Partial depth PCB holes - Page 1
Forum section: electronics / general

author: Eamonn Harter
author_rank: Newbie
timestamp: January 17, 2019, 08:53:57 pm
content: Due to space constraints on a PCB design, I have a need for partial depth holes in a 2 layer board. This would be in a 62mil thickness 2 layer board, and the finished depth of the holes would be 45mil. Each hole would be 26mil in finished diameter and centered in a pad of at least 50mil diameter. At this point, I am unsure if they could be finished with copper plating or not, but my PCB fab says that they can manufacture partial depth holes. Does anyone have experience with partial depth PCB drill holes? And how would I enter this information into Altium Designer? I could use a fabrication note, but would rather have a more solid way to enter this information directly in the Gerber and NC drill files so that the Chinese manufacturer knows exactly what to do. I read somewhere on here that you have to enter this into the PCBDOC files and it's not possible to have it in a library component.The specific component that will fit into the partial depth holes is a press-fit Mill-Max pin.

author: mrpackethead
author_rank: Super Contributor
timestamp: January 17, 2019, 09:08:39 pm
content: What you are talkign about is a 'blind' hole. This technique is often used on multilayer boards for vias, so they do not go all the way through the board. You can also have buried vias.Altium will let you set up vias that go between various layers.. However since your board is only two layers, there is only one drill pair.I have never heard ( though never asked for ) of what you are asking for.. I suspect it will be expensive, and the accuracy of the Z depth for the holes will be interesting.. It would have to be milled.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: January 17, 2019, 09:20:21 pm
content: I think in AD17+ they added blind holes as an option, without having to set up drill layer pairs? I haven't touched it so I'm not sure.Otherwise, the canonical way to represent them, in Altium, I think, would be to set inner layers, at the depth desired, and use vias on those layer pairs. You would then add a fab note that the inner layers are not to be fabbed, that they are intentionally empty, and that the design is to be fabricated as a 2-layer design with blind holes of specified depth.No, I don't think there's a streamlined way to do this. It would be nice to generate extra fab outputs, say a drill file for thru holes, a separate one for blind holes including correct depth commands, and so on; and you can probably do this, but how it's going to be represented in the EDA files, and if there are unnecessary side effects (like including layers you don't want), dunno.Ed: and yeah, for a pin like that, you'd normally have a thru hole, and that's that. Mind that the minimum depth, to the shoulder of the hole (the drill will have a conical tip, or if an end mill is used, it will have some corner radius), has to be at least the maximum length of that pin. With a tolerance of maybe 5 or 10 thou depthwise (don't expect miracles -- do check with the fab to see what their capability is), the typical hole will likely break through the other side of the board anyway. If you need a sealed hole, consider using the next size thicker PCB (typically around 0.093" / 2.4mm?), or a soldered pin.Tim

author: mikeselectricstuff
author_rank: Super Contributor
timestamp: January 17, 2019, 09:32:16 pm
content: Another way to do it is to use a special drill size, and spec it as part-drilled in the tool list.

author: Eamonn Harter
author_rank: Newbie
timestamp: January 17, 2019, 10:17:39 pm
content: Thank you all for the quick responses. I have used this same Mill-Max pin in several other designs and have always used bona fide plated through-holes that go through both layers. Alas, due to space constraints a normal plated through-hole won't work for this particular design because an SMT footprint will be immediately above the location (on the top surface) of the pins (on the bottom surface).Another option I have considered are pins that solder directly to pads on the bottom surface. I have searched the Mill-Max, Samtec, and Molex catalogs and have a few possibilities, but nothing is obvious. One option might be some type of header that is in cut tape that would be assembled by PNP. Or I guess I could load Mill-Max pins into a fixture, apply solder paste to the bottom surface pads, and then send the boards and pins through the reflow oven. For my design, the pins are in a standard DIP pattern (100mil pitch, 300mil row spacing). Does anyone have any recommendations for surface-mount contact pins?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: January 18, 2019, 02:18:34 am
content: Quote from: Eamonn Harter on January 17, 2019, 10:17:39 pmWhat do you mean contact pins -- do they press into a flexible surface? They look pretty rigid so it's hard to see what advantage this type would have over, say, standard square pin headers (which are available in standard SMT styles).For contact with rigid surfaces, there are spring-loaded (bed of nails) types available in various formats, more expensive of course, and also usually longer (taller) and maybe not in SMT at all.Alternately, there are springs in SMT and THT format, typically for pad contact, and EMI grounding. I think some are small enough that they could be placed in a row at 0.1" pitch.Tim

author: Eamonn Harter
author_rank: Newbie
timestamp: January 18, 2019, 02:54:56 am
content: By "contact pins" I am referring to standard rigid pins. The board design is a replacement for a 14 pin DIP component with two rows of pins in 0.1" pitch, 0.3" row spacing and the pins on this board would install into either a DIP socket or a 14 pin DIP target location on another PCB. The space on the top of the board is required for trace routing and SMT pads which precludes the use of normal through-holes for press-fit pin installation, so I need a way to mount pins directly on the bottom surface.As you said in your reply, standard square pin headers in SMT styles might be the solution. What would be ideal is a surface mount pin header in a plastic carrier module that has pins on 0.1" pitch and 0.3" row spacing. Does anyone here know of a source of such a part? I am going to explore the Digi-Key catalog to see if I can find a solution.

