pretty new to the KiCad club, so please be gentle with me.
I am trying to design my own Buck Converter with a lmr50410.
After a fairly long day I managed to calculate all the values for the components and place them in the schematic as the datasheet recommends it.
Now I would like to start the PCB layout, and for obvious reasons there can’t be all the components in the world listed in a single library.
This means I managed to create the symbol for the lmr50410 and add an existing footprint (SOT23-6).
But now I need that for the inductor too, but I struggle to recreate the L symbol and add the footprint, which is 06024 (from the schematic).
The Inductor I want to use is (found on JLCPCB):
MHCI06024-150M-R8A
You will find the inductor “L” symbol you require in the “Device” library alphabetically listed under “L”. You just need to change the generic value to the required value.
For the footprint you desire, make one from scratch, or, as @tom3f suggests, modify an existing footprint.
As you are new, I’d suggest modifying as all the layers are already present, so all you need to do is a bit of pushing stuff around.
This one looks like a likely candidate:
I’m assuming you have already created a Personal Footprint Library, if not, read here.
To copy that part to your personal library:
Open your Kicad footprint editor, scroll through the items 'till you find that footprint, and right click it.
Select “save as”, give it the new name you require, scroll through the library list 'till you find your personal footprint library, highlight that and save.
Close that footprint editor, open your personal library, reopen the footprint editor, select your newly named footprint and now you are ready to modify.
To modify, double click the pads and change the dimensions to those of the data sheet. Move the pads so they are the correct distance apart (you will probably need to use a fine grid for this), then move and/or drag the lines on the other layers to suit the data sheet. Finally save.
You now have your required footprint so you can associate it with your symbol.
From your post, it is not clear to me whether you have any experience with pcb layout of electronic circuits. Let me caution you that proper pcb layout is the “secret sauce” behind many types of electronic circuits, particularly including switching regulators. The datasheet for the LMR50410 does include layout information but IMO it is not so clear because it does not show realistic footprints for the passive components:
I would like to recommend that if you complete a preliminary layout, post a clear image of it on this forum and get some feedback (from me or others here with the right experience) to improve the chances of having a good design.
@jmk I am going to follow your guide as soon as I come home
@BobZ At school I had electronics as a subject, so I have a basic understanding of it. But we never made any PCB’s, so the whole Software and layout thing is new to me.
As soon as I have a layout, can I post it directly here or do I need to create a new post to let it review?
That all depends on how long it takes to lay up a board.
Don’t rush and make mistakes. Take the time to explore the software. @BobZ offers good advice, he knows stuff.
It was there when I posted. No idea why the poster removed his own comments.
@jmk
So, I started the process as you described it.
I came to the conclusion that the pad Size and the spacing between, would already be what I need.
Although I am not so sure about it, to prove that I just added C to B, so I would get the whole length from the left side of the left pad, to the right side of the right pad. And that distance corresponds to the KiCad footprint.
Thank you for the “vote of confidence”. I can remember one experience many years ago when pcbs were all expensive and slow to get. Handwiring breadboards was relatively common. I was looking at the output of something like a high frequency boost switching converter, and I had an output interconnection which was 10-15 mm of wire. (about a half inch.) The dI/dt (rate of change of current) in that wire was sufficient so that the oscilloscope displayed about 9 volts difference in spike voltage amplitude according to where the oscilloscope probe touched that length of wire. That can make a big difference in the operation of a circuit. I intend this as evidence (particularly for any newbies) that proper pcb layout is essential in switching voltage converters, as well as many other circuits.
Okay guys, so this is my attempt on a Buck Converter circuit.
Since I am a new user and I can not upload files as pdf, here is one png.
If I did not give enough informations about settings and so on, please let me know.
To get to this point, I followed the youtube Tutorial from “Phil’s Lab” (can’t post the link, still a new user…).
IMHO, that layout is OK, not great.
I would rotate both R1 and R2 90°, and put the VFB pads right next to the VFB pin of the IC.
Beef up the ground connection a lot (it acts as a heat spreader for the IC), and rotate C4 90°, connecting the ground pad on that large ground area. The SW trace should also be enlarged.
Basically, you want as much copper area connecting the IC as you can get away with.
To beef up is an English idiom meaning make stronger, increase capacity, and so forth. A beefy person is big or muscular. 3Dogs is saying make the traces fatter.
Assuming you keep the layout the same, I’d add a ground fill in the empty area below L1 and in the area your ground trace currently goes, make it as think as possible and cover all the area under your IC that’s not covered by anything else. Then you might want to add more vias in the area south of L1 for a better connection to the gnd fills on the other layer(s).
Better. However I’m wondering why you haven’t added a GND fill on the front layer, too. For example why not enlarge the GND fill below C1/C2 so that it includes the GND pad of J1? Or even fill the whole board (with a lower priority than your other fills)? Or do you plan to add other things there?
