Touch circuit sound, led. 555 timer

[eTech]

If I were going to manually route this board, here's my approach.

1. Place all parts at locations where placement is critical.
Orient all IC's so notch is in same location.
Place the IC decoupling cap close to the +supply pin of each IC.
2. Place parts in close "functional block" proximity to each other.
This helps create the shortest track.
3. When routing tracks, only route tracks between pads and use no more than two connections to pads.
(Do not create a "branch" off of a track).
4. Use 2-sided board (all parts on top).
4.1 Plan to have a "ground" plane on bottom of PCB.
4.2 Route +V tracks and signal tracks on top layer.
4.3 Route signal tracks on bottom layer only when necessary.
4.4 Route +V tracks first and try not to use vias.
4.5 When all tracks have been routed, add a copper pour (ground plane) to bottom layer.
4.6 When all tracks have been routed, add a copper pour (ground plane) to top layer.
The ground planes help keep noise to a minimum.

5. Clean up silkscreen.
Orient text and ref designators so they can all be read with the PCB oriented in one direction
6. Perform design rule check and correct errors.
(No use submitting a PCB for manufacture if it can't be made)
7. Generate Gerber plots and verify with Gerber file viewer.

Hopefully, if you follow these guidelines you'll have a nice looking PCB designed with a purpose.

 

[eTech]

HERE is my final file. i hope. ive cleaned it up a bunch. the rule checker is upset about overlapping screens but it visually looks ok to me. Can you recommend a developer for this PCB i need 20. 50x80mm

Not bad.

I would use JLCPCB at JLCPCB.com.
They are excellent quality, inexpensive, and deliver quickly.

 

[eTech]

HERE is my final file. i hope. ive cleaned it up a bunch. the rule checker is upset about overlapping screens but it visually looks ok to me. Can you recommend a developer for this PCB i need 20. 50x80mm

I would take a look at cleaning up via locations and even remove them is possible.

 

[ThomsCircuit]

I have to absorb this. That's alot to understand. I'll do what I know and research what I dont then if I need (and I will) ill reach out again. Thank you sir.

 

[eTech]

I have to absorb this. That's alot to understand. I'll do what I know and research what I dont then if I need (and I will) ill reach out again. Thank you sir.

Ok....good luck.

 

[gophert]

The through holes go all the way through the board. You don't need to add a via to get the trace to the "right" side of the board before you get to a through hole point. Most of your vias can e eliminated.

 

[ThomsCircuit]

Most of your vias can e eliminated.

If you could tell me what a vias is and how would I eliminate them.

 

[gophert]

A via is the little "rivet" in the board that allows a per trace continue on the other side of the pcb.

 

[rjenkinsgb]

4.1 Plan to have a "ground" plane on bottom of PCB.
4.2 Route +V tracks and signal tracks on top layer.
4.3 Route signal tracks on bottom layer only when necessary.
4.4 Route +V tracks first and try not to use vias.

That seems "upside down" to conventions, or are you calling the solder side the top?

Normally the interconnecting tracks are on the solder side (underside) and the ground plane, when used, isolates the components from signal tracks that pass underneath them; as well as providing a low impedance, low-noise ground.

Example below - a board waiting for a few final parts, with an almost complete ground plane, just a couple of segments of track set in it where they bridge other tracks on the underside.
The "vias" are the plated-through holes that connect the top and bottom tracks but do not have components fitted.

For info, It's only soldered on the underside - the solder visible around component leads is what has flowed in to the plated holes as the underside was soldered.

 

[ThomsCircuit]

is the little "rivet" in the board

Ok. Got it. So I dont need them because they are for diagnosis. Something I will not be doing. So I can just delete them. But you had said "most of them" so I would have to know which ones are necessary or is it my choice to keep some?

 

[eTech]

That seems "upside down" to conventions, or are you calling the solder side the top?

Normally the interconnecting tracks are on the solder side (underside) and the ground plane, when used, isolates the components from signal tracks that pass underneath them; as well as providing a low impedance, low-noise ground.

Example below - a board waiting for a few final parts, with an almost complete ground plane, just a couple of segments of track set in it where they bridge other tracks on the underside.
The "vias" are the plated-through holes that connect the top and bottom tracks but do not have components fitted.

For info, It's only soldered on the underside - the solder visible around component leads is what has flowed in to the plated holes as the underside was soldered.

View attachment 129888

your way seems upside down to me
The ground plane on a two-sided board is on bottom and additionally, but optionally, on top as well.
I keep the +V tracks (any +V tracks) on top without vias if possible. So the parasitic's can act like a filter.
I could, optionally, use a +V plane on top as well, but usually choose not to unless high currents are involved.
Even though the board youv'e shown is only soldered from the bottom, the result is still the same as if it were soldered from
each side (for the benifit of the TS).

 

[eTech]

Ok. Got it. So I dont need them because they are for diagnosis. Something I will not be doing. So I can just delete them. But you had said "most of them" so I would have to know which ones are necessary or is it my choice to keep some?

No....remember when I said the autorouter doesn't do a good job of routing?
This is an example.

Vias, on a double-sided board, are "plated thru holes" that are used to pass a connection from one side of the board to the other.
The autorouter will use them as it tries to make connections between pins on devices. Its standard practice to clean them up after an autoroute.
Back in the day, vias were expensive. There is still an additional cost but not much anymore.

 

[rjenkinsgb]

The ground plane on a two-sided board is on bottom and additionally, but optionally, on top as well.