author: Kasper
author_rank: Frequent Contributor
timestamp: January 18, 2019, 05:30:44 am
content: How about quantity 2 of:SMT, 7 positions, 1 row, 0.1" pitchPlaced parallel to each other and 0.3" away from each other.https://www.digikey.ca/products/en/connectors-interconnects/rectangular-connectors-headers-male-pins/314?k=&pkeyword=&sv=0&pv88=15&sf=1&FV=1680001%2C1bf80001%2C1f140000%2C1f140003%2Cffe0013a%2C1140003&quantity=&ColumnSort=0&page=1&stock=1&pageSize=25

author: mrpackethead
author_rank: Super Contributor
timestamp: January 18, 2019, 05:51:13 am
content: threads like this are very useful.

author: martin1454
author_rank: Regular Contributor
timestamp: January 18, 2019, 07:28:25 am
content: We used partial depth hole to mount a connector intended for 1.6mm PCB to mount it to a 3mm PCB - We had to use 3mm for the stiffness, but it worked out great with the partial hole - It was done in autodesk eagle, and could not be marked in eagle it self, so it was marked in the "readme" file we gave to the fab.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: January 18, 2019, 07:32:10 am
content: Ah, IC replacement, so square header pins will blow it out (0.025" square, much thicker than an IC pin). At best, ruining a spring type socket, but not even fitting inside a machined pin socket at all.I remember Mill-Max headers available with 0.3" rows for just this purpose, but I forget if they had any with bent pins for SMT.Could also just take whatever headers and do a butt joint. Assuming you can get an iron in there under the plastic retainer strip part. This usually leaves a small fillet though, may be too weak. Or there's those headers that are DIP sized but have turret posts on the other side, often used for wired jumpers, resistor options, that sort of thing. Those turrets, SMT'd, would have okay bite, again if you can solder them.Another option, if you have the vertical height, is to build two PCBs in one. Snap them apart and slot one into the other, so the one is the connector board as it were, and the other stands up vertically, with whatever components on it. Yes, that's getting towards the "heroic" side of solutions, although not really all that bad as it's pretty easy to assemble.Tim

author: ar__systems
author_rank: Frequent Contributor
timestamp: January 18, 2019, 01:57:26 pm
content: I used partial depth routing where I needed easy depanelizing but have some interconnects going into the boards while still in panel. It is doable. Extra cost, but not terribly expensive.Although for this application I don't see the point. Just drill through.

author: mikeselectricstuff
author_rank: Super Contributor
timestamp: January 18, 2019, 02:44:49 pm
content: One minor issue that may affect cost is that mulriple PCBs are often drilled at once in a stack, so this would not be possible with partial drills.

author: Eamonn Harter
author_rank: Newbie
timestamp: January 18, 2019, 05:15:02 pm
content: I think using two rows of 7 pin surface mount headers is the best (and cheapest) solution. The only potential issue would be keeping them aligned in parallel and separated by 0.3" to replicate a 14 pin DIP package footprint. I think some of the manufacturers will make custom components, but this would probably not be cost-effective for a relatively low volume (<10,000). The link that Kasper shared was useful and has given me a few more ideas; the Mill-Max surface mount header interconnects look promising. I have always had good experiences with Mill-Max parts.It would be really nice if it was possible to assemble one of these components using a PNP machine. Assembling a handful would be no problem, but hundreds or thousands would be really difficult and time consuming to solder manually.

author: Kasper
author_rank: Frequent Contributor
timestamp: January 18, 2019, 07:50:00 pm
content: Glad you liked my link.Some of those male headers come with caps over the pins so PNP suction cup has something to grab.

author: mrpackethead
author_rank: Super Contributor
timestamp: January 18, 2019, 07:56:52 pm
content: what pins will replicate a DIP packages pins...

author: Eamonn Harter
author_rank: Newbie
timestamp: January 18, 2019, 08:45:27 pm
content: I contacted Mill-Max to hear their advice, and one of their application engineers recommended their series 150 surface mount DIP headers. It's good I contacted them because I didn't see this option in their catalog initially. I ordered a few free samples which should be here next week. And we should be able to assemble this part to our PCBs with PNP machines, so no manual soldering.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: January 18, 2019, 09:03:35 pm
content: Bingo! Thought I saw something like that beforeTim

author: mrpackethead
author_rank: Super Contributor
timestamp: January 18, 2019, 11:49:25 pm
content: Now that is pretty useful. :-)

author: mikeselectricstuff
author_rank: Super Contributor
timestamp: January 19, 2019, 11:59:26 am
content: Another solution for DIP pins :http://oshchip.org/products/Flip-Pins_Product.html

author: Doctorandus_P
author_rank: Super Contributor
timestamp: January 24, 2019, 08:41:34 am
content: Via's that go from the outer layer to the next inner layer are called "Blind Via's"."Buried vias" are via's that are inside the PCB and not visible from the outside, for example between the inner 2 layers of a 4 layer PCB before the outer 2 layers are sandwitched on."Micro Via's" are very small vias that also do not go through the whole PCB.These are (often?) not drilled, but lasered into the PCB.The inside of holes is usually coated with some conductive layer of carbon and then copper is added via electrolysis in an acid bath.Applying the carbon to blind holes can be done, but is more difficult than for through the board holes.Some of the bigger PCB manufacturers have a fair amount of information on terminology and information of the whole PCB manufacturing process.With a bit of searching there are also pretty detailed video's on Youtube.That is also where I have my info from. I am not an expert in PCB manufacturing.For example, here are some informative video's from Eurocircuits:https://www.eurocircuits.tv/category/electronic-manufacturing-technology/