I was so excited in completing my first board (2 layer), that I missed an important detail. All my components are through hole - resistors, capacitors, IC’s. I also have a generic 25-pin 0.1" single row header, and I located a footprint somewhere to use for it. As a newbie, it did not occur to me that there were some parameters I needed to check, nor did I notice that solder mask was covering the pads for the header when examining the Gerber files. The first error is understandable, the second was a lack of paying attention.
What I found was that in the pad parameters, all the other components have the F.Mask and B.Mask “Technical” flags set. But the header pads did not, and as a result the boards I will be receiving will have a coating on the pads of the header. I assume I can scrape off the coating and hopefully they will take solder, which I am not thrilled about but lesson learned - but my main question is will the pads be plated through?
If there is a solid copper pad in the copper layer (gerber) and a drill mark in the drill file inside that pad area, yes, it will be plated through.
EDIT: on second though, if it’s covered with mask, the mask may have gone to the hole. Then it has to be scraped off from there, too.
Depending on your manufacturer and the state of your order it may still be possible to send them a message, asking to uncover the THT pads. Sometimes they notice these kind of things and ask you. Sometimes they fix it without asking (unfortunately, because they don’t always guess correctly.
There is no need to guess the plating of the holes. The KiCad drill file, either Gerber or NC, can contain attributes that indicate whether the holes are plated or not.
They can also indicate whether it is a via or a TH component hole. This may not be correct if the footprint is rotten. If, however, it is indicated as a TH component chances are the fabricator will notice this in CAM, and guess it is not right, and fix it. (With or without asking, depending on his style and whether he has spare time on his hands for such things.)
Can you share your drill file?
Remember, tented vias are also plated holes that are covered in mask, so having a plated through hole covered in mask isn’t unusual. The vendor may or may not catch it (depending on if they care to recognize the hole pattern as a header strip), but there is no problem manufacturing a board with mask covered plated holes. (The mask process happens after hole plating.)
KiCad Copper layer files do or can contain attributes that indicate whether pads are TH component pads or via pads. (I suppose one can turn this off, but why anyone in his right mind would do that, I would not know.)
The question is whether the pads are correctly tagged, taking into account that there are things wrong with the component. Maybe not. Can you share the component side copper layer? The fabricator will normally check whether the TH component pads are free of mask. If the attribute is correct, you should be OK. (If you have turned off including these attributes, well, good luck)
We can’t see what you did, If you upload the Gerber or kicad_pcb file someone would have the change to look at it.
If you did it wrong or think you did it wrong, ask the manufacturer to not start producing it and send him to correct file when you have them. But do that fast, they can’t change it anymore when you are too late. And you may pay extra when they have more work.
In case you get the PCB with too much solder, you can scrape the solder off with a scalpel and you can still solder them. I did that many times. I assume you didn’t order many PCBs?
Here is a picture of the attributes I am referring to in Pad Properties. On all other parts I placed, the F.Mask and B.Mask attributes for pads were checked as they are here - but they were NOT checked for the 25 pads in the footprint for the header along the bottom (and three 1 and 2-pin ones) that results in what is seen in the images on the right. Incidentally, I made my own footprint with SMD pads recently, and I was prepared when I previewed the result and the same thing happened - the x.Mask box needed to be checked for the appropriate layer for bare copper to show. I believe my main concern that the holes will not be plated through is not valid - since plating is on both sides the holes should be plated. I did not discover this for three days, so I did not attempt to contact the manufacturer…
Right. I don’t see a reason why they wouldn’t be through plated. The mask layer shouldn’t affect that at all in any way. It’s possible that they remove the mask (i.e. add graphics to the mask layer) from the holes but not from the copper pads so that the mask substance doesn’t flow to the holes. But you’ll see that later.
