Methods for making a PCB mounting hole in Altium Designer - Page 1
Forum section: electronics / general

author: rzeznicc
author_rank: Contributor
timestamp: October 13, 2015, 05:23:04 pm
content: I want to make a mounting hole of 2.4 mm diameter for a M2 screw.I have found three methods used to make mounting holes, none of them is satisfying to me:[SEE ATTACHED IMAGE]METHOD 1.Place a pad on the PCB, set hole size to 2.4mm and annular ring size to less than 2.4mm.problems:-if you set annular ring to 0mm you will get manufacturer errors, as you will get a virtual 0mm point surrounded by soldermask clearance ring in gerber files-if you set annular ring to 2.4mm, same as hole size, you will get a hole with soldermask clearance ring (makes the soldermask susceptible to peeling with screw torque)-using a PCB template rules fromhttp://www.eurocircuits.com/Altium-Designer-templates-with-Eurocircuits-design-rules(my fabricator of choice) for Class 6C - 2 layer - 1.55 mm i get an design rule error saying "Hole Size Constraint (Min=0.25mm) (Max=2mm) (All) 4" which means they do holes up to 2mm. Clearly that can not include routing and cutouts. What gives? How do I make a larger hole then?METHOD 2.Create a PCB library footprint for the hole (also from a pad). The bonus is that you can add a 3d model of the screw [SEE ATTACHED IMAGE], which makes it much nicer for the final board 3D render. You could add a 3D model to each screw hole in the METHOD 1, but you would have to align it one by one, and here its all pre-done.problems:-this METHOD gives errors when processing the PCB as it is an object in the PCB not referenced in the schematic-I also tried creating a schematic library part, and adding the above mentioned PCB library footprint(pad) and 3D model to it - now I had to hide unnecessary bloat items in the schematic-same Eurocircuits fabricator problem as aboveMETHOD 3.Place a primitive/polygon on a mechanical layer and perform [SEE ATTACHED IMAGE] TOOLS>CONVERT>CREATE BOARD CUTOUT FROM SELECTED PRIMITIVESproblems:-there is no nice screw model representation like in METHOD 2-will it generate proper gerber drill data to the manufacturer? I am afraid it will be just a random cutout that they will have to route in some expensive way-I don't get the nice dimension outlines: screw head (grey circle) and screw clearance (green circle)-it will not make a plated hole: I have read that its best to keep all holes plated, even mounting ones, as it reduces the tooling overhead. Is that true?I am offering ten(10) engineer-nice-person points for an elegant solution to this trivial problem!cheers

author: Batang
author_rank: Regular Contributor
timestamp: October 13, 2015, 05:43:54 pm
content: I have always used method 1 and set the annular ring size to the screw head size.The benefits are stronger mounting point (i.e. copper and plating for screw head and or nut).If I want a nice 3D screw I add them manuallyTypically only 4 mounting holes, not a panties bunching problem.Cheers.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: October 13, 2015, 07:16:47 pm
content: If you want an unplated hole, I suggest using pads (or proper components with footprints, containing a pad of the same description), setting the copper pad maybe 10 mil below the hole size. No particular reason, it just looks okay that way.If you can't drill holes that big (I haven't seen a single manufacturer that couldn't do >3mm holes..!?), then (technically speaking) you must use a route, which will have a ring (or whatever shape) in the Keep-Out Layer. You should probably also add a Region that's tagged as "board cutout". Make sure the manufacturer understands they are holes/cutouts, in case it doesn't come through quite right. Provide a mechanical drawing labeling the positions and dimensions.Routes can also be plated, but check if that's extra or anything. Do expect worse tolerances.Tim

author: free_electron
author_rank: Super Contributor
timestamp: October 13, 2015, 07:53:12 pm
content: NON-ISSUEplace a pad with pad diameter and hole diameter set to 2.4mm. Uncheck the 'plated' checkbox.send data to boardhouse.They will detect unplated holes in the Gerber data and automatically convert these to post plate step. since the size is larger than 2mm it will be automatically converted to a milling step.all the boardhouses these days use either Ucamco or Genesys Frontline as data intake software. These tools do this conversion in one shot.Almost nobody drills larger than 2mm : they switch to router bits as these have a longer lifespan.if you set mounting holes to unplated they simply get milled during board contour milling so you incur no additional processing step on the drill ( board fabs use different machines for drilling and for milling . milling plated holes means the board needs to visit two machines prior to plating.and the mill to do contour routing. unplated mounting holes means no visit to the mill prior to plating so you save a production step (unless you have plated slots in the board in which case it doesn't matter at all)so , maky your life simple and simply place a pad with pad diameter and drill diameter set to the same value and 'plated' unchecked.done.

author: ajb
author_rank: Super Contributor
timestamp: October 13, 2015, 08:10:37 pm
content: What he said ^^^. You might still see some low cost fabs that don't do unplated holes and only do outline milling, but a fab that cheap probably won't complain about the annular ring and will just run it as you send it.As far as handling the mounting holes in your design, I prefer to design mounting holes as components with appropriate clearance for the mating hardware marked out and link them to schematic symbols. That makes it easy to link the holes to a net if necessary and ensure that the net assignment is preserved even if you have to update from library. It also makes it easy to have a few different versions with/without models of the hardware if you care to show that in your renders.Having a couple of mounting hole symbols in your schematic really isn't that big a deal. You can shove them onto a separate mechanical sheet if they really bother you. I seem to recall that the documentation for some of Atmel's dev boards even have the rubber feet and barcode stickers called out on one of the schematic sheets.

