There are a couple of ways to do it - for Example:
• First, set up your GND Net for the GND Tracks
• Can use the ‘Create Filled Zone’ tool
• Can Draw Zone Shape using the Draw Tools
Either way, after drawing the Shape, you need to Fill the Zone
Example - Video shows Drawing on B_Cu using the Draw Tools
You can see the GND Pads/Tracks get absorbed into the GND filled area.
I drew a Shape but, if wanting the full PCB Shape, you can select the Edge-Cuts, Copy it and Paste into B-Cu (and set it to B-Cu layer) then continue the process… [could also simply Draw the Filled Shape using the Edge-Cut layer as a guide… etc]
ADDED: You can set the Pad connection to the Type you want - video shows Solid. Screenshot below shows PTH (≈ Thermal). The one on the Left…
Select Bottom layer and among tools at right side you have “Add a filled zone”. You can draw rectangle bigger then your PCB. When you start you will be asked to specify at what layers it will be and what net. Electrical Properties you probably can left as they are default. I always change them to:
Clearance: 0.25
Minimum width: 0.2
Thermal relief gap: 0.25
Thermal spoke width: 0.25
Among visibility tools on the left you have tools to show/hide zone. During routing KiCad ignores zones - you can place footprints and route tracks like there were no zone. Press B whenever you want zone (all zones) to be refilled by KiCad.
I don’t know what’s going on with the zip file. I downloaded it from this forum and it opens without problems. I created the file on my Linux box, with some unknown program (It was just installed automatically).
But I’ve made a 7z file now. Maybe that works better for you.
I use a “Mountinghole”. There is also a “Mountinghole with pad” in case you want to make an electrical connection to the mounting hole. but also, the Choose Symbol dialog has a search function:
Footprint placement has improved a lot and the PCB can now easily be routed without even thinking much about it.
Try this for fun:
Hover the mouse cursor over a pad.
Press x to start a track.
Press f to finish routing (to the nearest pad) of that track.
Personally I don’t like wired parts. I find SMT easier to work with.
No messin’ with drilling holes if you etch yourself.
No constant turning between front and back (Mirror image madness).
No parts falling off because you of turning the PCB upside down.
You don’t have to cut the leads of all those parts.
But it’s your project, and you already made the choice for THT and that is of course also fine. One thing I would change (and forgot to mention earlier) is that I would use put my resistors flat on the PCB instead of vertical. You have plenty of room to do this and it makes the PCB less fragile. But do pick the right footprint for the resistors you have. The easy way is to take one resistor, bend the leads in an “easy way”, and then fit them into a piece of matrix board and count how many distances you have for the pitch between the leads. (Probably 10.16mm (400mil) or 12.7mm (500mil). Another advantage of laying the resistors flat is that you can easily use them to bridge a few tracks. For example, you can place R2 in such a way that it jumps the tracks between C11 and R6, and as a result you don’t have to detour the track under RV2.
Additionally. Usually it’s easier to have both the schematic and PCB editors open, and then start placing parts on the PCB that are connected together on the schematic, and then immediately draw the tracks (or at least some of them) before you place the next footprint on the PCB. This gives you a much clearer overview of the PCB taking form. You can even drag footprints around (with the d key) while keeping tracks attached. So you can change their position later easily if it is needed.
I see your point about the resistors. I’ve changed those to lay them down.
I would like to play around with wider tracks and wider clearance between tracks and pads. Is this done be creating different net classes or is there another way?
There are different ways to set the track width. Setting up net classes is the most flexible and powerful way, but it requires preparation to assign nets to those net classes. Another way is to use: PCB Editor / File / Board Setup / Pre-defined Sizes. You can then select a specific list from that list to use with the combo box in the upper left corner of the PCB Editor:
It is also possible to draw tracks and then change their width and clearance afterwards (with a right click and entering data in the properties box (or in the properties manager). Making tracks or clearances wider is a nuisance though, because it only changes the track width and clearance, and as a result there will be MANY DRC violations that you will have to fix by dragging tracks further away.
U2 is an TDA7284 Some IC dedicated for audio cassette players. It’s an old one working on audio frequencies only. It’s datasheet also show mostly electrolytics in the examples.
