plated slots ... again - Page 1
Forum section: electronics / general

author: djacobow
author_rank: Super Contributor
timestamp: March 22, 2017, 02:40:03 am
content: So, this is, I think a perennial topic, and I just want to make sure I understand the right answer, as there seems to be a lot of variation of expectations out there. For example, OSH Park has guidance that can be summarized as "follow these steps ... which 'usually' work." (http://docs.oshpark.com/submitting-orders/cutouts-and-slots/)What is the state-of-the-art in plated slots for people who are using your basic bargain basic Cheap Chinese PCB House? I've had really good experience with Seeed Studio up until now and will continue with them if they can do this properly.Here's my design right now. the larger slots in the upper left are for 45A Anderson PowerPoles. OSH Park recommend just using large holes, which I think will not be sufficiently mechanically secure.

author: djacobow
author_rank: Super Contributor
timestamp: March 22, 2017, 03:41:12 am
content: Following up my own question... a further complication is that the OSH instructions tell you to use the board layer to draw out the routed area. But if I do that, Diptrace won't allow a flooded fill, which I very much want, as these are high current traces.Not sure how to get around that right.Other threads seem to indicate that setting the whole to "oval" (yes, they're not really oval) and sending it out just like can work fine, no fuss or muss, at least at some places, like Elecraft:https://www.eevblog.com/forum/manufacture/can-elecrow-do-oval-(plated)-holes/When I load my gerbs into an online gerb viewer, like at OSH Park, or Seeed, or gerber-viewer.com, I only see the pilot holes for the slotted part. However, the NC drill file does show the extra x,y pair for the slot like in the thread in the link above.Hmm.

author: tycz
author_rank: Regular Contributor
timestamp: March 22, 2017, 04:24:01 am
content: The way I've always done it is to draw the slots onto the board layer as the article from OSH Park describes. I've had no problems at all with communicating plated slots, non-plated slots, and v-score this way. If it looks confusing to me I make a separate drawing to show what is what, but this isn't necessary for something simple like your slots in component pads.I've been mostly using Seeed Studio for my prototypes ever since they started offering the service. I've attached a photo of a little panel made with their 100x150mm service last year. It features plated and non-plated slots as well as v-score.If you have trouble drawing on the board outline layer for some reason, you can probably draw the slots on another layer and combine it with the board outline when generating the Gerber (all pcb design software I've used has had this feature). I'd be wary of trying to mis-use the drill file to communicate router cuts. To me it sounds like it could have your slots turned into single holes by mistake of the cam engineer.

author: DerekG
author_rank: Frequent Contributor
timestamp: March 22, 2017, 05:48:03 am
content: Quote from: djacobow on March 22, 2017, 03:41:12 amAs I understand it:There is no point trying to flood it as the board is actually going to be cut away.You can draw an oval board cutout by:From the 2nd to top ribbon menu, selectBoard Cutoutfrom the drop down list.then select the shape type (3 icons to the left of the board layer drop down list where you chose Board Cutout). I suggest choosingFilled EllipseThis is still shown as a routed ellipse on the board but point out to the board shop that it is being fully cut out.HOWEVER:The better way to do it is to place a plated elliptical hole. To do this simply place a pad on the board, then double click on it & change the parameters to:Shape = EllipseHole Shape = OvalThen input the dimensions for the hole's width & height.This hole will be plated through which will give you the extra current carrying capacity you are looking for.PS: By the way, a nice board designed in Diptrace. This software package just gets better every year now

author: djacobow
author_rank: Super Contributor
timestamp: March 22, 2017, 04:06:36 pm
content: Quote from: DerekG on March 22, 2017, 05:48:03 amI probably wasn't clear. I just want big fat polygon traces from these pads to the other parts of the circuit, so I typically draw a polygon and let it fill. This works on normal pads, and though it makes soldering much harder, I turn off spokes. I just noticed that when I tried to draw little board cutouts inside the pads, the polygons somehow wouldn't fill properly. Maybe this is user error and I need to noodle with it some more.Quote from: DerekG on March 22, 2017, 05:48:03 amGreat! This is actually exactly what I am doing! It definitely seems to be how the tool is supposed to be used and is perfectly intuitive.What I am noticing is that when you do this in Diptrace, the way this is actually manifest in the output is not in the gerbs, but in the drill file. The gerbs do not show the slots in the board outline layer or any layer for that matter. The drill file instead shows a little linear path for the slotted cuts. If you open the gerbs + drill file in any of the viewers, you won't see these slots, as it appears that the viewers only deal with the initial point in the drill file. That makes me a bit nervous.But, if you say that you use Seeed and normally just let Diptrace "oval pad" do its thing, and it all works out, that makes me happy!Quote from: DerekG on March 22, 2017, 05:48:03 amThank you. I like Diptrace, too. I think it is the PCB tool out there that seems the least like a wrestling match to use.I've got a board out for fab right now and am looking forward to bringing it up. It is designed using screw connection terminations, but after I bring it up and deal with the inevitable mistakes, I'll spin it again and switch to the slots + powerpoles. I also did the first board is SMD, but the one pictured is 100% through-hole, as I plan to provide it as a kit to some friends who will not touch SMD. :-)

author: djacobow
author_rank: Super Contributor
timestamp: March 22, 2017, 07:16:25 pm
content: I keep following up my own posts, but I guess that's life.Through digging, I think I have determined that when you use oval pads, Diptrace uses the "G85" command in the Excellon drill file to create the routes. This is a supported, normal think in a drill file, and most fabs should handle it no problem. That OSH Park makes the point saying that is _not_ supported, I think, makes them the outlier.

author: PCB.Wiz
author_rank: Super Contributor
timestamp: May 03, 2017, 03:57:46 am
content: Quote from: djacobow on March 22, 2017, 04:06:36 pmWhich Viewers did you try ?It is normal for the Gerbers to not show the slots, but when you load Drill info, the slots should show in any good viewer.eg When I try this inKiCADs GerbView, slots show 'as expected', as slots of the drill width.GerbView seems to have an unusual graphical Colour based OR with no 'in front' control, so load drill first, then load one gerber layer, & fiddle with the colours as you add more layers.

author: djacobow
author_rank: Super Contributor
timestamp: September 13, 2017, 04:37:37 pm
content: Just to follow up this thread again, I have made more than one board with oval holes using Seeed Studio, and they've all come out exactly as intended.The whole business of drawing a slot on the cutout layer is crazy junk. The NC drill command G85 is designed for milled holes and it works as intended. In Diptrace, this is what you get if you ask for an oval hole.The outlier is OSH Park which for whatever reason cannot get their act together to support a modern drill file (or they weaselly imply that it will probably work, but they can't guarantee anything), and they offer a nonsense alternative of drawing the slots directly that requires turning off or ignoring DRC checking for copper-to-edge.