All I can say is that in 50 years of professional electronics, I have never seen a commercially designed two layer through-hole PCB with a ground plane at the underside (other than as fill in addition to the topside ground). Surface mount boards and especially such as RF stripline obviously have different rules.

Example - in a quick dig for commercial double sides boards I found five, all in the photo below. All ground planes on top side only or primarily.
Colander ground plane veroboard does not even have solderable track strips on the top, only solderable points over the solder-side ground bus tracks.

As I said, one of the functions of the ground plane is to act as a signal isolator between components and unrelated signal tracks. It can only do that if it's between the two.

Anyway, just for information, not trying to cause an argument.

 

[ThomsCircuit]

1. Place all parts at locations where placement is critical.
Orient all IC's so notch is in same location.
Place the IC decoupling cap close to the +supply pin of each IC.
2. Place parts in close "functional block" proximity to each other.
This helps create the shortest track.

this i believe i have done

3. When routing tracks, only route tracks between pads and use no more than two connections to pads.
(Do not create a "branch" off of a track).

clarify a pad is where a components are soldered

4. Use 2-sided board (all parts on top).

the design i currently have has a 4 layers. two copper and 2 silkscreen. all components are on top. (see photo.)

4.1 Plan to have a "ground" plane on bottom of PCB.

i looked this up. i understand this.
has a few uses but for my board it is to reduce noise. so it will be defined as a silkscreen added to the bottom. assigning a NET is not necessary.
i am to add this last. it shows up in Layers as a silkscreen.
i make a copper rectangle, pour it, then assign it to net "VDD" ground. if needed. (see photo)

4.2 Route +V tracks and signal tracks on top layer.
4.3 Route signal tracks on bottom layer only when necessary.
4.4 Route +V tracks first and try not to use vias.

working on it.

4.5 When all tracks have been routed, add a copper pour (ground plane) to bottom layer.
4.6 When all tracks have been routed, add a copper pour (ground plane) to top layer.

i believe this is a clarification of 4.1

 

[eTech]

clarify a pad is where a components are soldered

yes. A (pin)pad is where a component pin is inserted and then soldered.

the design i currently have has a 4 layers. two copper and 2 silkscreen. all components are on top. (see photo.)

You are correct in the context of "virtual" layers of the PCB design tool.
But...the term "layers" in the context of the physical PCB board refers to the number of copper layers.
You board is a double-sided (or, 2-Layer) through-hole PCB. This will be reflected in the Gerber files you send to the fabrication house. When you specify the layers to the fabrication house, you will need to specify the number of copper layers (2).

i looked this up. i understand this.
has a few uses but for my board it is to reduce noise. so it will be defined as a silkscreen added to the bottom. assigning a NET is not necessary.
i am to add this last. it shows up in Layers as a silkscreen.
i make a copper rectangle, pour it, then assign it to net "VDD" ground. if needed. (see photo)

The ground plane would be defined as a "copper pour" in DSPCB. It is not a silk screen and is usually not added until you have completed all placement of parts and routing of tracks. The "pour" will be need to be assigned to the same net name you used for "ground" before you "pour" it, so there is no need to route tracks for this net as, when poured, it will automatically connect all ground pins to it.

You can watch this video for details:

DesignSpark PCB - Copper Pour Basics Part 1

We have noticed quite a few questions from our users regarding how to use Copper Pour within DesignSpark PCB. We have prepared a new video tutorial to show you step-by-step.

www.rs-online.com

i believe this is a clarification of 4.1

yes.

 

[ThomsCircuit]

it took me 5 hours but i manually routed the tracks. hot and signals on the "signal" layer, grounds on the "ground" layer. minimal vias (12 total) signals on bottom layer only when necessary. I have yet to ad the copper pours. I need a few "pours" myself. could not figure how to move tracks from over crowded pads

 

[ThomsCircuit]

Same PCB with assigned bottom copper pour "Ground pad" i notice all the ground tracks are not visible any longer. i assume they "attached" to the pour layer.

 

[eTech]

Same PCB with assigned bottom copper pour "Ground pad" i notice all the ground tracks are not visible any longer. i assume they "attached" to the pour layer.

I can't tell the pour from the rest of the design in your image, but yes, any pin pad or track that is assigned the same net as the pour should now be merged with the pour.


Any pin pad that connects to the pour should have a pad that looks like this:

This is called a "thermal pad". It is designed to allow the pin to heat up and solder. Otherwise the pour would draw heat away from the pin and it would be difficult to solder.

You'll need to do a spot check and verify the thermals exist. You dont have to check all, just a couple of them.

 

[eTech]

it took me 5 hours but i manually routed the tracks. hot and signals on the "signal" layer, grounds on the "ground" layer. minimal vias (12 total) signals on bottom layer only when necessary. I have yet to ad the copper pours. I need a few "pours" myself. could not figure how to move tracks from over crowded pads

Its not unusual for it to take long to manually route a board. I've taken days to route a board. Just depends.
I expect you will make multiple design passes since this is your first board. But it will get easier.

 

[ThomsCircuit]

You'll need to do a spot check and verify the thermals exist.

i can see them. some have two and others have more. i assume its because of room and that there are existing tracks going to the pad.

i did get an error when i added the top pour layer. A single pad U3.6 (pin6) did not receive any thermals. the images below show the same area with each layer. is this a problem? the green image is the bottom layer, blue is the top, then one shows both. I can see that the pours did alter my tracks. i can see many tracks in the image that is showing both layers. All very interesting. i hope i have provided you with enough detail to see that i have done a good job here and most importantly that the issue with pin6 is really an issue. it is a DIP socket and not a component.