I want a special thru hole pad for soldering .05" ribbon cable right to the pcb.
Such a hole doesn't seem to exist so I tried making one, it failed.
The hole filled in with copper and wasn't as big as I set the diam for initially.
It was an elongated .025 diam via with a .02 hole size, prolly couldn't get 30awg wire in the hole the fab sent me..
Anyway the next pcb was .03 diam elongated via with .027 size hole and it works ok, but there is not as much mask between the pads as i'd like when I space them .05" apart.
Also, the hole size shrinks when you view it in layout and on the pcb the fab sends back and i'd like it to be bigger.
I think that's where the problem is.
Maybe there's a limit on annular ring that's causing it?
If its not doable in Eagle i'd be glad to try a different CAD program that can.
Why not use SMD pads?
Such small annular rings seems like asking for trouble.
Use a transition connector
Many reasons not to, first cost, even at $.50 it would be the most expensive part on the board!
Second sometimes I only want to solder a set of 4 conductors to my smallest boards.
Lastly space, not necessarily on the board's real estate, in the case of my larger boards, but inside the electronics these boards are being added to. Most of my work is with old video game consoles, some like the Atari JR have near zero extra room.
Why not use SMD pads?
I've thought about it, but some of my boards are DIY kit type projects and it would be nice to be able to solder on the ribbon cable much like a through hole component, insert wires through holes, bend the leads on the bottom so its held in place, and solder it up.
The drill size specified in CAD may be interpreted by the PCB mfg as literal drill size -or- finished hole size. Make sure you know what it means to them. You certainly can do 50 mil spaced pads in Eagle. Here is part of a board I just got from seeed with 50 mil and 100 mil 6 pin pads...
The drill size specified in CAD may be interpreted by the PCB mfg as literal drill size -or- finished hole size. Make sure you know what it means to them.
I still don't think its the PCB mfg, the pad immediately looks different in the layout editor than it did in the library editor.
That's why I think its some setting in the DRU, which was made up by the guy who runs the group buy I use, used to be Dorkbot, now OSHPark.
But I will ask about the drill size meaning to the fab.
You certainly can do 50 mil spaced pads in Eagle. Here is part of a board I just got from seeed with 50 mil and 100 mil 6 pin pads...
Yes i'm already experimenting with 50 mil spaced via's, its just the via's ID that i'm having trouble nailing down.
Can you share that 50mil 6 hole 'device'? Maybe I can just modify that...
Thanks a bunch oPossum!
I also posted this at Eagle Central forum and still no responses after 70 views...
Here are the
board and library files.
I have not had any boards with that 6 pin connector made by OSH Park, but I have had other boards with 0.6 mm (0.023622 in) drill made by them.
On the boards made by OSH Park, I can easily put a 0.5 mm dia component lead in to a via that used a 0.6 mm drill
Thanks for sharing oPossum!
I think i've finally found the settings that were messing with my original thru hole pad.
In the DRC, restring tab, if I change Pads's Mins and %s to 1 then the specs come out as I intended.
However, I have no idea if the fab will tolerate those specs.
It also changed the thru hole pads on other components too though, kinda wish it didn't...
Could be worth a go...
Have you checked the sizes in the NC drill data?
Also, some manufacturers have different toleances for via holes and normal holes.
For example, a big european pooling PCB manufacturer (EuroCircuits) considers holes < 0.45 mm (18mil) to be via holes.
Normal holes have a tolerance of +/- 0.1mm (4mil), while their vias have a tolerance of +0.1/-0.3mm.
In addition, they use metric drills in 0.05mm steps, which are selected by rounding the NC drill size to the nearest 0.05 value.
Suppose there's a hole of 0.474mm (19mil), it gets rounded down to 0.45mm, which is considered a via, which can have a -0.3mm tolerance.
So the final hole can become 0.15mm, and still be within production spec!
Long story short: check the design specification and tolerances of your PCB supplier.
Long story short: check the design specification and tolerances of your PCB supplier.
Good info, but I don't think OSH Park (Dorkbot) has released the info on who they use, though I assume its in Portland, OR.