author: rzeznicc
author_rank: Contributor
timestamp: October 13, 2015, 10:00:43 pm
content: thank you everyone for your repliesQuote from: free_electron on October 13, 2015, 07:53:12 pmI'll do that from now on, however, this method adds to the soldermask layers, as you can see the outer ring in the attached image. I guess I will have to use pad diameter smaller just enough than the hole size for it not to show (soldermask is still there though).The reason I was hesitant about it, is that it leaves all this unwanted junk in gerbers and makes the fabricator do some second guessing based on best practice, to which I thought, surely there must be a more elegant solution given Altium's Designer sophistication and its userbase expertise (there is no irony here, Im a newbie myself, as is evident).thanks again

author: rzeznicc
author_rank: Contributor
timestamp: October 14, 2015, 11:05:20 am
content: UPDATE: I have received reply from Eurocircuits:Eurocircuits can only provide in chamfering for M3 screws, as you can read here :http://www.eurocircuits.com/Chamfered-mechanical-holes-or-countersunk-holes'In some applications it is important to sink the heads of fixing screws into the board when no protrusion on the board surface is allowed. This technique is called chamfering. It is not so obvious to do this on epoxy material but we can do it for the standard screws M3.The chamfering needs to be checked in the order details and the holes need to be clearly marked and specified in your data.'Holes, larger than 2 mm are milled and not drilled, so that is not really the problem.

author: free_electron
author_rank: Super Contributor
timestamp: October 14, 2015, 12:40:46 pm
content: If you want the soldermask opened simply check the box to override soldermask and type in the size of the opening over the pad.Chamfering is indeed a different animal ... I would not do that in boards unless they are very thick , like 2.4 mm and above. And even then .. Simply press a PEM it in the board and screw it from the back side (no ,it's not what you think it is. Perverts !)

author: Jeroen3
author_rank: Super Contributor
timestamp: October 14, 2015, 01:49:47 pm
content: Eagle has a mounting holes library. You add the holes to the schematic, with a note to the specific board size and enclosure used.What's preventing you from doing exactly that? Stubbornness?And, a hole is not a pad. There is no annular ring, it's actually a hole, with some keepout/restrict layers and silk screen.

author: free_electron
author_rank: Super Contributor
timestamp: October 14, 2015, 01:57:38 pm
content: here ya go : hole with solder mask clearing. you can even set different clearance for top and bottom by unlinking the top and bottom ( the vertical 'chain' button next to the clearances )

author: rzeznicc
author_rank: Contributor
timestamp: October 14, 2015, 03:42:10 pm
content: Quote from: free_electron on October 14, 2015, 01:57:38 pmthanks! That's an option I have overlooked. Now its simple and elegant. 10 points are yoursQuote from: Jeroen3 on October 14, 2015, 01:49:47 pmUsing Altium Designer? As this subforum name and topic name indicate?

author: free_electron
author_rank: Super Contributor
timestamp: October 14, 2015, 04:39:16 pm
content: Quote from: rzeznicc on October 14, 2015, 03:42:10 pmyou have to remember 1 thing about altium : if something takes more than 3 keystrokes or mouse clicks : you are doing it wrong...Granted, it is not always obvious to figure out, because the tool simply has so many functions and features. And, every update brings in additional stuff ... so it is an endless learning process.

author: Jeroen3
author_rank: Super Contributor
timestamp: October 14, 2015, 05:23:34 pm
content: Yes. I very well noticed that. But now the mounting holes are still technically a pad. Which is incorrect and can lead to errors and confusion with future designers.I just referred to eagle because there it is done in a way that is easy to share to keep a consistent type of mounting pad over all designs in the company.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: October 14, 2015, 07:09:45 pm
content: My standard approach:The schematic component has basically no data, and if you use Assembly Variants, they should be tagged as Not Fitted (if you'd ever fit anything, e.g. screws, standoffs, etc., that should be assigned on a separate mechanical BOM/drawing).This is good to avoid inconsistency between SCH and PCB, especially if electrical connection is needed (and hey, more grounding the better, as far as I'm concerned).Tim

author: free_electron
author_rank: Super Contributor
timestamp: October 14, 2015, 07:23:51 pm
content: Thats how i do it as well : creat library symbol. For the schematic set the type to no bom then it does not appear in the bom

author: Bud
author_rank: Super Contributor
timestamp: October 14, 2015, 10:02:47 pm
content: So if it is not plated, you still able to connect the symbol to Ground in the schematic?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: October 16, 2015, 12:05:44 am
content: Well, if it's unplated, you'd presumably leave the pin off the schematic symbol...You can actually connect unplated pads. For instance, you can have the pads on top and bottom, but no barrel. (Or whatever shape on each layer, since they can be specified separately.) Of course, if the pads are smaller than the hole, so that there's no way to connect them... good luck with that.Tim

author: free_electron
author_rank: Super Contributor
timestamp: October 16, 2015, 01:57:37 am
content: Quote from: Bud on October 14, 2015, 10:02:47 pmif it's not plated there is no copper . duh !

author: Bud
author_rank: Super Contributor
timestamp: October 16, 2015, 02:14:55 am
content: So the compiler would not generate a "unconnected <whatever>" warning ?

author: DutchGert
author_rank: Frequent Contributor
timestamp: October 22, 2015, 07:49:35 pm
content: Quote from: Bud on October 16, 2015, 02:14:55 amTrue, u could create a schematic symbole for a hole (correct way to do it in my opinion) but if the footrpint of that holes specifies it as a NPTH u could indeed end up connecting something to a none plated hole without getting an compile or DRC error in Altium.Ofcourse it's common sense not to do this but still.