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?
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.
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.
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.
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)
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)
KiCad does not allow you to violate the design rule check by default. If you did not setup the rules correctly then you might not be able to create your pcb as you want it to be. (The DRC rules should be setup to fit your manufacturer. The default rules are a bit conservative and might therefore be too restrictive.)
I’ve tried a few designs with kicad now and got the following problem. When i make a copper pour it doesn’t fill, even when pressing the B button or the button on the left of the screen. When i check it on gerberviewer it doesn’t show up either. It does show a dotted line indicating there is a pour. I have also given the pour the correct netname. I dont know what i’m doing wrong here.
The idea of this pcb is that the frontmask is of so i can solder additional copper on there if needed. On the bottom i have created extra an extra pour to minimise the resistance of the pcb, and i have added plenty of via’s to get maximum conductivity. On the bottom is the pour that is not working.
just to clarify, a copper pour is not the same as a track? In eagle you dont have to for example connect a groundpin to a groundplane if the part is in a pour. Do you need to draw tracks through the pour? I’m confused about the exact application of the pour. You can connect tracks through a pour, and if they are all on the same net, why would a via not connect through the pour to a track?
Kicad has two ways to create vias. One is using the track tool. The other way is the add via button. The later is intended for connecting two zones of the same net with each other. (Stitching vias.) The other requires the via to be connected to a track.
Kicad selects the net of every element automatically when creating connectivity information. Eagle has nets explisitly assigned to elements at the time of creating them. Neither way is truly superior. Each has its benefits and drawbacks. And of course some actions require different interactions (meaning interface knowledge of one tool might stand in the way of effective use of the other.)
I opened Tom’s project and the copper pour would not fill, which I found strange.
As a test I added a small copper zone of my own, also on the /common net, and then the whole area filled.
Then I noticed that none of the via’s are aligned with the center of the PCB tracks they connect to.
KiCad really likes to have centers of things aligned with each other.
For a zone area to get filled it needs at least one solid connection to a pin, so if you draw even a single track from a center of one of the slots to within a copper zone then the zone connects with a pin and it gets filled. This is quite normal operation of KiCad. Within a normal PCB, unconnected copper areas within a zone do not get filled.
This is a quite difficult PCB design. Not because the PCB itself is complicated, but because the way it is drawn is “different” from a “normal” PCB. As a result, things that are logical and self explanatory in a regular design become puzzling. Even so, this PCB is pretty trivial to design for someone with KiCad experience, but as a first design with KiCad this adds to the confusion.
Why have you abandoned my tip in post #11 of making a symbol for your fuses?
Why have you drawn the via’s on a different grid as the slots?
(If you draw them on the same grid, they get automatically aligned with the tracks).
Your schematic also needs “resqueing” when I open it it KiCad V5.0.2, and you are apparently still using KiCad V4, which makes exchanging data more difficult. Were you able to open my schematic / PCB with the Fuse component? Just a few days ago KiCad V5.1 got released. Please consider updating Kicad.
When i connect 1 track directly to the via it works.
Makes sense, when it is not connected why would there be a copper pour? Good point!
It really is. For me it’s important to fully understand the fundamentals of a program because i tend to ■■■■ up a lot and spent hours trying to fix something i don’t fully understand. The upside is that i have tried so many features of this program that it really helps me fully utilize the software.
I have a design with the fuses but it got quite small in the middle since the fuse needed pretty large pads because you want to lay fat tracks to it. I might bring them back in the future since it does look good but manually drawing tracks is a lot faster than placing all those fuses by hand on the board on the same spot.
I just placed them pretty random on there because i assumed that anywhere on the pour would be fine. The reason that i have a track from the top slot to the bottom slot is because it saves me one click.
I run 5.1.0, just downloaded it yesterday on my desktop, dont understand how the file could be wrong…
