PCB Design Rules - Page 1
Forum section: electronics / beginners

author: elefurtronik
author_rank: Regular Contributor
timestamp: February 10, 2023, 11:24:06 pm
content: Hello,I would like to know how can I learn the PCB design rules? Is there any specific design rules or book for it?If not the case, while designing a PCB what I should pay attention?

author: james_s
author_rank: Super Contributor
timestamp: February 11, 2023, 12:51:14 am
content: There aren't too many rules, but there are a handful of best practices. Neatness counts, avoid weird angles and sharp 90 degree bends, don't forget about mounting holes, and pay attention to things like grounding and layout tips from datasheets for circuits like switching regulators. You can learn a lot by studying commercial boards. What sort of circuits are you interested in building? Find a simple project to start out with, download and install KiCad and we can give you guidance.

author: dobsonr741
author_rank: Frequent Contributor
timestamp: February 11, 2023, 02:47:04 am
content: Set and keep a few simple rules; depending on the density you are about to use. For example, for through hole all holes to be on the 0.1” grid, use 1mm track width, or more if higher current. Do not go in between two pads on the 0.1” grid.If your density is SMD, you can still set rules with smaller dimensions for yourself to follow.Another design rule is to arrange the components first, including connectors, so that related blocks are together and their connection lengths minimized. You can see that on the “ratsnet”.Route GND and power first, so that you can have short lengths and low impedance on those nets.Avoid placing vias every time you can’t reach a destination, take it as a puzzle and rearrange. Once all connections are in place, don’t be ashamed to spend equal amount of time rearranging, making it neater and make the track patterns visually appealing. You’ll also find bugs while beautifying.Finally, review the gerbers in a viewer before sending off to manufacture.

author: wasedadoc
author_rank: Super Contributor
timestamp: February 11, 2023, 06:05:05 pm
content: If the board has tracks with AC mains on them you need to pay special attention to spacing from others.

author: Infraviolet
author_rank: Super Contributor
timestamp: February 11, 2023, 07:31:39 pm
content: Design rules are usually set by the board house you'll be having fabricate the boards for you. Most board house's rules for "typical" designs (not oens using special higher priced higher precision services) will be broadly the same, usually things like clearances of >0.15mm between all separate conductors, minimum via 0.3mm, minimum track width around 0.15mm, how close to the edge of a pad you can depend on the soldermask being... Many board houses will have a design rule file you can download for your PCB CAD program.

author: nigelwright7557
author_rank: Frequent Contributor
timestamp: February 11, 2023, 09:41:55 pm
content: Quote from: elefurtronik on February 10, 2023, 11:24:06 pmYou need to visit your pcb manufacturers website for component clearances, min via hole size etc.I use JLCPCB.

author: tooki
author_rank: Super Contributor
timestamp: February 12, 2023, 01:39:18 am
content: Quote from: Infraviolet on February 11, 2023, 07:31:39 pmQuote from: nigelwright7557 on February 11, 2023, 09:41:55 pmFrom the wording of the original post, I don’t think the OP means “DRC rules for my layout program” or “manufacturing tolerances”, but rather, best practices and general know-how of PCB layout.

author: golden_labels
author_rank: Super Contributor
timestamp: February 12, 2023, 03:36:17 am
content: Hard rules:I can’t think of many.For high voltage side you want to remember about proper distances between traces and clearly separating high-voltage and low-voltage sections.GHz+ range RF circuits are very unforgiving and require careful planning to ensure proper impedances, but this is a “when you need it, you will know it” thing.Soft rules?Clear separation of functional areas.In particular keep power supply, analog and digital blocks separated — assuming there even is such a clear division. This will reduce interference between them.In the past, in particular for homemade circuits 90° turns and unbeweled T-joints at narrow angles were a big no. They were causing overetching. But that is no longer an issue for manufacturing houses. Still a good idea to avoid them, even if for aesthetical reasons, but no reason to panic about them.There is a strong aeshetical preference for 90°/45° angles. The historical reason behind this kind of a layout is limitation of early CAD software. Programs could not handle anything other than horizontal and vertical traces; later extended to 45° ones. Before that no one cared: google for “1960 pcb” images to see, what I mean. Now we slowly regain ability to make arbitrary traces. However, the preference for 90°/45° aesthetics remains. The reason remains unknown to me.Never forget about mounting holes. If there are connectors on PCB, consider if their placement with relation to the mounting holes makes sense: you do not want to split your PCB in half while attaching cables.Keep footprint designation at meaningful places, so the reader could tell, to which part they refer to.In general, make the layout possibly easy to read and follow.

author: NOON Design
author_rank: Contributor
timestamp: February 13, 2023, 12:20:01 am
content: Also, always keep in mind that you're designing a 3D object in 2D software. You need to be aware of the height, width etc of all components and connectors and how they fit and interface with the enclosure it's all being mounted in. The mechanical design of a PCB is at least as much work as the electrical design.

