Differences in through-hole and smd from KiCAD perspective

[nick]

I am designing an arduino shield in KiCAD.
This is my first KiCAD project and my first pcb designing project in general.

I bought some nice through-hole resistors and capacitors, under the logic that they will be easier to solder them.

Then i thought about the actual layout of the board, and on the bottom side i will be having a GND layer, and in the upper side i will be having a Vcc layer.

But then i thought that the through hole components are soldered on the back side.

So how does this change things?

Do i reverse the layers so that the bottom layer is Vcc and the upper layer is GND?

How does through hole components change the actual layout of the pcb and the designing process?

[paulvdh]

First:
If you want to make an “arduino shield” project, then start with one of the templates:
KiCad project manager / File / New / Project from Template

This gets you the PCB outline, connector layout and more, depending on what template you choose.

@nick

I bought some nice through-hole resistors and capacitors, under the logic that they will be easier to solder them.

I do not like THT resistors much. You have to bend the leads, put those finicky leads though the holes (Yuck if you have to drill all those holes yourself) Then cut the leads. Fold the ends a bit, or devise some other method to prevent the resistors from falling out when you turn the PCB.
On top of that, al that turning of the PCB costs a lot of time (also because components do fall out sometimes) and you have to work with the mirror image half the time, which is especially a nuisance with Matrix board.

THT resistors are handy for quick prototypes on breadboards though. (Make sure to cut of ends with the gooey glue. Do not pull the resistors out of the paper strips. You do not want that goo in your breadboard !)

With SMT resistors you just need some decent tools (Temperature regulated Iron, extra flux, good quality tweezers). Then put some solder on all the “left” pads of each component, add a bit of extra flux (not needed if you solder fast so the flux does not all evaporate). Then use the tweezers to hold a resistor in one hand, place it on the PCB and reheat the solder on the PCB. After that you can solder the other side. Some holder that prevents the PCB from moving too easily also helps. 0805 size resistors are easy to solder without magnification equipment for most people. 0603 is still doable for about half the people, and for smaller you very likely want a stereo microscope.

---

All that said, back to you project.
Using one layer as a GND plane and another layer for a Vcc plane is often not the best way for relatively “simple” circuits. 4 layer boards are easy, there you just use a GND and a Vcc layer and two extra layers for the signals, but for hobby level double sided boards the goal is to put as many tracks as possible on one side, so the other side has a continuous GND plane. That does not leave much room for a Vcc plane on the other side, because that side is cut to pieces by all the tracks.

Instead use some via stitching to mostly close the gaps in the GND plane you had to make, and distribute Vcc with some relatively thick tracks. For example 1.5mm wide. The layout of the decoupling capacitors is more important then the routing of the Vcc plane.

In short:

• GND plane is the voltage reference for all signals thought the PCB. It must be good.
• Decoupling caps are the (short term) power supply for each IC. They must be placed close to the power pins, and connected to the GND plane too.
• Vcc is just to deliver some bulk power to the decoupling caps at fairly low end of the frequency spectrum, and is therefore not so critical.
• For good practice add a relatively big buffer cap on Vcc. Somewhere between 10uF and 100uF. in addition to the 100nF decoupling caps.

This is good enough for simple microcontroller boards. When you get to more complex designs it gets a lot more complicated. If you want to have fun, then have a look at the “Olinuxino A64” from Olimex. The project is on github as a complete KiCad project.

@nick

But then i thought that the through hole components are soldered on the back side.
So how does this change things?
Do i reverse the layers so that the bottom layer is Vcc and the upper layer is GND?

It’s completely arbitrary. Do whatever you like. It is most common though to put the THT components on the Front layer.

@nick

How does through hole components change the actual layout of the pcb and the designing process?

I believe you are overthinking this. Earlier you wrote this is your first PCB. Use your first design to get to know the software, and then use your knowledge of the software and what you’ve learned about general PCB layout to make your next design better. Learn by doing. Not by thinking about what you might do.

[dchisholm]

@nick

I bought some nice through-hole resistors and capacitors, under the logic that they will be easier to solder them.

There’s no way to resolve matters of taste, but I agree with you, Nick.

@nick

But then i thought that the through hole components are soldered on the back side.

So how does this change things?

Do i reverse the layers so that the bottom layer is Vcc and the upper layer is GND?

In the “good old days” (formerly known as “these trying times”), you had, at most, two layers . . . and sometimes only one. They were sometimes called “component side” and “solder side” (rather than “front” and “back”; “top” and “bottom”, etc). And sometimes, the traces and soldering was all on the same side as the components! So, like @paulvdh said, for the type of project you’re doing it doesn’t matter which side of the board you designate as “power” or “ground”.

But, like @paulvdh also said, circuits that we don’t think of as being “high speed” or “noise susceptible” will sometimes benefit, performance-wise, from having a relatively uninterrupted ground plane. Where ground planes are concerned, continuous is next to godliness - but it’s also next to impossible. So adjusting component locations and trace routes to keep the ground plane as continuous as possible is a worthwhile mental exercise, but don’t lose any sleep over the task.

I will also mention that component placement has a major effect on how easy, or difficult, it is to route the traces. That is something you will develop a “feel” for as you gain experience.

@nick

How does through hole components change the actual layout of the pcb and the designing process?

Probably not a significant change in the design process. SMT components are physically smaller, so you can pack more of them into a specified acreage. This might be a good thing, or it might lead to problems if you concentrate too much heat into too small an area. THD components give you a “free” via at each lead, which also could be either a good thing, or bad.

Do a few boards. Get familiar with the tools, and which parts of the design process are easy or difficult for you, personally. Post your project here, if your employer or customer permit, and ask for comments and critiques. Forum members tend to be a helpful group - I have never seen a request for comments get answered by a reply that begins with, "YOU IDIOT!! . . . . ". Just allow a day or so to get responses.

Dale

[paulvdh]

Some extra remarks about:

@nick

How does through hole components change the actual layout of the pcb and the designing process?

You can route a lot of copper tracks under a single THT resistor because it is so big and the pins are widely spaced. This can be a big advantage on single layer PCB’s.

SMT components don’t have holes at all, which means you can put them on both sides of the board. But if you put the footprints too close together, there is no room left for laying tracks, unless you go to more copper layers. If you look at PCB’s such as used in phones, they are usually densely packed with components on both side, but can also have 8 or even more copper layers.

But the only real way of getting a feel for the differences is to route some boards yourself. Don’t use an autorouter (even if it is available) First learn to route board manually, and then later maybe try to overcome the limitations of autorouters.

Autorouters can be a useful tool in some cases, but they are not a “press a button and go drink coffee until it’s done” tool. Many long posts have been written about this.

[Piotr]

@nick

How does through hole components change the actual layout of the pcb and the designing process?

I think most, what is important was said.

At first I started to use SMD resistors and capacitors. Those time my designing was - THT ICs at top and SMD R and C at bottom. That allowed me to have smaller PCBs than with using only THT components.
Now I use only SMD (with few exceptions like terminal block or relays) and I make all connections at top to have continuous GND at bottom (2 layer PCBs).
THT components (by definition) don’t allow to have 100% continuous GND.

[BlackCoffee]

Re: @paulvdh Using Arduino template is good but, I found dimensional differences between them and real hardware. However, bare in mind that a handful of different companies make the Arduino to the same general spec’s. So, differences are to be expected.
I just bought some Arduino Megas R3, only to find the Reset button is in the middle of the PCB and Not on corner near USB.

Whether or not using a Template, you can adjust the Z dimension to place it under the PCB. Can draw a PCB shape on the EdgeCuts layer and add the PinHeaders, Cutouts…etc Example below…

I grabbed a pinheader just to demo this (it’s not the correct quantity of pins for real use…) Also, I did not set the proper height for this demo…

Note: I made alignment marks for proper placement (versus guessing)…

Looks like you want to make your own PCB (I do) so, consider that with the Arduino underneath, the PCB can be large enough to accommodate THT part (and avoid FUSSING with tiny SMD - just my opinion…)

[EDIT - changed last image to real product. Ignore the Blue jumpers ramming into LCD, that’s just graphic and there was no need to fuss with it. Hardware is correct…]

[EDIT - FYI; before someone tells me I’m wrong about the Mega R3, last image is from Official Arduino…]

[paulvdh]

@BlackCoffee

Using Arduino template is good but, I found dimensional differences between them and real hardware.

A few years ago I bought some cheap arduino clones from China and some LCD screens that are supposed to fit onto them. They did not fit, and there was 1.5mm difference in widht between the connectors.

One of them must be wrong.

[BlackCoffee]

… always worth double/triple checking stuff… I just snagged the image below from Arduino.cc and, though Pinouts haven’t changed, I think it’s not professional for them to keep old images… Some of us base initial design concepts from info/images until having hardware in hand (as I discovered when I received the Mega’s). Not at big deal at that point but, well worth noting. And your experience serves to confirm it…

[nick]

Thank you guys for your helpful answers!

This is a picture of my schematic.

As you can see, it has several components, plus three 16-pin ICs.

How many layers do you think my board should have?

Thank you!

[paulvdh]

I’ve seen that schematic before…
… one or two weeks ago.

Something about thos MUX IC’s and drawing them according to function instead of pin numbers to clean up the schematic.

Apart from that.
Two layers is plenty for simple board like this.
It’s a good match to get some practice as a beginner in PCB design.

[EI9HEB]

Nick,

You can make your life much easier by using the labels and ground symbol.
You don’t need to run the GND wire and signal wires between the components just add the GND symbol again and add the labels for your signals.
This will make the schematic very clear to read.
You can see it on the small example bellow:

[nick]

Thank you very much guys!
@EI9HEB Yes, thank you. I know that now, but i didn’t when i designed the schematic!