X-Authentication-Warning: delorie.com: mail set sender to geda-user-bounces using -f X-Recipient: geda-user AT delorie DOT com Message-ID: <55B84CA5.3000200@buffalo.edu> Date: Tue, 28 Jul 2015 23:46:45 -0400 From: "Stephen R. Besch" User-Agent: Mozilla/5.0 (X11; Linux i686; rv:31.0) Gecko/20100101 Thunderbird/31.8.0 MIME-Version: 1.0 To: geda-user AT delorie DOT com Subject: Re: [geda-user] Component Cut-outs in PCB References: <55AFE14E DOT 5040704 AT buffalo DOT edu> <55B7DEED DOT 5080005 AT buffalo DOT edu> In-Reply-To: Content-Type: text/plain; charset=utf-8; format=flowed Content-Transfer-Encoding: 7bit X-PM-EL-Spam-Prob: X: 10% Reply-To: geda-user AT delorie DOT com On 07/28/2015 07:53 PM, Erich Heinzle (a1039181 AT gmail DOT com) [via geda-user AT delorie DOT com] wrote: > If I were doing it I'd generate a circle with line segments, turning it > into a footprint, and place the footprint where it is needed. Using integer > multiples of line segments per quadrant, and the use of line segments, > would lend itself to ears being added where needed etc... > > With this utility, you'd be just about done: > > https://github.com/erichVK5/HybridRingCouplerFootprintGenerator > > The footprint pad elements used to generate the footprint could then be > turned into silk lines quite easily in a text editor, by removing the > un-necessary fields. > The code could be fairly easily modified to do the same. > > Regards, > > Erich. Well, starting with a footprint in the shape I needed was exactly what I did do first. Looked great --but! The problem is that you can't put any graphic in a footprint that doesn't wind up on the silk layer and you can't move the footprint silk stuff onto any other layer - which I also tried - PCB simply ignores the move. That's why I eventually gave up on that strategy and drew the cutouts directly on the "Spare"/"Cutout" layer. I've also done the multi-segment circle/arc stuff. Yes. it's straightforward, but tedious when you start getting large numbers of segments when one ARC item can replace a lot of line segments. Steve > > On Wed, Jul 29, 2015 at 5:28 AM, Stephen Besch wrote: > >> >> On 07/28/2015 02:57 AM, Erich Heinzle (a1039181 AT gmail DOT com) [via >> geda-user AT delorie DOT com] wrote: >> >> Is there a standard set of shapes you use? >> >> Not particularly >> >> Can you describe the sort of cutouts you're routinely doing? >> >> >> Usually these are Cutouts in PCB's mounted on panels that need clearance >> openings for components that won't fit between the PCB and the Panel. A >> typical example might be a 10-turn pot mounted next to a toggle switch. The >> clearance cutout for this is basically a circle with 2 ears and a hat. Best >> shape is obtained with 6 arcs and a few straight lines. >> >> Steve >> >> Can you attach any examples if they are hard to describe. >> >> Cheers, >> >> Erich. >> >> >> On Thu, Jul 23, 2015 at 4:00 AM, Stephen Besch wrote: >> >>> Several years back there was a lot of discussion about the occasional >>> need for odd shaped cut-outs. Even though several suggestions were made >>> none worked - in some cases at all, or even when they did the results were >>> marginal. This is still a problem today. The only work around is to draw >>> them directly on some unused layer - for example "Spare" works for me. This >>> is however not a really good solution. Nevertheless it's better than >>> drawing them on the outline layer. First off, every board shop that I deal >>> with want cut-outs in a separate gerber file. If you use the outline layer >>> then you can't have a separate board layout - unless of course you put the >>> outline on some other unused layer. >>> >>> However, this solves only part of the problem. As long as the cutout is >>> only straight lines it's simple. If you need arcs - or worse, full circles >>> or linked arcs it gets really hard. This is largely due to problems with >>> the ARC tool in PCB: 1) you can't control/change Radius; 2) you can't >>> control degrees of arc, and 4) you can't control start angle. This is >>> really weird because the arc[...] item in PCB allows control of all of >>> these items. >>> >>> I have found only one way to get this to work. First select the target >>> layer. Then let's say you have a cutout consisting of a closed loop that >>> requires 6 linked arcs and 2 lines. Just draw them on the selected layer >>> (Spare for example) more or less where you think that they will need to be. >>> The arcs will have to be in more or less random locations owing to the >>> severe limitations of the Arc tool. >>> >>> With this as a starting point, save the PCB file (but leave PCB open) >>> then open the pcb file with your favorite text editor (AND KEEP A BACKUP). >>> Just make sure that whatever you use does not add junk characters or muck >>> around with end of line characters - Gedit is a good choice. >>> >>> Once the file is open, search for the name of the layer you are using. >>> Once found, you will see a parenthetically bounded list of the line and arc >>> definitions for the stuff you put on the layer. Here's an example of each: >>> >>> Line[1525.00mil 1565.00mil 1525.00mil 1450.00mil 1.00mil 1.00mil >>> "clearline"] >>> Arc[1425.00mil 2005.00mil 450.00mil 450.00mil 1.00mil 1.00mil 305 290 >>> "clearline"] >>> Line arguments are: Xstart Ystart Xend Yend Width Clearance Flags >>> Arc arguments are: Xcenter Ycenter Radius1 Radius2 Width Clearance >>> StartAngle AngleofArc Flags >>> >>> The 2 radii are supposed to let you draw ovals, though I haven't tried >>> it. Also, for cutouts the clearline flag makes no sense and can be omitted >>> (just have to leave the "". Clearance makes no sense either but it has to >>> be there anyway or PCB will throw an error. In fact you must be extremely >>> careful when editing these parameters since PCB is very intolerant of >>> formatting errors. >>> >>> The rest of the process amounts to entering your own values for the >>> various parameters until you get the shape you need. The coordinate >>> crosshair is very useful here. I stongly suggest saving the file after >>> every few changes (maybe even after every change) and reloading. PCB will >>> detect the change and prompt you to reload. Do this every time to verify >>> that your changes actually show up and incidentally did not corrupt the >>> entire file (the message log window helps a lot here). During this editing >>> process you may be able to do some of the positioning by dragging stuff >>> around directly in PCB. Just be forewarned that you will need to save using >>> PCB and reload the text editor after every such change made in PCB. In >>> other words: Never edit in one tool anything that has not been saved in the >>> other. >>> >>> This is extremely tedious and annoying but when you are desperate for a >>> cutout I'm afraid that it's the only way. >>> >>> Stephen R. Besch >>> >>> >> -- fictio cedit veritati