Hopping on the PCB layout bandwagon - need opinions! - Page 1
Forum section: electronics / projects

author: shadewind
author_rank: Frequent Contributor
timestamp: March 14, 2011, 09:31:20 pm
content: Yeah, I'm going a little "me too" here and I want to show you my first PCB before I send it off to manufacturing. I was going to try my luck with ITead Studio since it's so cheap and it's my first board.http://dl.dropbox.com/u/2462319/topside.pnghttp://dl.dropbox.com/u/2462319/bottomside.pngI hope you can tell all that is needed from these two pictures. It's an RGB LED controller based around an ATMega8A. The reason I use such a big chip when I need so few I/Os is that it's the cheapest AVR I could find and I have a couple of the lying around. It's powered by a National Semi LM2676 switcher. I probably could have made it smaller using surface mount components but since I've never soldered those before, I don't want to go into two, unknown territories at once (both SMT soldering and PCB layout).Anyway... as can be seen from the pictures, I've flood filled both the top side and the bottom side with GND. I've seen some people do VCC flooding on the top instead... when should you do this and when should you not?Also, I'm wondering what information is appropriate to place in the overlay? I've seen some people include text and information in the copper, why would you do that?

author: VIPR
author_rank: Contributor
timestamp: March 14, 2011, 11:28:46 pm
content: Nice work for a first PCB design!From a quick look at both side I can only find a couple of things that I would change if I were you, and depending on which board house you use, may have to in order to be within their abilities.First lets touch on the overlay layer (yellow). I would move the R1 and R2 labels so that they are not right on top of a pin for the ATmega8. The overlay goes on last so you overlay ink will be on the plating surround the hole and might make it difficult to solder from the top side. It's quite common to put the part label within the confines of the part outline. However, this does make it more difficult later on if you have to troubleshoot since you won't be able to see the label. That should not be a problem on this board since you designed it and it is relatively simple. Also, in case you didn't know, you can rotate just the labels for the P1 connector. Just press and hold the left mouse button over the individual number and press the space bar twice and then move label into proper place.Now for the copper layers and through holes. First thing I would do is beef up you annular ring for every hold by about a third, otherwise you will probably be fighting with soldering in the components since you will have to have very little copper to get in contact with around the holes. If this board was going to be wave soldered you could get away with the smaller dimension annular ring.Something the board house will probably gripe about is the Q1 thru Q3 having too little clearance between pins. By looking at it on my monitor it looks like you only have about 2 mil of copper on the narrow sides of the pads. They won't like that but they especially won't like that there is even less clearance on the solder mask layer. In order to make an adequate solder mask they normally need to have clearances of about 4 mil between pads (this is due to how solder masks and overlays are made but I won't get into that). Without solder mask between pins you will very likely have solder bridging happen when you are attempting to solder those transistors. Trust me, those pins being that close together will make it quick difficult to solder without bridging. So, double click the component and uncheck the "lock primitives" box. This will allow you to move the pads individually without moving the whole part. Spread the outer two pads away from the center one by about 50%. You may also need to move the overlay outline of the part some too in order to get enough clearance between pads. Now you will have room to beef of the width of those pads so that you have enough annular ring all the way around and the board house should be happy. Don't forget to re-check the "lock primitives" box when you are done.As for when to use copper fills on one or both or many layers is really dependent on what the PCB is going to be used for. In RF PCB design it is very common to use fills throughout a design for several reasons but mostly to keep crosstalk to a minimum and to provide shielding. Also, it is quite common to have a third signal layer sandwiched between to outer layers that are filled with ground on one and power on the other. This helps to shield the inner signal layer(s) from outside interference. There are several other reasons for using the fills but I won't get into all that since this post is long enough already.When to not use fills: when you are doing audio work or other mixed signal PCB design. In those case you want to have an analog ground and a digital ground and you want them to be separate so as to keep the digital noise off the analog ground. In most cases you will want to run all of your analog grounds directly from each ground pin to where the ground is introduced to the board. This is mostly due to the voltage that will develop across your ground traces thus rendering your ground not really ground but just above or below ground based on how much current is traveling through the PCB trace.If you have any more specific question about Altium just let me know since that appears to be what you are using.

author: shadewind
author_rank: Frequent Contributor
timestamp: March 15, 2011, 12:29:00 am
content: First of all, thanks for the great input!I actually knew that the labels shouldn't be on top of the pins, I was just being sloppy apparently but I've fixed that now as well as adjusted some other things (more room for an eventual heatsink on U1 et.c.).About the annular rings, these are from the footprints that come with Altium... are you saying I'll have to make my own for every component? I'm not sure that I'll actually have any problems soldering this by hand...About Q1 through Q3, those are IRF MOSFETs with an I-PAK package and the spacing between the pads is actually 10 mil so that should be fine, shouldn't it? I don't know about the solder mask though but it isn't really that close so I don't actually think I would get any bridging when soldering.For the record, I am indeed using Altium

author: VIPR
author_rank: Contributor
timestamp: March 15, 2011, 01:36:25 am
content: Well, the footprints that come with the software are really designed for wave soldering a board in a commercial assembly house so the annular ring does not have to be very wide. However, for hand soldering it will make the job a whole lot easier if there is more copper around the pin to heat up which will help with solder flow through the PTH and thus a better connection and less likely hood of a cold solder joint. I'm not saying you can't do it as it is or that the PCB manufacturer will have a problem with it but why not make the job a little easier on yourself if you can.Changing the default annular ring can be done the hard way or the easier way. The hard way is to just double click on each pad throughout the design and change the X and Y dimensions of the pad. That is a tedious thing to have to do but it will get the job done eventually. The easier way is to use the built in PCB filter tool to either select all of the pads of a particular part or all of the pads of the same footprints at the same time. What then happens is only those items are selected on the PCB and you just use the PCB inspector tool to change the X and Y dimensions all at the same time. Once done just press Shift+C to clear the current filter and start on another footprint or set of pads. Use the "Builder" option in the PCB filter tool as it is more intuitive and thus easier to use. Just add the first condition that the object kind is a pad and then add a second condition that the pad is associated with whatever footprint you are looking to change the pads on. This method still take a little while but is much quicker the former method. Actually, most PCB design work take a while. Just be thankful that you have the best software out there for the job IMHO.The I-PAK footprint: 10 mil between pads with a default solder mask expansion of 4 mil = 2 mil of solder mask between pads. That is normally less than most board houses will accept for through hole pads. You can always bypass the the solder mask expansion rules on those particular pads and change it to only 3 mil. That would leave about 4 mil of solder mask between pads which should be acceptable to most board houses. For reference the average thickness of a human hair is 4 mil. This means that your pads will have about 2 1/2 human hairs between them at 10 mil. That's pretty tough to solder by hand without having lots of solder bridges. It can be done with a good soldering iron tip but still tricky.The other think about those I-PAK footprints to be concerned about is the amount of copper on either side of each pin hole (the annular ring we've been talking about). From the pictures it doesn't look like much--I'm guessing about 2 or 3 mil. That may not be acceptable to the PCB manufacturer. One of the reasons why is that the manufacturer has limits to their guaranteed hole registration (drilling accuracy). For example, look at the boards that Dave just got from Itead Studio. That can become quite a problem with really tight spacing. Remember, we're only talking the distance of a few human hairs.

author: shadewind
author_rank: Frequent Contributor
timestamp: March 15, 2011, 01:49:09 am
content: The distance between the pads and the solder mask between them is fine according to the design rules of Itead Studio but the space between the hole and the edge of the pad is not I suppose? But the minimum track width of 6 mil shouldn't affect this since the holes are drilled afterwards, should it? Anyway, misalignement when drilling might screw the whole thing up so I'll go ahead and increase that clearance like you said.Is it possible to create a new footprint by modifying an existing footprint included with Altium? In this case, I could simply make a new footprint and apply that to the IRF MOSFETs and then save it for use in future boards (those MOSFETs were cheap and worked great even when driven directly by the MCU so I'll probably get some more of them)?

author: VIPR
author_rank: Contributor
timestamp: March 15, 2011, 01:54:54 am
content: Oh yeah, a couple of things I forgot in the last post. If you do decide to move the pads around on the transistor footprints you don't have to delete your current copper fill. Just go Tools-->Polygon Pours-->Shelve Polygon(s). Then, when you are done all you have to do is go Tools-->Polygon Pours-->Repour All Polygons. That might save you some time over completely redoing the fills each time you move something.Also, on your updated pictures I noticed under R2 there is ratsnest wire showing, so something is not connected that needs to be. Might want to have a looksee at that or just run a DRC. Nothing more annoying then sending off your boards for production and getting them back, building them up and have them not work right because of a simple mistake like overlooking one connection that is glaringly obvious after the fact. I believe everyone that has designed a PCB has probably had that gut wrenching experience.

