Kicad board without schematic


#1

Hi,
i just build and ordered a pcb that i designed and when i got it it wasn’t what i hoped it would be.

The idea i want is really simple. It’s a small 10*100 mm strip with on one side little pads where i can solder on nickeltabs, these pads go to a via where the trace to the via acts as a fuse. Then on the other side the via goes to a big copper surface. I have drawn copper pours on both sides, removed the solder mask so i can solder on it and have drawn the wires and vias. When i got it, the wires were insulated from the pads and the via was insulated from the copper pour on the other side. Is it possible to make what i want without schematic? In the 3d viewer of kicad it all looked fine but when i got them everything was isolated from each other.

I am a beginner so i hope someone can help me out :slight_smile:


#2

Why would you want to make such a thing without a schematic?

Start by drawing a schematic with 2 connectors and wires between them.
Then make a netlist and import that in Pcbnew.

Maybe you can assign some standard footprints for the connectors in Eescheama, or else you can make up some names and draw custom connectors in Pcbnew / Footprint editor with the footprint wizards.

From there the rest is trivial.

You can make the PCB easier to draw by inserting fuses on the schematic between the connectors. Then you can design a footprint for a PCB trace as a fuse the footprint editor. You can even combine the fuse trace with SMD pads. If you do this and the fuse gets ever blown, then you can solder a SMD fuse on it, instead of having to replace the whole board.


#3

You could give your design for us to look at. With manufacturers the most basic rule is that you have to tell everything explicitly to them unless you do and want only ordinary common things.


#4

@TomTheDutchy I have promoted you to basic user level, so you can share the pcb file here.
There is almost no use case where not doing a schematic first is a good idea


#5

Yes, you can use the nifty plugin called WireIT
This is also great for Pinswap, and variant footprint adding.

KiCad needs net-names to ensure things are connected.

Are you sure 3d was ok ?
You can also load things into GerbView, to confirm it is what you hoped for.


#6

Wow, thats a great idea. Love it! I am afraid i started the process backwards by immediately wanting to draw in pcbnew. This is my original design. So the idea would be to create a new part that has exactly the footprint of the size of the nickel tab that i want to solder on, then connect that part in the schematic to for example 5V net, make the whole bottom a 5V copper pour?

I noticed that when i use the plugin wireIt the copper pour doesnt fill it up, only gives the outline, when i check it in gerber-viewer there is no copper pour. Im still learning a lot and at times it can be quite frustrating.

Thank you for the help :slight_smile:

Fuse_Strip_v2.kicad_pcb (16.7 KB)


#7

I have used WireIt on pcbnew but it keeps crashing. Sometimes just nothing happens when i activate the plugin, when i reboot my program it does work again. Also when i define a net with it, the copper pours dont work anymore. Do you have any experience with that?


#9

I’ve not had it crash, but maybe your design is more ‘empty’ than it has been tested to ?

Your PCB imports like this

Which is strange in a couple of places.
The B.cu pours have filled in all but 1 case, but the fills have what look to be clearance indents, but I cannot see what they are clearing from ?
Hmm, I hit ‘B’ to reflood, and those go away - strange, did something not load, or did you delete something ?

The zone that does not fill is net-named, but there is no net passing into that zone, that means it will not fill.
You need to match the Zone-net to the trace-net that enters the zone.

If you need large solder pads, usually you just drop a single pin component and adjust the PAD shapes.
That gives you a net-tie pad and also includes the solder mask infos.

I think this is what you are trying to do ?

Here, I quickly grabbed a 1-pin connector, and changed the PADS to SMD, RECT, resized, - when that is right, just duplicate and it copies everything, including the net name.
Then WireIT connected to Boom net, and ran to a via. (your fuse?)
The via now connects to the fill area on F.Cu, which now fills because it has a net-entering.

If you want a true fuse, I’d maybe make the via another part, so you can have a larger hole and pad.
You want to ensure the fuse is fixable copper, not the plating corners, of a tiny hole :slight_smile:
For same-action, all fuse elements should be identical lengths and widths.

WireIT added the net to the pad just fine, no crashes…


#10

The original post makes sense after seeing PCB_Wiz’s screenshots. You didn’t refresh the zone fills before creating gerbers. At least that’s how I now understand what you meant by “insulated”.

Did you even check the gerbers with a gerber viewer? It’s a must every time you’re going to send them anywhere.

In any case I don’t recommend doing anything without a schematic.

At least since 5.0 there is “Check zone fills before plotting” option in pcbnew plot dialog. It’s good to keep it checked. (There’s one bug there right now which could have affected this case, I just reported it: https://bugs.launchpad.net/kicad/+bug/1817797 .)


#11

I’ve been toying a bit around with your design, I hope you like it :slight_smile:

I first made this schematic:


Then I made a library with 2 custom footprints.
A rectrangular footprint for the “Testpoints” and a symbol for the fuse.
For the fuse I used an SMD pad on one side, and a Through Hole pad on the other side. So you don’t need to use via’s.
Ouwtch. I could have used a really long SMD pad on the other side, and then I would not have needed the Test points at all…
In the 3D viewer the Fuse looks like:

I was a bit confused about your board. You said you made a 100mm long board, but the board in your .kicad_pcb file was only 93.8mm long ??? I took the liberty to make your board 100mm long.
It now looks like:

You probably want to adjust the size of pads, or of the fuse wire.
You can do this with:
1). Open the Footprint Editor.
2). Footprint Editor / File / Open Footprint / Selectr by Browser
3). From the Library “Fuseboard”, double click on “asdf_Fuse”.
4). Single click on pad nr3 and press “e” (Edit).
5). In the “Pad Properties” window, change “Size Y” & [OK].
6). File / Save / [OK] to save the symbol back in the library.

7). Open Pcbnew, and zoom in on one of the fuses.
8). Pcbnew / Tools / Update Footprints from Library / [Apply].

At the moment you clik on [Apply] you will see that all fuses get updated. This ensures that all of your fuses have the same length and width.

The design of the board is pretty simple, but making the symbols and library was a bit “rusty” for me and took some time. Try to play a bit around with some of the settings. Maybe you want to put the fuses on the bottom. Maybe you want to remove the “Testpoints” and extend the “SMD” pad of the fuse Footprint.

Oopsie. With making steps 1) through 8) I changed the width of all the Fuse wires from 0.25mm to 0.4mm, and that is probably too thick.
I’ll leave it as an exersize for you to change them back to what you want. :slight_smile:

One more thing:
I made the outline of the Zone on the bottom very big and with ragged edges, and I did this on purpose. The zone should be limited by the board outline, but if anything goes wrong with the board outline and you make Gerbers, you will see that something is wrong.
2019-02-27_FuseBoard.zip (8.8 KB)


#12

Wow. I have never seen a more supportive community then this one. Thank you so much guys! I’m going to go at it straight away and will post some pics when the definitive parts are in. The thickness of the fuse wires doesn’t really matter that much. It’s for 18650 cells, they can theoretically short which means all the other cells will unload through it and blow it up. That will be easily 100 amps so any trace will evaporate immediately. It’s practically never going to happen and when it does you wont notice it because the cell just gets disconnected. Therefore reusability of the fuse is not a must, especially since the strips will cost around 10 cents a piece. I do like the idea of placing a smd pad so that you can if you wanted to place a manual fuse there.

Many thanks :smiley:


#13

I have seen thin traces used as fuses from time to time, but I have also come across comments saying they are unreliable due to inconsistent fusing currents. Can you post a reference to a verified procedure for designing PCB trace fuses?

Dale


#14

I have never used a PCB trace as a fuse before, nor do I know anything about the fuse currents for those things. My personal interest in this project for me was to figure out how to design custom Footpints and Footprint library and how to add them to a project. That the object in question is a fuse is purely accidental.