I know that I haven’t followed everyone’s suggestions here, but I really appreciate all the help. I’m thinking that designing a board layout, while there are certain electrical and physical parameters that must be considered, is part ‘artistic’. Because I’ve worked on a lot of electronic equipment over the past 50 years, I personally prefer wider tracks. I’ve seen some boards that were mostly copper, where the tracks were much wider than needed for the circuit to work, but it made working on the board much easier.
So here’s my latest try, using a track width of .7 mm and I think a clearance of .5 mm. I’m actually using Freerouting, which appears to do a pretty good job, especially compared to autorouters that I’ve seen in the past (30 years ago).
I printed out this board layout in 1:1 size. It may not be exact, but it look close. The pads and holes seem to be a bit small, so I’m going to try to increase those sizes a bit.
Nothing wrong with that. There are a lot of different ways that lead to a satisfactory end result, and a part of the suggestions are mostly personal preferences too.
Looks quite reasonable.
I did notice that the examples in the datasheet also have some small ceramic capacitors. I don’t know how important those are for the design. You’ve never posted a schematic.
Also, a review is easier if you zip up the whole project and upload it (Exclusive the backup directory and other unnecessary files)
Some (small) notes.
Assembly is a little bit easier if all electrolytic capacitors are in the same orientation. (I learned that in a production environment long ago).
Rotate R2 90 degrees and put it just above R5, so the resistor is used as a bridge to jump over those two tracks (this is an common and important trick for PCB design).
The track between pins 8 & 10 of U2 can easily be routed under the IC.
Check your voltage regulator. I’m not sure, but it may need some ceramic capacitors for stability too. (Also, if it turns out to not be needed, you can just not place the footprint. That’s easier then modding in a kludge for when it is needed but there is no room for it).
R10 is still vertical.
How did you make the 0.7mm wide tracks? I see neither a netclass setup not pre-defined track widths. It could be this is because the project file is missing but I’m not sure.
But overall, these are all small things, and it looks quite good for a first design:
Do note that KiCad does not have 3D models for all footprints, so it’s normal that some appear to be missing.
Do you want to etch at home or order a PCB somewhere? Before you go though this process, you should double check whether all parts match with their footprints. Especially the potentiometers and capacitors can be troublesome. Those can be bought in many different form factors. For test fitting you can use:
This has been going pretty well, but I found that I needed to enlarge my mounting holes.
So, I extended the size of the board slightly, in all four directions.
I changed the footprint to a slightly larger size (3.2mm M3 Front and Back).
Then I reselected the bottom of the board and created a zone (GNDREF), just like I’d done before.
Then I Draft Filled the Selected Zone, just like I’d done before.
But this time, on the bottom of the board, it created a ‘space’ around the pads that are around the mounting holes such that the pads are insulated from the ground on the bottom of the board. All other ground connections to parts look good.
I changed the hole pattern back to what I’d used before, and repeated these steps and it created a ‘space’ around the pads that are around the mounting holes (just like it did with the 3.5mm M3 holes) such that the pads are insulated from the ground on the bottom of the board. All other ground connections to parts look good.
Obviously, something is different than before. What would cause this now and how do I fix it so that the pads around the mounting holes on the bottom of the board are connected to the GNDREF foil?
Make sure you use the Mountinghole_PAD schematic symbol.
Make sure the pad is connected to the net you want.
Change the footprint link in the schematic symbol to point to your bigger footprint.
Schematic Editor / Tools / Update PCB from Schematic [F8]. And make sure the “Replace footprints with those specifiec in the Schematic” checkbox is on.
Ok. I’ll start over and try that. I was trying to change the holes in the pcb editor
Also, how can you make a change to a patter in the library and save it. I keep getting a warning that it’s read only, even when I try to save it as a new file name.
Patter? Footprint or symbol? But for either, … / File / Export / Symbols to Library (Or **Footprints to Library) in the PCB Editor should work. It even helps yo by asking whether to update the footprint or symbol links in you project. If you changed the footprints in the PCB Editor, you can also port the changes back to the schematic with: PCB Editor / Tools / Update Schematics from PCB (Which is the other way around from the normal update.
I don’t know why you have trouble with creating a New file. Are you sure you have write permissions to the location you want to create the file?
Libraries installed with KiCad are read only. Create your own libraries, copy the original footprints there and edit them. Creating a new global library gives me this dialog by default:
