Secrets of PCB Optimization - Rick Hartley - AltiumLive 2020

on to the first speaker and as i said this gentleman is really one of my favorites um i've heard him speak now i don't know if i'd be exaggerating if i said 10 times probably 10 times at least um i've learned something new each and every time he has a real commanding presence live and i'm assuming that commanding presence probably translates over to this virtual event as well um there's just something about his voice that just soothes me and i really focus in and i learn something new each and every time and i can hear him now talking about um the current flow doesn't actually flow through the traces but it flows in the space between the traces and between the layers of the board and uh he's just an excellent excellent presenter he's also one of those gentlemen uh that we're quite proud to be associated with because of his legendary status and without further sort of delay we'd like to bring in rick [Music] hartley [Music] rick hartley retired from l3 avionics is the principal engineer of r-heartly enterprises through which he consults and teaches internationally to resolve emi noise and signal integrity issues he's helped major corporations in the u.s and 14 other countries rick's 50 years in industry is focused on circuit and pc board design for computers aircraft avionics and telecommunications his consulting focuses on those industries as well as medical systems automotive electronics and appliances rick has an engineering degree and 55 years in electronics engineering he starts seminars at various ieee events pcb west freescale technology forum altim live ipc apex expo and other public and private forums rick is a member of the ieee the executive board of pcea and a past member of the editorial review board of printed circuit design magazine additionally he's written numerous technical papers and articles on methods to control noise emi and signal integrity please welcome rick hartley hello everybody thank you for attending and thank you for that very nice introduction pc board optimization meaning what there's a lot of things you could optimize on a pc board in this particular case we're going to talk about designing boards to optimize manufacturability mostly we're going to discuss fabrication but to a small degree we will also discuss assembly when i was putting the material together for this it occurred to me that i could make a really long presentation out of this i could easily make four to six maybe even eight hours of material on this topic and i might very well do that in the future but for today we have an hour and a half and we've got a lot of ground to cover and that hour and a half includes q a so let's get started bear board fabricators when you send a circuit board a design to a bare board fabricator they have a list of critical parameters that they look at and they review those parameters relative to your design to decide just how producible your board is and here's a list of some of those parameters board size versus number that will fit into a panel is notice that's item number one on the list that's one of the key items that fabricators will look at when they're reviewing your design why because how how much material they have to use to build your boards will have a big impact on what they're going to charge you and what it's going to take for them to get to give you a reasonable price and still have a profit margin for themselves we're going to talk in a few minutes about what i mean by a panel for those of you who aren't familiar with the term circuit board fabricators don't build boards one at a time they build panels and i'll go through more of that in a moment another of the parameters they look very hard at is material of construction what is it made of chem three fr4 polyemit whatever each of them has a different weighted cost and you'll see what i mean on that in just a moment as well number of layers clearly everybody listening to this knows that number of layers plays a role with two layer board is going to be cheaper than a four cheaper than a six and so on and so on but not just layers but layers for given board thickness i've met far too many engineers in my life and board designers who somehow think it's okay to put 16 or 18 layers in a 62 mil thick 1.6 millimeter thick circuit board i'm not sure where the concept even came from while i do know where the concept came from a lot of engineers think especially mechanical people that circuit boards always need to be a sixteenth of an inch thick that's been a long-held belief because in the early days of circuit board design and fabrication the materials they used that they started with early on just happened to be a 16th of an inch thick that was simply what they used there were many reasons for that not going to get into that today but they started with 16 material and the early one and two layer boards were laminated were i'm sorry were created were fabricated on a 62 mil thick material that concept is kind of stuck with everybody and to make matters worse a lot of people put boards and card guides that plug into a backplane and a lot of the card guides have 62 mil slots in them or 70 mil slots allowing forcing you to put a 62 mil thick board in there and that's all fine and dandy but you really have to think about the art of the possible when you put 16 layers into a 62 mil thick board the dielectrics are painfully thin and it makes the fabricator's job much harder than you think it is or should would be especially if it's a controlled impedance design controlled impedance boards require much greater care and much more control of dielectrics than the thin dielectrics you'll end up with putting 16 or 18 layers in a 62 mil thick board when i was at l3 for example l3 avionics systems i don't know that all l3 divisions do this but ours did we did a lot of 12-layer boards and we worked with our fabricator to come up with an optimum board thickness for 12 layers and we collectively working with them arrived at a 75 mil plus or minus 5 mil thickness for our 12 layer boards that gave us dielectrics that were easy