Kicad board without schematic

Layout
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:

1 Like
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

1 Like
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.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:

image
image1049×406 41.6 KB

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

image
image1049×406 42.1 KB

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.

image
image1049×406 40.6 KB

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)

22

When the fuse wire is bare copper it’s resistance will vary more over time because of oxidation and dirt, which makes the fuse less reliable.

Fuses can only “burn out really violently” when there is a lot of voltage over them. With low voltage fuses the current simply stops as soon as the fuse wire breaks, but with high voltage over the fuse there will be a substantial arc which melts more of the fuse wire before the fuse current stops.

Not too long ago I was looking at some youtube video’s about solar panels and electrical faults and fire hazards. Think for example about a burning house and firefighters want access to the house via the roof. Then how do you treat a damaged solar installation which may have 600V and can deliver 10A continuous?
DC currents are able to generate much longer arcs then AC. With AC the conductive plasma arc extinguishes momentarily at each zero crossing, and it has 100 opportunities to stay out each second.

There are coarses for becoming aware of potential risks and learning how to handle such situations. There are also plenty of tests on youtube which show what kind of sparks such a 600V 10A installation is capable of generating.

In the latest iteration of your board you have Silk screen print over the solder pads. Some manufacturers print the silk screen over the coppper, which makes soldering difficult, while other manufacturers assume you do not want silk screen printed directly on copper and they remove it.

On the side of the fuses you also have an exposed copper strip over the whole length and this gets quite near the fuses. If an arc is generated when a fuse blows, it may arc over to this copper strip.

Almost all copper tracks are 0.5mm wide, but in one corner you have a track of 0.25mm. Did you look at your board with the 3D viewer before ordering them?

23

Hi everyone,
The pcb’s are in and they look great. Some minor bugs but nothing major.

IMG_20190314_091811886
IMG_20190314_0918118863120×4160 2.9 MB
IMG_20190314_091755655
IMG_20190314_0917556553120×4160 2.32 MB

The lessons i have learned is that it makes a big difference to create footprints. The WireIT tool almost never works for me, i dont know why but when i click it nothing happens, and sometimes it does.

When i comes to the design of the board i already know i want to make a few changes. Soldering the tabs on there is okay but pretty labour intensive. My next idea is to make thin slots where the nickel tabs slide through and then you solder the joint. I contacted jlcpcb and the minimum plated slot thickness is 0.65.

Things i want to learn/figure out are the following:

  • How to create slots
  • How to combine slots in a footprint, you cannot use the edge layer in footprints
  • How to efficiently duplicate patterns on the board. My approach now has been to lay everything out by hand, its time consuming and you make mistakes. I am going to try the duplicate function in pcbnew
  • How to duplicate complete board lay-outs. For example if i first make a schematic of 2 parts,
    lay them out by hand in pcbnew. Then duplicate them in pcbnew. The duplicate them in the schematic and when i update the netlist pcbnew recognizes the duplicated parts. Does it work that way? Is there any other way around that?

Lots of stuff to learn still but i am glad to be through the initial frustration fase where nothing i want to do works. It’s really cool to draw something, order it and then actually have it.

Last question is, i don’t understand forums. Apparently i have been responding to paul but not making general posts in this thread. I hope this is a normal post.

24

Just use oval pads. (And some characters to fullfill the damned 20 characters limit…)

25

Your screenshot looks like the layout would be easiest to make with a User Grid. Define the horizontal vertical grid pitch so that it’s the distance between two footprints. When you move footprints they will snap to their places.

“Create Array” might also be useful, but then you wouldn’t have different reference designators unless you change them manually.

“Duplicating layouts” is a more complex question. You can look into for example the Replicate Layout action plugin:

But you need to use hierarchical sheets for that. Hierarchical sheets can duplicate schematics which is then reflected in the board, but duplicating the exact layout (relative positions of the footprints of duplicated sections) needs either a script plugin or manual labor.

26

What do you mean by this?

27

Well known (for regular forum users) annoying limit in the forum software or settings, you can’t reply without writing more than 19 characters even though the answer is shorter. Now I see that the rant can be seen as part of my answer… sorry for that.

28

ah got it :stuck_out_tongue:

29

I have been running into some what seems like bugs in kicad. It crashes quite often i have to say, i’ve got it on my desktop and my laptop and on both it has crashed quite a few times.

Now there is a problem that has cost me a lot of time. I’ve had it twice now that i can’t connect components that are connected in the schematic and have the same netname. The first time it took me 3 hours of selfdoubt and messing around until i tried rebooting kicad and the problem was gone. Just now i have had the same problem where i can’t connect 2 components together, i saved, rebooted kicad and all was fine.

I’ve added my project file, i’m pretty sure all is legit. PCB_Slot_V1.zip (213.4 KB)

30

I know this is offtopic but it kind of fits:

It is something that can be set by the admins i think. It however makes sense to have some limit. The idea is to discourage people from giving single word answers like agree, thanks, … as most of them can be made by clicking the like button.

If i have a short answer to make i simply add a lot of dots or minus/underline signs or even a smiley. (depending on circumstance)

31

Report crashes over on the bugtracker please.

That would also be a serious issue that should be reported.
Please include the version info as found in help->about->copy version info