Yup spot on. Except then I forget about it and clean the directories out. I'm an idiot sometimes.
Hah! Baby steps for me but at least I’m up off my face for now. I think I succeeded in generating a library part for the Omten 1217 switch which I’ll be adding to the bottom of a triple 16650 2S3P carrier for a mag mod. The switch will be soldered to the bottom of the neg end pcb As with the BTU Shocker. The top end pcb will have both + and - pads for connecting to the driver.
Next noob question: What do I need in the lower battery board schematic besides the switch and what do you put in a schematic that has no parts like the top end pcb?
Nothing. You only put what you need. You can theoretically create a board with no schematic at all. I treat Eagle like Paint almost. If no parts are present you need to manually make your traces. You can do this with the 'wire' tool, or even using polygons, the poly command and so on. Run wild!
WEEEE!
edit- time for some sleep. :weary:
You can make library parts for simple stuff like spring/brass button pads, via’s and header pins, that way you have a sch file even for simple stuff like contact boards.
I have library parts for all that kind of stuff, PM me your email and I’ll send you my .lbr for that.
Thanks, can you share them in the Eagle Libraries thread for everyone?
edit maybe a Dropbox account is needed to do that.
oh yeah, that’s how I tweaked TexasPyro’s board, it was just the .brd file, and I really like the poly command and it’s ability to auto route the solid pour around wires and vias…very cool
I am learning bit by bit about Eagle…and it’s not as hard as I thought it would be, still an amateur compared to most
I keep seeing way to import eagle components from PDF’s, well have to convert the PDF to something, then import that something into eagle
and others
I have been finding all the .lbr files I can find and getting the ones that most suit our needs, I have a repository already…if anyone is interested
https://www.dropbox.com/sh/i47cuo70drszxud/AACTRLd1pGuv4WKTRruFe_Cea
Oh Mattaus, I also tweaked your CAM processor to include the drills as a .TXT file and make a Milling layer .GML
It is here
https://www.dropbox.com/s/pandmdvdrr8ryaf/Matt_Gerber_Generater.cam
I add all the CAPITAL letter files generated by your CAM file to the .zip file uploaded to OSHPark and it seems to work out just fine (not like it didn’t before)
Plus I can import the files into the grbv viewer and it autodraws a 3D render without the .GML it chops some of the board
http://piratery.net/grbv/index.html
in the colors directory, I copied the OSH.lua, and renamed it to default.lua, now when I drag the gerber files over to it…viola…instant 3D rendering of the board and traces
like this
Hey now that's pretty sweet...
QUestion about the CAM generator. Why the need to add the extra layers? Purely for the 3D view? My CAM generator has always worked fine - never had any problems with boards other than my own stupid mistakes.
Started watching your tutorials today. Very easy to follow. It would have taken me a good amount of time to absorb that much material reading manuals and online guides. Another of many great contributions to the forum. Thank you Mattaus. 
There was a post someone sent to dirtyboards.com or something…they need drills in .TXT format…and just added the milling layer for the 3D thing…they aren’t needed at OSHPark but some board manufacturers use the drills in .TXT format.
I’ve found a cool little trick, you can save your preferred grid settings as a preset then simply select it with a right click.
I’m having an issue, I swapped out some CAP’s in the .sch (removed 0805’s and replaced with 0603’s) but the board wont update, it tells me
“Board and schematic not consistent!
No forward-Backannotation will be performed!
Use the ERC command to get a detailed report.”
How do I get the board to reflect the changes?
edit: I was able to swap out the parts on the board by using the replace command but still wondering why its giving me that error.
Care to share? You can tell that I have become used to a way of working and have not bothered changing out of pure laziness haha.
[quote=Cereal_killer] I'm having an issue, I swapped out some CAP's in the .sch (removed 0805's and replaced with 0603's) but the board wont update, it tells me "Board and schematic not consistent! No forward-Backannotation will be performed! Use the ERC command to get a detailed report." How do I get the board to reflect the changes? edit: I was able to swap out the parts on the board by using the replace command but still wondering why its giving me that error. [/quote]
That's odd. Whenever I remove parts from the schematic it removes them from the board, and adding new parts always puts them on the board. In fact I did it last night whilst revising my Medusa board.
Yeah pulling components from the sch will rip them off the brd, this is why using the “replace” command works so well
On the board, right click component, then use replace
I had to do that with the SOD-123’s I brain farted and put on the BLF15.17DD instead of the correct SOD-323, doh…then possibly a teeny trace extension to tie in the new pad
Hey Matt, could you go through the process of adding a library part again only this time include the unzipping part? The video is too quick for me to see what you are doing. Also, maybe add some instruction on editing an existing library part.
As in another video? Can do when I have time. But if in text...
Adding new library from a zip package:
- Download the part from where-ever (e14 for example).
- Unzip the entire contents to a temporary folder (I use the desktop)
- In Eagle go File > New > Library
- In the new window select File > Execute Script...
- In the window find unzipped contents you extracted earlier, and inside there should be a file name end with '.scr'. Open this.
- The window will now become populated. If you like you can check through the package, symbol, and device views to ensure its the right part.
- Once you're happy, click File > Save As... and save the file into your desired library parts location. Make sure you use an appropriate or easily recognizable name. Saving it as it's manufacturer part number is pretty much useless most of the time because you may end up with 'ERJ-B1AJ101U@E' when in reality 'Resistor 2010 Wide' is much more appropriate 
Editing an existing part:
- Open the existing part via File > Open > Library
- Click on the Device view
- Write down all the connections before you do this. Click the 'Connect' button (bottom right) and in the window that opens hit 'Disconnect' until there is nothing left under the 'Connection' tab. Alternatively if you know exactly what pad/pin combo you want to change you only need to disassociate those items, not everything.
- You can now edit the symbol and package to your hearts content. Just remember to name any pad or pin changes that you alter or remove as you go. I can't really go too in depth at this part as it really depends on what you're changing and how dramatically you're changing it.
- Once you're done with your edits go back to the Device view, and again click the 'Connect' button. Connect the appropriate pins and pads back together.
- File > Save As... if you want to create a new part and leave the existing part.
- File > Save if you're modifying an existing part.
If more detail is needed please ask :)
- Matt
once you have the settings how you want you right-click the grid icon (on my screen directly above the i button) and go down to the bottom to “New…”
A pop-up asking “Alias for current grid settings” will show up, name it there, it will then be at the top when you first right-click the icon for all your boards.
You can do the same thing in the .sch.
Not finished and already needs changes but here is my first effort.
Top
Bottom.
Anyone care to reveal how to make tented vias?
What is that about a 35mm driver? It looks good, that’s it for? What’s going on with that giant via in the middle?
To mask the specific via’s right click, go to properties and check the stop box. To remove the mask on all via’s go to DRC, go the the masks tab at the top and enter 50mil as the limit (bottom box going from memory).
Also is that a 13A-SSU? It looks a little wide (like it might be a 208mil).
How many do you want tented? You can right click them individually and uncheck “stop” or you can adjust your design rules to effect all vias below a size you choose.
What is the purpose of the SOT-89 chip in the VIN line, marked LD2981?