Is it possible to do solid filled circles ? - Page 1
Forum section: electronics / general

author: snoopy
author_rank: Frequent Contributor
timestamp: February 19, 2017, 05:40:44 am
content: In PCB library editor or PCB itself I cannot see how to do a filled circle. Sure you can do the outline of a circle but cannot see any options to solid fill it.Is it possible ?cheers

author: T3sl4co1l
author_rank: Super Contributor
timestamp: February 19, 2017, 06:29:37 am
content: A couple of ways you can do it. All a little hacky.Using a circle:- Set the Radius to half the desired radius.- Set the Width to the desired radius.(Thus, 1/4 and 1/2 the desired diameter.)The width fills all the way to the center, so you get a solid circle.This is the way I normally do it.Alternate:Set the radius to very nearly zero. Perhaps 0.001 mil.Set the width to the radius (technically, the radius minus 0.001 mil).The width is traced around a very nearly zero radius circle, so the resulting image is very nearly diameter = Width.Without using circles:Place a Region or Polygon, and drag around the points to an inscribed square. Grab one side and CTRL+SPACE until you get an arc. Move this arc's control points until you have the desired curvature.Repeat with an opposite side.Move the points so that the object only has two vertices (both of them arcs), and so the arcs have 180 degree angles and radii equal to the desired circle.This is the most piddly and special-case (special because Altium approximates the polyregion arcs with line segments), but is an important trick to remember when working with 3D bodies (which can only be expressed as polyregion outlines, extruded to the specified height).Tim

author: DerekG
author_rank: Frequent Contributor
timestamp: February 19, 2017, 10:13:17 am
content: Quote from: snoopy on February 19, 2017, 05:40:44 amSimply place a round SMD pad onto the layer you want.

author: julianhigginson
author_rank: Frequent Contributor
timestamp: February 19, 2017, 10:44:11 am
content: +1 for the circle primitive at radius r/2 and track width, r. It's very easy to calculate and type into the editor, post placing in the right locationYes a pad will also do it, but that's a pad, and well, pads are special things in Altium... so it's going to do more stuff in the design that you might not also want.

author: snoopy
author_rank: Frequent Contributor
timestamp: February 20, 2017, 01:42:47 am
content: Thanks.I've used one of these techniques before but you would have think Altium would have added this feature as standard by nowcheersdavid

author: mrpackethead
author_rank: Super Contributor
timestamp: February 20, 2017, 01:59:14 am
content: Draw the circle, and select itTools -- > Convert -- > Create Region from Seleted Primatives.Boom. Done.Works with any collection of curves/lines.

author: julianhigginson
author_rank: Frequent Contributor
timestamp: February 21, 2017, 12:35:09 am
content: Quote from: mrpackethead on February 20, 2017, 01:59:14 amSeems to me that if you're creating and placing the arc anyway, may as well set r/2 and r in the arc and leave it as done.... easier to edit later, too. You can precisely reposition it and resize it numerically, or drag it by the centre. While a poly region gets dragged by its vertices. (and to engage full pedant mode, a circular poly region isn't actually circular, it's piecewise linear around the edges, at pretty fine resolution, but still....)Agree it's absolutely the best option for more complex shapes though!

author: technotronix
author_rank: Regular Contributor
timestamp: February 24, 2017, 10:42:22 am
content: Have you change the mode "Fill to Solid"? This would help to fill the circles.

author: free_electron
author_rank: Super Contributor
timestamp: February 24, 2017, 07:37:51 pm
content: Quote from: DerekG on February 19, 2017, 10:13:17 amNO ! . ABSOLUTELY NOT !

author: guillep2k
author_rank: Contributor
timestamp: May 09, 2017, 12:34:38 am
content: Quote from: free_electron on February 24, 2017, 07:37:51 pmHow come? Care to explain?

author: julianhigginson
author_rank: Frequent Contributor
timestamp: May 09, 2017, 01:12:13 am
content: Quote from: guillep2k on May 09, 2017, 12:34:38 amBecause a pad is much more than a metal layer shape. It effects other things, and basically, you should not use a pad unless you want it to actually provide connectivity of some sort.And in that case, you should really have it drawn in the schematic and import the pad from there into the PCB inside a footprint. Even if the footprint only contains the one pad and even if the pad doesn't connect to other nets.