In lot’s of applications consistent fusing currents are not very important, but still add some level of protection, and you get them for free on the PCB, which makes them still attrictive for some applications. An example of this is using such a fuse in the antenna coax of a TV. Normally it has some uA antenna signal, but if the coax accidentally gets nailed into the house wiring, they want to blow the fuse. Anything between 10mA and 10A is OK in this situation.
A long coax cable might have such a high resistance that it does not blow the mains fuse, but might become hot enough to be a fire risk in such a situation.

When you’re interested in PCB traces as fuses, then watch this video from Mikes’ Electric Stuff:
https://www.youtube.com/watch?v=Fmcg_cVO_1s

It is about a consumer microwave with such a fuse and when it blew it caused a short on a nearby PCB which destroyed so much electronics that it is beyond economical repair.

A very naive approach to PCB fuse calculation:
Copper melts at 1084 Celcius:

https://en.wikipedia.org/wiki/Copper
If I put a temperature rise of 1050Celcius in KiCad’s PCB Track Width Calculator, (35um Copper Thickness) then I find:

Wdth: Current:
0.10 3.49144
0.15 4.68459
0.20 5.77101
0.25 6.7844
0.30 7.74315
0.35 8.65873
0.40 9.5389
0.50 11.2139

Note that the Track Width calculator clearly states, that it is only valid for temperature rises upto 100 Celcius.

Out of curioucity I had a quick peek at IPC2221,(124 page PDF) but PCB trace fuses are not mentioned there.
https://www.sphere.bc.ca/class/downloads/ipc_2221a-pcb%20standards.pdf


#15

The picture I posted earlier was plucked directly from a DuckDuck Image search. Just now I re-encountered it on:
https://electronics.stackexchange.com/questions/200350/can-thin-sections-of-copper-traces-be-used-as-fuses
Citation for the source of the Image points to:
http://www.bcae1.com/images/rca/temporaryrcashieldrepair.html

The article on StackExchange also points to a 18 page document about designing PCB Fuses:
https://www.ultracad.com/articles/fusingr.pdf

If you’re really serious about this stuff, you may want to look into:
“PCB Trace and Via Currents and Temperatures:: The Complete Analysis”, which is a 202 page paperback, with a price tag of USD58.
https://duckduckgo.com/html?q=978-1530389438


#16

Hi Paul,
I have been making my own footprint and trying to recreate what you made. I’m still a bit confused about how you use the different layers. For example on the internet i found a tutorial that where you only draw a rectangle in silkscreen as a outline.

https://kicad.txplore.com/index-p=111.html

Now in your design i saw that you used multiple layers to get the result you wanted. For example do you need to manually draw every layer of the component or is there some automatic conversion?

When you just use the silkscreen the component works, but you are not defining any soldermask, copperpours, etc. Is that done automatically when you create it with silkscreen in de footprint editor?


#17

Pads can define multiple layers in one go (For most SMT pads it makes a lot of sense to have copper, mask and paste defined by a single entity. Similarly with THT pads. Here you want all copper layers and top and bottom mask defined by a single thing.)

In reallity only the layers listed above are needed for the device to function. Every other layer is to make it easy on the user. (Add documentation, Ensure clearance between parts is correct, …)


#18

I had a brief look at the txplore tutorial you mentioned, and it looks quite complete. Date on top is from 2016 though, and some details probably have changed.

If you want to get a grip on designing your own footprints, or even make a PCB, you have to have a clear idea of what the layers do and how they work.
Your first attempt (Start of this thread) failed because the pads were on the bottom of the PCB, while the copper tracks that should connect to them were on the top.

A lot of the layers in KiCad have very specific meanings ( Silkscreen, courtyard, Edge.Cuts, etc) while other layers (Dwgs.User, Eco1.User) are mostly arbitrary, and are meant for your own notes.

You can read more about Layers in the Pcbnew User Manual.
On my PC (And somewhere on yours if you installed the documentation):
file:///usr/share/doc/kicad/help/en/pcbnew.html#_layers
Or on the KiCad Website:
http://docs.kicad-pcb.org/

KiCad does a lot of things automatically.
If you make a new footprint, then it automatically puts the Reference name on the Silkscreen. If you draw a SMD pad, then it automatically creates a cutout in the solder mask and solder paste.
I created the asdf_Testpoint from scratch by defining a single SMD pad.
I created the asdf_Fuse by copying data from a 1206 resistor (There may be some leftovers from the resistor in the footprint) and modifying it a bit.
I drew the fusewire as a pad, and then manually removed the [v] checkbox for the cutout in the soldermask, so it gets covered under the mask.
I would have liked to draw it directly on the copper, because of DRC, but I don’t know how to do that.
I “abused” a THT (Through Hole Technology) pad as a via, because I had troubles starting a track from the pads because the “fusewire” pad needs a clearance and I could not get to the center of the pad with a track.

You have now a custom Footprint library in the FuseBoard project. I recommend to add a few Footprints to it, and then examine what it means.
With the 3D viewer you can have a pretty goot representation of what the final result will look like.

Pcbnew / View / 3D Viewer

Oops, I just looked at the bottom of your board in the 3D viewer.
It automatically created “Thermal reliefs” in the connection between the zone and all the pads. You probably want to remove them for all the fuses, and maybe also for the solder pad TP11, or at least make those spokes wider, or they may also become fuses on you PCB :slight_smile:

Most of the things in KiCad are not very difficult, but because there are so many details you can change it all becomes pretty confusing.
Here is a screenshot of the bottom of the PCB:

Then I grabbed the solderpad on the bottom and dragged it to a corner:

You can see it moved the pad, but the spokes from the thermal relief (Green cross = copper under solder mask) has not moved.
You can update the zone settings by pressing “b” in Pcbnew.

KiCad makes the zones according to a bunch of rules. The cutout for the pads are all automatically calculated. I drew the zone itself as a big pentagon around the rectangular PCB, and still KiCad knows to only fill the zone upto 0.5 mm from the edge of the PCB.

Don’t be afraid to experiment. Worst case you delete the edited files and start over from the zipped project. (If you made something beautiful it’s wize to make your own backups of that).


#19

Hi, i have been at it for a while and slowly i am getting the hang of it. This is what i made, hopefully you guys can have a look at it( i already ordered it at jlcpcb since it’s so cheap and fast). Thanks for all the support!
Fuse_Strip_2-B.Mask.zip (16.3 KB)


#20

You’ve done quite some tinkering on your board :slight_smile:
Getting started with a program like KiCad (or any other PCB package) takes quite some time, but once you’ve got some experience it will get progressively better & faster.

You have only Gerbers in your project, not the KiCad project itself, which makes it a bit harder to look at it.
A few things I see:

  • You’ve left the via diameter at it’s default of 0.4mm, which is quite small.
  • There is no solder mask over your fuse wire, which makes it (a bit?) less reliable. (Dirt, oxidation).
  • There are 2 drill files, NPTH drill (Not Plated Through Holes) is empty.
  • I see slight differences in Y coordinates. On a coarse grid it is easier to align perfectly, than it is to align approximately on a fine grid.

Have you tried to base the fuse wire dimensions on the “fusingr.pdf” I linked?
Do you think it is a good idea if you sacrifice one of your boards to test the fuses?
You can do this relatively easy by using a few batteries in parralel to make sure each has a low enough current to not damage them, and use a few meters of copper wire as a resistor to approximate a test current.


#21

Sorry, that was the wrong file. I updated the file in this post.
I assume that having soldermask over the fuse wire is not good because they might burn out really violently, but it’s not really based on anything. I didn’t think about the via diameter, bigger would indeed be better.

I am definitly going to test one of these little board’s to the max. I have a lab power supply which allows me to regulate current precisely so by slowly increasing the voltage i can regulate the current. I plan to manually look for the limit with my powersupply, but i am also going to short it out with 12 cells in parallel because i need to know how it reacts. The pcb’s should be in tomorrow, cant wait for the result. Will keep you posted!Fuse_Strip_2.kicad_pcb (40.1 KB)