Is solder mask necessary?

Thank you. Solder mask will be a regular step in the process.
You’ve got a working pcb from 1986?

I clicked around to try to figure out how to apply solder mask…and it looks like it’s done automatically.
I guess my next step is to learn how to inspect the gerbers.:confounded:

It is nothing unusual.
In 1982 beeing a student I have build oscilloscope. All pcbs were made by:

  • printing design at milimetre graph paper,
  • punching PCB holes positions through this paper,
  • printing a tracks with shoes painting paint taken (using siringe) into ballpen refill with deleted ball,
  • etching with FeCl3,
  • removing paint with solvent,
  • drilling holes,
  • cleared with sandpaper,
  • covered with alcohol dissolved colophony.

It was soldered with no PbFree solder so it is still working.
I thought about putting here a photo of its interior but thought - not place for it.

inspecting the Gerber files is trivially easy to do with the gerbview tool that is part of the KiCad suite.

That’s amazing. It would be great to see a picture of it. If it’s not against the rules it please post a picture.

I was becoming more familiar with gerbview last night. It was easier than I thought but I still didn’t save anything. There is still one issue I can’t figure out: My signal traces are on top while my THT solder pads (annular rings) are on bottom. Are the through holes plated or should I put the signal traces on the bottom?.

It depends on how you are getting this board made.

  • If you are making it yourself (either with by chemically etching or milling the copper away) there won’t be any connection from the top to the bottom of the board that you don’t do yourself. I don’t know of any home DIY hole plating technique. Just soldering short pieces of wire from top to bottom or rivetting.
  • If you are sending your design out to one of the many PCB services that do short run “prototype” services (check PCBShopper for getting a quote from many different services), the default service is a double sided board with plated through holes (PTH).

Personally, I would suggest the second option. Pricing is comparable or cheaper than buying the supplies for DIY, you never pay for manufacturing errors (design errors are something different), and depending on who you get to make the boards the turn time is only days to weeks. I’d only use the DIY if I MUST have the board that day or next day.

1 Like

I’m going to use JLCPCB. I’m sure everybody has seen the 10 boards for $2 promotion. I couldn’t pass it up especially since this is my first attempt to design a pcb.
I have a pcb that was designed years ago by somebody else. I never understood how it was actually built. I was happy that it worked! It has plated through holes but I wanted to be sure that PTH was the standard.
I had to think about the differences between thru holes, vias and mounting holes. I had to learn a ton of new concepts but thankfully I’m almost finished.
Thank you.

One way to think of them that might help (and possibly annoy you when other people inevitably use them wrong :wink: ) is this:

  • Thru holes are plated holes intended for component leads or wires to be soldered through the board. The plating allows for solder through the board to help mechanically support the component or wire better. That the plating allows power or a signal to change layers is a secondary benefit.
  • Vias are plated holes who’s primary purpose is to allow power or a signal to change layers. They are not intended to have component leads or wires soldered to them so usually they are smaller diameter. (They are, however, useful when making circuitry modifications to an existing board to solder a small 30AWG wire to for making new traces.)
  • Mounting holes are (usually) not plated, and are designed to physically attach hardware to the board. Occasionally they are plated, usually to allow an electrical ground connection to the chassis that the board is mounted to. Though some engineering practices don’t allow this because of a philosophy of not combining electrical and mechanical purposes in one feature. (If you are reading carefully, you will notice that through holes violate this philosophy… This aspect is conspicuously ignored for smaller component, but for heavier components mechanical mounting is added.)

I’ve been thinking about your question a little more. There are some people who would move your signal traces to the bottom for any of several reasons:

  • Purely aesthetic of removing the cluttered look of the traces from the component side of the board. But there is the complimentary aesthetic of “showing off” the traces on the same side as the components. This choice is fully in the hands/mind of the designer.
  • It is easier to make design changes to a populated board if components aren’t physically covering traces. (You can’t cut a trace if a component is in the way.) It is also easier to reverse engineer a board (because of lack of or lost design documentation) if you can see all the traces.
  • If all (or nearly all) traces can be put on one side, then putting them on the bottom allows the top (component side) to have a full (or nearly full) ground plane to:
    • shield sensitive components from noisy signals.
    • shield signal traces from noisy components.
    • simplify layout by removing one of the nets with a large number of connections.
    • provide good return paths for signals almost without thinking.

Ultimately, it is your choice (or if for pure aesthetics, your customer’s choice) to leave your board as is with your traces on the top of the board or to move the traces to the bottom side.

1 Like

It can also be useful for a non-connected hole to be plated and have an annular ring. It makes it more durable when the screw is tightened. There can also be small vias around a larger screw hole. See the KiCad’s standard library MountingHole footprints for examples.

1 Like

There is a lot of useful information in these replies and I will revisit this thread from time to time.
Wireless motor control is one area where I want to experiment because of RF and inductive noise.

Personally I have nothing against going from time to time a little off topic. But putting photos being off-topic seems for me too-much.
Recently I learned that clicking at your symbol I can send a message “off-line” to you.
So I will send you the 3-side photos of interior of my scope and its screen view with simple (one day made) wobbulator attached to it.

I especially question the shielding part of your response. Especially for signals on the same pcb you will be in near field which is incredibly hard to shield.
The main reduction (as far as i understand it) is a direct result of the reduction of emissions in the first place. Reason being the reduction of the area generated by signal and return path. (Which you get for free by the return path being determined by the lowest impedance path that is available on the uninterrupted plane. -> Return path will be directly below the signal.)

I will not give my head for it but I have read that:
If you have a solid GND at your PCB and if you separate geometrically sensitive signals from noisy sugnals (like 2cm width zone with GND and without signals then you get pretty good separation because these signals don’t mix their return paths in GND. There are people who just says it is better solution then thinking about separate GNDs connected in only one place.
Try to define such one place connection for 4 input digital scope.
You can think of input sockets GND being connected with case.
For each of 4 A/D converters you read in datasheet: “connect analog and digital GND in one place just under converter”.
How to do it?

And about external signals (internal also).
If a track lies 1mm from continuous ground plane I imagine any incoming EM field as reflecting from that plane. So its amplitude is 0 at GND, and full at 1/4 of wave length from plane. For 1GHz the wave length is 30cm. So the maximum amplitude is at 75mm from ground plane. So the amplitude at 1mm is sin(90st*1/75)=0,021 of maximum amplitude. The lower frequency the better result. The same effect is if you think about track as emitting antenna - the emitted signal is combined with reflected from ground plane (during reflecting signal is reversed).
PCB is not vacuum and ground plane is not superconductor so my calculation is not accurate but gives the rough idea how ground plane shields PCB.

Separating grounds is only a viable option if you never have a trace cross that gab. (Otherwise place a cap near the trace to connect the two grounds to ensure that there still is a return path. Without that you create a very efficient slot antenna.)

DC/DC converters are one system where it can make sense if you also ensure you do not violate this assumption with other signals. Another example is a guarded crystals for your MCU but you need to ensure no (“important”) trace crosses that area on any other layer.

If you have such a case then either use keepout areas to create the separation or use net ties.

6 posts were split to a new topic: Explaining the design process on the example of a wobulator

I’m glad you mentioned the topic of noise. I’m reading the dialogue between you, Rene_Poschl and Piotr. I’m going to perform some new tests on a project I put aside months ago because I couldn’t find the source of the problem with it.
I will rewrite a program and replace the DC motors with LEDs. The LEDs will remove the inductive noise. If the problem that I had disappears then I know the problem can be solved by pcb design.

No. Your conclusion goes too far.
You only know that a problem can be solved by replacing motors with LEDs :slight_smile:
I suppose solving the problem would need some schematic changes and not only PCB design changes.

I hope the forum will allow me to ask for advice concerning schematic changes if the need arises.
The LED tests will also help me see if my code is a problem.

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.