author: guillep2k
author_rank: Contributor
timestamp: May 09, 2017, 01:28:14 am
content: Quote from: julianhigginson on May 09, 2017, 01:12:13 amWell, we use pads for mounting holes and other kinds of NPTH, and they're not that special, are they? Even for slots, like for mounting USB connectors.The way I see it, pads are simply powerful objects. For instance, a pad can exist in a non-copper layer (as much as any other shape), so it's handy for drawing a disc in the overlay. If you use one in any copper layers they will follow the electrical rules as well. It's not like they'll be corrupting your gerber files or anything. They're more efficient and compact than a set of segments which won't really form a disk (as in regions) nor they are a hack as with the circle with 1/2 a radius and a thick trace.Granted, conceptually they're not meant for drawing "discs" and they could become the target for rules not intended for them, but that doesn't look like enough reason for NEVER EVER use them.

author: julianhigginson
author_rank: Frequent Contributor
timestamp: May 09, 2017, 01:40:53 am
content: Quote from: guillep2k on May 09, 2017, 01:28:14 amMounting holes are fine to make from pads - Even if not electrical, and not connected to a component like a USB socket, they are still a connection to the board (and speaking of PCB mounting holes, they are also very conceptually easy to include in the schematic. then you also have the option of defining one to be PTH, and tying it to GND for a chassis connection if you want... And if you use a parts database you can easily define and manage the exact mounting hole designs your boards have!)The issue with pads isn't that they *can't* be used ad-hoc for different things. I've certainly done lots of things with free pads in the past that I wouldn't do now..... but I learned from my mistakes.The issue is though, if you use them to draw a circle, then from that point on, the responsibility is on the board designer to manage the side effects of a "circle" on some layer actually being a pad... you are buying yourself or at least your customer/employer a possibility of future headaches when you misuse pad primitives for something that isn't a pad. This is why it's better to just create any non-pad things you need without using pads - because then you don't have that future source of mistakes lurking in your design forever, waiting for someone to trip up.

author: guillep2k
author_rank: Contributor
timestamp: May 09, 2017, 01:51:04 am
content: Quote from: julianhigginson on May 09, 2017, 01:40:53 amCan you give me an example of the kind of headache we're dealing with here? Electrical? Mechanical? Do they mistakenly appear in the BOM? I'm not trying to argue here; just trying to learn from other people's experience.One use I give pads is to make fiducials. They have their own footprints so they're not technically "free pads", however they are pads used as discs and for pure "graphical" reasons. I've thought most people did them like that.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: May 09, 2017, 02:04:42 am
content: Pads and circles (of suitable width) are both circular graphics features.They don't make any difference in the Gerbers, or the PCB fab*. None at all.*With suitable pathological exceptions, like building a shape out of a gazillion thin or small shapes that get optimized out by the fab. I've had that happen before, on bitmaps.So, assuming thick, proper, intended shapes here.So what's the point? Why have either, anyway?It's all about the EDA data, and the process.If you're taking more time constructing copper shapes out of inconvenient entities, that's your wasted time.If you're taking more time setting the design rules to allow for all the exceptions to the entity types used, that's your wasted time.If your use of primitives has resulted in a confusing mess on the testpoint output, that's your PCB fab's and test house's wasted time.If your customer requests the files (or a compatible export format), and finds they're behaving goofy because of weird shapes or buggy export/import, that's their wasted time.So, for a basic fab -- no, it won't matter. For a full production process, it can matter.(A lot of these can be addressed very easily, like in Altium, for any "IsPad" rule, use "AND OnCopper" with it. Or for test data, place a few pads on random layers and export some IPC and ODB++ files, and see if they show up or not. I've never tried but I wouldn't be surprised if only copper pads are enumerated by Altium.)Me, I only use pads for electrical connections, and fiducials (which are, in a sense, a visual connection, that the fab or assy needs to know, so should be exported with the test data that they will also need). This makes sense to me, and avoids the bother of qualifying "IsPad" anywhere.Tim

author: guillep2k
author_rank: Contributor
timestamp: May 09, 2017, 03:11:15 am
content: Quote from: T3sl4co1l on May 09, 2017, 02:04:42 amOK, thanks for the explanation.