I wouldn't add the plating bar, let the fab do it.
The connector should be made as one Part. Whether you do it as one gate (all pins), two gates (one for top pins and one for bottom pins), or as individual gates (one per pin) is up to you.
For the Decal, for a dual sided connector, most likely you will place separate top and bottom surface-only pins.
If it's a double-sided but same pin number connector (the kind you don't hardly see anymore - usually with a built-in via at the top), just build like a TH part, with the surface pins offset and the inner layer pads as rounds.
Assuming it's properly built as one part, you need to pin it out per the applicable standard or maybe the data sheet for the connector it plugs in to.
If you don't have a standard or connector to go by, I would pin odd numbers on Primary (aka Top) side, even on Secondary (aka Bottom) side - but I would double-check that that is correct or acceptable with my engineer.
I see, OK good points, Another question though addign to what was said.
Haven't used fingers in awhiel & was always used to supplying plate bar, btu not does make life easier here.
OK if we go down the path of making it two separate parts one top & one bottom, (not tied together with vias)
I guess I am a little confused with the terminology with repsect to how PADS defines pads.
There are two possibilities I see for something other than Top or internal pads, they are "Opposite Side" & "Bottom"
what in earth is the difference? Would it then be better to create two parts both top side SMT, one with pins 1-61 & the other with pins 62-122 (that is the way they will be numbered)
Then push the 62-122 to be a bottom side part in PCB.
Or what pad choice should I use fi I make th esecond decal using pads to be on the Bottom? Use Bottom or Opposite Side????
Don't worry about the plating bar, it wouldn't be surprising if probably 90% the time, the fab ripped yours out an replaced it with something they liked better anyway.
Build the Decal as one part, with pins 1-61 on the Primary (aka Top) side, with 0 drill size, uncheck the "Plated" box, with Inner and Secondary/Bottom/Opposite pads as 0 round.
Add pins 62-122 on the Secondary (Bottom aka Opposite) side, with 0 drill size, uncheck the "Plated" box, with Primary/Top and Inner pads as 0 round.
Don't forget to add your soldermask blocks.
If you want, send me a pdf of the documentation for your edge connector, and I'll build you one, look at my profile for an email address. That way you can see how it's done.
Put something like "Gold Edge Finger Connector" as the subject and let me know what version you need the data to be in.
First thanks very much for the offer to build it.
I kind of have it pretty much done. But still wonder about pad options?
Again one question I had was about terminology I guess if you will.
What is the difference if any with respect to how PADS handles it in a PCB
Seems there are two options for top & bottom to define a pad stack?
For Top you have "Top" & "Mounted Side"
then of course "Bottom" & "Opposite Side"
I think it may handle it differently depending on which is used here?
Or do they both sync up to what ever the layer definitions are for top & bottom (i.e. layer #) once in Layout.
Basically what is the meaning of having these two options? Or was it just something left over from old versions of PADS
or is there a real meaining to using one vs the other?
I'm just a little confused on these items.
Also for smt pads wouldn'y these also want to be left as plated checked? I see many examples of this in PADS libs
and other designer here has left some as plated checked and some not. Is there really any difference here with SMT pads?
I really have to leave it as two part/decals becuase of the way the schematic symbols were done in Oracd can't change that now.
Of course on solder mask clear.
Not a problem on the part, that is a standing offer BTW. As long as you (or others) don't go nuts asking.
On terminology: In the database, the system default layer names are Top and Bottom, then you have however many inner layers there are, if any. Now, you can rename these to whatever you want, hence my calling them Primary and Secondary (my personal default names).
If you just go to build a Decal in the library, the layers are called (I believe - I've changed my default layer names) <Top Side> and <Opposite Side>. Top Side = Top, Opposite Side = Bottom. As far as the Inner layers are concerned, unless you want/need to set up specific pads and things on specific layers, setting the <Inner Layer> pads will be a default for all inner layers, regardless of how many there are. You pretty much always (probably 99+% of the time) build as if the Decal is mounted on the top side. And always use the pinouts (if indicated) in the mfr data sheet.
The layers are called <Mounted Side> and <Opposite Side> in the pad stack window only. Why? Who knows? Mounted = Top, Opposite = Bottom.
Don't know why the layer names are set up that way, but consistency is definitely not one of PADS' strong points.
Now, if you go to edit a Decal from the layout editor (select the part and RMB - Edit Decal), the layer setups and names will be the same as set up in your board.
The "Plated" switch is for through-hole plated pads, thats all. Though it doesn't necessarily hurt to leave it checked, I personally don't and wouldn't ever check it for SMT pads.
And, IMHO, the supplied libraries aren't really all that great, except maybe to use as a starting point to build your own libraries. For instance, they put stuff on "All Layers", this should pretty much never happen. And their pad geometries tend to be a bit oversized (like the way-too-large default "Standard Via"). Their silk outlines and any text, including designators, tend to be too large. Plus, they don't have assembly images or use pad stack setups. Some of th emost basic schematic symbol items are, however, necessary for PADS to work correctly.
Component silk outlines and any visible attributes should go on the Top layer. Use Top Silkscreen for anything else, like text (or blocks or logos in the PCB itself). You can use Top Silkscreen layer for the part outlines and attributes, but I've found that putting them on the Top layer works best. Don't know why [shrug].
Don't know why people keep making edge finger connectors as two parts, that is NOT the right way to do it....
Yup it certainly was a little confusing why in decal editor they give you two choices for what is supposedly a top or bottom pad could be defined as?
Just doing regular smt parts you only build the top so it never came into question with PADS till I need to build a conn finger.
Yes I was trying to convince the Engineer to make one part, and just break it up into two pieces within part. That way he would have been happy too I thought?
But did not win that battle this time. It was done as two parts with of course two Ref Des so I had no choice.
Thanks very much!
This is a bit off topic but PADS now includes IPC standard libraries in the V9.3.1 download. Choose PADS Layout Extended Libraries when installing the software. The libraries are also available for download on the V9.2 download site at:
Start the download and a window with gray boxes will appear. The libraries begin at the third gray box. You do not need the LP Viewer. Just download and unzip the library files and add them into the Library List as usual.
I know about but have never used or even looked at those libraries because I already have a fairly extensive library I've built up over the years with very specific naming conventions, pad geometries, and layer and other setups. Could you send me a sample IC-type part from it? I just want to see how they compare and whether or not I may want to switch or use parts of that library.