Pulse Electronics inductor part. I created this component from the datasheet which I found by searching for the part on the Digi-Key website (http://www.digikey.com). The datasheet has a clear drawing for the layout (land pattern) for the inductor. Actually it has two. I chose the low profile version. Make sure you choose low profile when you purchase your parts.

Generally you should check all components before submitting your design to fab. The best way to do this is to have samples of every component and place them on an actual-size printout of the PCB. If it’s not possible to have all components to hand, you should at least look up and very carefully check each land pattern against the layout. I did not check this component “very carefully”. I created it in about 5 min. I’m leaving it to you to check it. It’s a simple component and I have a bit of experience so it’s probably ok. Caveat emptor.

Similarly, the 330uF capacitor is not likely to be available in a 0805 package. You need to find an appropriate part, look at the datasheet for the package and use that package in your PCB.

Good luck with your project.

  • Chip
3

I just took a quick glance at your board, and see a few issues:

  • Verify your power jack doesn’t have a step on the bottom. If it does, you may need to move it closer to the left edge

  • The holes for the jack seem rather small

  • Power and ground traces should be short and wide, or use a ground pour to reduce impedance. I would use a top-side pour with cutouts for the radio here

  • Traces are run within the keepouts of the mounting holes. They may contact a screw head or be damaged by mounting posts

  • 24V input is short-circuited by the trace that runs from the power connector, through the tab of IC2, to IC1. Note that the tab of IC2 is connected internally to pin 2, so it is grounded

  • Some backside traces are very close to each other; make sure you are not violating the minimum spacing of your board house

  • Likewise, verify the minimum spacing between vias and pads

  • Look at the data sheet for IC1 and follow their recommended layout and copper pours. Switchers can be tricky to lay out correctly

  • Should the LEDs be closer to the right edge of the board? Should they line up? You may want to rotate them 90 degrees if you will bend them over and have them poke out the right side wall

  • You have traces under the antenna end of the radio module. Is that allowed? Are there any keepouts specified?

  • Ember Zigbee chips can draw large slugs of current when they wake up. I’d add some bulk capacitance near the radio (I use 100uF and 1mH on my latest design)

  • Bypass capacitors MUST be located right next to the Vcc pin they are bypassing. Best layout is trace → cap → pin

  • The schematic is missing part types for IC2 and IC3

  • There are vias under the metal bracket for X1. These will short out to the connector

  • Traditionally, connector reference designators start with P or J, not X. Crystals and resonators start with X, not Q (which is used for transistors)

  • Traces should connect to pads straight on, not forming acute angles, which can form acid traps. For the SOIC, I’d run the trace straight out the short end. There’s not enough space to come out the side

/mike

4

I also would recommend using File>Export>Image to take images of your design. Use the DPI setting to get a high resolution image so we can see details.

5

Hi all,

Thanks for the replies especially n1st. Having read the replies this I’ve made some changes:

I’ve re-positioned some components as I wanted to ensure traces connect to pads straight on/symmetrically, not forming acute angles. I understand this can cause an acid trap problem.

I’ve eliminated the top ground plane leaving the bottom ground plane which I have brought inward with a margin of around 60mil.

I tried keeping the ground plane free of traces.

I’ve done my best to run the traces outside the keepouts of the mounting holes.

I’ve ensured I’ve adhered to the minimum spacing between traces as there were some backside traces which were too close.

With regards to component placement, I reviewed once more the recommended layout for the switching regulator and 3.3V regulator sub-circuits.

I’ve lined up the LEDs closer to the right edge of the board.

Removed traces under the zigbee module especially the antenna end.

Relocating the decoupling capacitors closer to the Vcc pins.

Removing vias under the metal bracket of the 15 pin connector.

I’ve attached my files and had a look at the gerbers using using Viewmate which has been quite enlightening. Do you reckon I’ve still got any return path issues? As per my board house I had some.

Regards,

Alex.

6

I went over the schematic and board, and made some changes. On the board, I moved the voltage regulators a bit, and a few caps, but let everything else alone. I didn’t re-do the crystal layout, nor the placement for the LEDs. I didn’t want to put too much time into improving the board. However, I put copper planes on both sides, which are connected to ground. I’ve included plenty of ground vias, as well. There is a 40-mil space between copper and the edge of the board. If you need more room, you may have to move some parts.

After reading the ETRX357HR datasheet, I removed copper from the left side of the part. Look at tRestrict and bRestrict to see what I’ve done. BTW, There may be a problem with the upper right screw head touching the 15-pin connector, but I left those alone. To see if parts fit well, without any interference (especially around holes), print the board actual size and place the parts on the printout.