author: dobsonr741
author_rank: Frequent Contributor
timestamp: February 13, 2023, 12:32:33 am
content: Great point on 3D. A good argument for KiCad. 3D view comes easy, has big built in library with 3D rendering. Super easy to check alignments and component heights in the 3D view.

author: rdl
author_rank: Super Contributor
timestamp: February 13, 2023, 02:21:41 am
content: Dave has a PCB design tutorial in pdf form available here:http://alternatezone.com/electronics/Despite being 20 years old, it still has useful information.

author: basinstreetdesign
author_rank: Frequent Contributor
timestamp: February 13, 2023, 05:07:55 am
content: Here is a checklist we used to use when doing pcb artwork. Some things need to be confirmed with the fabrication house, such as dielectric constant(s), etc.Component Placement CheckoBoard OutlineoMeasure for accuracyoNo components in Keep-Out areas (especially .2” border around outline)oIn-board cutouts are correct dimensionsoConnectorsoPin 1 and pin 2 in correct locationoPins spaced correctlyoEnd pins or every nth pin numbered on silkscreenoSilkscreen outline is correctoNew Library PartsoAll parts used for the first time are correct size (also check with actual part on 1:1 scale dwg)oCheck pad sizesoCheck silkscreen outline is correctoPin locations are correctoComponent Layout’oAllowance for device sockets where neededoAll components are oriented correctlyoAdjustable parts located and oriented correctly - check for pot rotation, etcoTextoAll reference designators are outside part outlines and off all SMT land patternsoAll designators and other text is oriented as required by the client or to be right-side-up when the board is viewed as per normal practice when in use or during servicingoFiducialsoAll fine-pitch IC’s 100 pins and over have fiducial marks in opposite corners of the IC footprint or located centrally to the part as per the clients instructionoThe board has fiducial marks in three corners and are aligned X & Y with each otherRouted Board CheckoAutomated ChecksoNetlist Check DoneoDimension Check DoneoCritical Tracks/LengthsoCritical line length report is produced and checkedoDrill ChartoDrill Sizes OKoTooling holes are non-platedoRe-annotationoIf the board was re-annotated check order of numbering is correct (left to right, top to bottom, etc)oThe back-annotation or “was-is” file was producedoDon’t forget to update the dependant documents accordingly using this “was-is” file (such as the BOM)oPlanesoGround and power planes are split correctlyoSplit gap size is at least .100”oClearances to mounting holes and board edge is at least .125”oApprovals RequirementsoCSA/UL clearance and creepage distances are correct according to latest rev standardsoFabrication Drawing to fab houseoDrawing of board with all major edges dimensioned especially those that fit between card guidesoLayer stackup is shown with layer-to-layer dimensions (confirm fab house will build-to-suit)oTooling holes are dimensioned from datum board edgeoIf controlled impedance tracks are required the dielectric constant and target impedances are includedoAssembly Drawing(s)oDrawing indicating those parts on the solder side are shownoAll on-board parts that require hand work are shown in sufficient detail to make clear what is neededoLayout File PackageoAll files are included (gerbers, aperture and X-Y position files)

author: Veketti
author_rank: Regular Contributor
timestamp: February 13, 2023, 05:45:14 pm
content: Quote from: dobsonr741 on February 11, 2023, 02:47:04 amSorry, not trying to hijack the thread, but could you tell why need to avoid vias?

author: dobsonr741
author_rank: Frequent Contributor
timestamp: February 13, 2023, 06:12:41 pm
content: In @elefurtronik's original context I assume a young player is asking how to start in layout design. There can be temptation to get to anymore on the board with vias uncontrollably. That's what the advice is attempting to put limits around.

author: elefurtronik
author_rank: Regular Contributor
timestamp: February 13, 2023, 07:27:32 pm
content: Thanks for all the answers. I am definitely a young player who wants to design rigid PCBs. I definitely think that it is like a puzzle. It is actually an art.

author: james_s
author_rank: Super Contributor
timestamp: February 13, 2023, 07:34:58 pm
content: Quote from: Veketti on February 13, 2023, 05:45:14 pmVias are a potential failure point, and typically have higher resistance than the trace. They also increase manufacturing effort as they are more holes to drill and plate. I don't go to heroic efforts to avoid them but I do try to use them only when necessary.

author: tooki
author_rank: Super Contributor
timestamp: February 13, 2023, 11:18:13 pm
content: Quote from: Veketti on February 13, 2023, 05:45:14 pmIt’s a good question. Of course, vias are there to be used. But at the same time, excessive vias (or rather, an excessive need to jump between layers) can be an indicator of an inefficient design. In low frequency circuits this is often of no practical consequence, but it sure is satisfying to come up with an elegant design! In high-frequency circuits (an area of electronics black magic that I’ve only just dipped one little toe into — we shall see this week if the board I laid out works out for my client, once i populate it…), the added inductance of a via can actually present a meaningful impact in the circuit.But honestly, to me, it’s kinda fun, figuring out how to create a layout that is simple, compact, and sensible. There’s a real satisfaction when it all just falls into place. It often takes a lot of work to come up with the solutionwhich looks obvious in hindsight. (The holy grail being a design so good that it looks like theonlyobvious solution.) In practice, the “obvious” solutions are often the ones that took the most work to get to.(Everyone knows the saying that something is “overengineered” when it has a very “heavy” way of doing something. But in actuality, that’s notoverengineering, it’sunderengineering. It’s easy toaddthings to design something to do what you want. The skill and effort go into making something that does what you wantwithoutadding things!)(Sorry for the philosophical rambling. I’m on the way home from a pub quiz and I’ve had a few ales! :p)

author: nigelwright7557
author_rank: Frequent Contributor
timestamp: February 15, 2023, 12:20:16 am
content: I remember a nearly pcb design I made.It was a USB audio mixer.Just laid it out best I could.Then built one up.With input shorted I got 1VRMS on output !After digging around wit ha scope I found the charging impulses into smoothing caps were modulating the ground line and the voltage was being amplified by the op amps.I reworked pcb keeping power supply separate and that fixed it.Another audio thing is star grounding to decrease hum. Same as previous problem with signals modulating ground line.

author: BillyO
author_rank: Super Contributor
timestamp: February 15, 2023, 01:32:02 am
content: For the hobbyist making low frequency deigns??Make sure there are no shorts and make sure everything is correctly connected. Other than that?PCBs are so cheap now I hardly ever do hand wired or breadboard prototypes.For high speed industrial/military/medical/consumer designs there are a mountain of rules you either must or should follow. Beyond the scope of a beginners forum.

author: golden_labels
author_rank: Super Contributor
timestamp: February 15, 2023, 01:40:45 am
content: Quote from: BillyO on February 15, 2023, 01:32:02 amKeep in mind “cheap” is relative. To a young beginner from Poland, who is hardly a hobbyist yet, $2 is not the same as $2 to you. And mind Poland is still on the richer end of the scale.

author: johnboxall
author_rank: Unknown
timestamp: February 15, 2023, 01:58:24 am
content: Quote from: elefurtronik on February 10, 2023, 11:24:06 pmThis is a good read:Printed Circuits Handbook, by Clyde Coombshttps://www.amazon.com/Printed-Circuits-Handbook-Seventh-Coombs/dp/0071833951

author: Psi
author_rank: Super Contributor
timestamp: February 15, 2023, 02:16:33 am
content: They're really just rules you impose on your own design so it can actually be manufactured and can be manufacture cheaply, or as cheap as practical.Your PCB manufacturer has things that can do and things they cant. And things that cost more than normal.So understanding design rules is really about understanding what your PCB manufacture can do and the costs.Then you setup rules to stop yourself accidently doing something that would make your PCB more expensive or impossible to make.You will be ok with any manufacture if you keep your track size and clearance size above or equal to 0.2mm (8mil), and keep your holes/vias at 0.3mm drill 0.6mm pad size or larger. And keep tracks 0.5mm from the edge of the pcb. And keep angular ring above 0.2mm. And keep silkscreen text lines above 0.2mm thick and text characters over 1mm tall. And keep solder mask expansion above 0.1mm

author: Bud
author_rank: Super Contributor
timestamp: February 15, 2023, 04:41:46 am
content: Quote from: dobsonr741 on February 15, 2023, 02:06:06 amI skimmed through the book and it seems it is meant for PCB factory production engineers. Seems to be useless or nearly useless for PCB design.

author: Bud
author_rank: Super Contributor
timestamp: February 15, 2023, 04:47:43 am
content: Quote from: elefurtronik on February 10, 2023, 11:24:06 pmPerhaps you mean PCB designpractices? PCB designrulestypically refer to physical and electrical limits and restrictions that you yourself define and enter into the PCB software, and then the software monitors your design and alerts you when you violate these rules.

author: Watth
author_rank: Frequent Contributor
timestamp: February 15, 2023, 12:38:51 pm
content: I think you could try a first layout and show on this forum. There are knowledgeable people here that could then give you a few pointers.

author: bidrohini
author_rank: Regular Contributor
timestamp: February 24, 2023, 12:00:52 pm
content: Here is a beginner guide to Altium Designer:https://www.pcbway.com/blog/PCB_Design_Tutorial/Beginners_guide_to_PCB_design_with_Altium_Designer.htmlYou can learn how to use Altium designer to design schematics from this. You can also learn how to turn it into PCB. And it also shows how to export Altium PCB files into Gerber for manufacturing it.