author: VIPR
author_rank: Contributor
timestamp: March 15, 2011, 02:17:31 am
content: Quote from: shadewind on March 15, 2011, 01:49:09 amYeah, you can modify all the schematic symbols and footprints that come with the designer but for such a simple footprint as the one you are working with why not try out making one from scratch. The software makes it pretty easy to make a new one. However, if you just want to alter the one that comes will the software you can but you first have to find where it is located and open that file, make the changes and then save the file. That particular footprint will be located in a library of PCB footprints that was used when making the integrated library that you probably pulled the part from. I am guessing that is the miscellaneous devices integrated library? In that case you will be looking at approximately this location C:\Program Files\Altium Designer\Library\Pcb for that footprint library which will likely be called Miscellaneous Devices PCB.PcbLib .I would strongly recommend you just make your own footprint library and then associate the schematic symbol with that new footprint. Just remember to double check that the pin numbers you assign on the footprint agree with the pin numbers on the schematic symbol. When I started using the software back in 2003 or 2004 I had the most difficulty understanding how all the integrated libraries worked (I was coming from OrCad at the time) and how to manage them along with their source files when recompiling the integrated libraries and how to make new ones too. I tell you this just so when your sitting there scratching your head in frustration trying to figure the whole thing out you will know that you are not the only one.

author: shadewind
author_rank: Frequent Contributor
timestamp: March 15, 2011, 10:22:45 am
content: I alredy know how to make it from scratch so that's why I'm asking. The inductor L1 and the electrolytic caps in there are footprints I've made myself

author: metalphreak
author_rank: Frequent Contributor
timestamp: March 22, 2011, 03:33:54 pm
content: Is that a DC power jack on the top left?Just make sure its the right footprint for the parts you have. Some of them are designed such that there is a slot milled out of the pcb to accomodate the flat pin. This is usually put on the "mill" layer and usually isn't put on the layers you send to ITead etc.Yours appears to have two holes per pin for mounting, and most of the common through hole jacks won't fit. What you really want is just 3 oversized pad holes. If you are using Eagle, I highly recommend downloading the Sparkfun Eagle library. There's a few variations in there for DC jacks with some notes on where to use each.Attached is a photo of the common one I use. Works great for jacks like these:http://www.laptop911.ca/images/page_upload/73/Image/R0007_DC-POWER.jpgYou just fill in the extra space with solderYou can see the boxes in red that make up the "mill" area where the slots would be.

author: shadewind
author_rank: Frequent Contributor
timestamp: March 23, 2011, 01:18:49 pm
content: The tip about polygons was great, I didn't know that! This will save lots of timeI redesigned this board to use the QFP32 version of the ATMega8A instead so I could fit it on a 50x50 mm board (and yes, this one was checked by the DRC checker). The same applies for the DC jack though. There is actually a mechanical layer for the DC jack although it's not visible in the pictures I posted. I included that mechanical layer to the file I sent to iTead so we'll see if it gets routed out properly. In if doesn't, I can always route it out myself using a drill so I think I'll be fine.Another question... when using the component clearance rule, Altium checks the clearance for each component using a bounding box for the whole component. While this is fine for many components, it wastes a lot of space when using large round components, space which can be critical on a tightly packed board. Is there a way to make it check clearances basen on the actual shape of the component?

author: VIPR
author_rank: Contributor
timestamp: March 29, 2011, 10:45:10 pm
content: You can add a new component placement clearance rule by right clicking on the component clearance rule in the "PCB Rules and Constraints Editor" and selecting "New Rule". Then just select that new rule and select the "Query Builder" option in the top selection box and simply filter out everything except the footprint or component(s) that you wish to apply the new rule to. Then set the new rule parameters (in this case less clearance) and hit apply. The DRC will now use the smaller placement clearance dimension for those components that you selected by filtering. You can add additional rules to any rule or rule category for tighter definitions of what you want to accomplish.I am not aware of any way to just set the clearance for all round objects.Hope that helps.

author: shadewind
author_rank: Frequent Contributor
timestamp: March 31, 2011, 11:39:37 pm
content: Yeah I knew I could do that but it's not really what I'm looking for. Thanks anyway though! What I'm doing now is simply ignoring the warnings when I'm sure the clearance is enough.

author: Time
author_rank: Frequent Contributor
timestamp: April 01, 2011, 01:46:28 am
content: if your gerbers can passwww.freedfm.commost any board house can make it error free.