for them to control and gate and allowed us to use line widths that gave us good routing densities and still hit the target impedance we were after all of these issues played together we could have put 12 layers in 62 mils but it would have changed things to the point where it would have made the fabricator's job more challenging because a 50 ohm line would have been a narrower trace and narrower traces are harder to hit with controlled impedance it's just that simple so the point i'm making is think carefully about what you're doing when you choose a board thickness drive into the mechanical people's heads pardon me drive into the mechanical people's heads the boards aren't all 62 mils thick they if you're gonna mount boards on four screws on standoffs or eight screws or whatever they certainly don't have to be a defined thickness they can be whatever you need for them to be make sure everybody's aware of that and work with that number of holes in a panel they used to charge per hole they don't do that anymore but you still pay based on lots of holes up to 3 000 is a is a fixed cost typically per panel three to ten thousand is a little bit higher cost in a panel and so on there are groups that they there there are uh quantities that they group together and when you step up in mass quantity of holes price is going to go up i mean it just takes longer to drill and wears out more drill bits it's that simple um smallest hole diameter what's the smallest hole they can put into a board based on your thickness and still get the drill to go through the board straight without wandering and be able to wash plating solution through that hole and get an even plating all the way through the hole when they get to the plating process there is a minimum size and it's not just a minimum size it's a minimum size based on board thickness there are aspect ratios that they can hit the aspect ratio for a 62 mil thick board might be different than the aspect ratio for a 93 mil or a 120 mil thick board six to one aspect ratio is something that in most boards most fabricators can hit asking for six to one aspect ratio and a 62 mil board is relatively easy ten to one aspect ratio is another one that they can most of them can hit but it certainly is going to be a cost editor you will pay more for a ten to one aspect ratio than you will a six to one can they do ten to one in a 62 mil board most fabricators can't because that would be a six mil plated hole they would have to drill a seven to seven and a half mil hole and plate it back to six mils very challenging for a fabricator to do talk to the fabricators know what you can do we'll talk more about that as we go um pad to hole ratio there are pad to hole ratios that are set by not only the fabricators but by the ipc standards most fabricators follow the ipc standards as the guideline for producing circuit boards if you're not familiar with ipc standards you really need to become familiar with them uh ipc 2200 series 2221 2222 and so on the 60 6000 series 6011 6012 if you're doing flex 6013 uh the the manufacturing series 610 611 and there are plenty of others those are just examples of standards you as a designer or an engineer your designing circuit boards need to be familiar with so keep all that in mind if your company's not an ipc member try to get them to be if not then just buy the standards directly from ipc you'll pay more if you're not an ipc member but they're still very reasonably priced i mean anywhere from twenty to fifty dollars each and that's not outrageous given that you probably only need a half dozen or so so think about that very carefully anyway all of these things that you see here hold the board thickness aspect ratio we talked about all of these things matter here are some additional items to consider and these are things the fabricator looks at in your design minimum trace width and space what is the minimum trace and space that you can put on and in the board and oh by the way you can put thin narrower traces inside of a board than you can on the surface of the board why because inner layers are printed and etched outer layers are printed plated and etched and it makes a difference just exactly what line width you can produce on and in a circuit board we will cover some of that later trace based width versus copper thickness we're going to talk about that later why would that matter because if copper is two and a half or three mils thick on an outer layer you honestly think you could etch a three mil line in copper that's three and a half mils thick it's no longer going to be a rectangle it's going to be a square when you look at it in cross-section and that's going to be a real challenge for a fabricator to do they might be able to do it but the scrap rate's going to go up speaking of which when there's scrap at a fab house who do you think pays for that if you've guessed us as the designers our companies you're right you've guessed correctly fabricators know their processes and know them well and if we ship them designs that make sense that are well thought out they won't have scrap or they'll have so little it'll be almost irrelevant when they have high levels of scrap it's because we i and others like me have not done our job properly scrap is our problem and guess what and guess what we pay for it and we'll talk more about that in a few minutes design specific features there are a lot of controlled impedance do you need controlled impedance you're going to pay more for that what tolerance do you need we'll talk about that in one second um the source for these bullet items uh that we're looking at is a paper from our friend happy holden and you can find it on altium's website altium.com all you have to do is look up design report card by happy holden and you will find us you will also find in that paper this particular table this is an example of a fabricator's report card and you can see the line items on here material of construction notice these are weighting factors you want low numbers on your report card because the lower number your fabricator comes up with on the report card the less they're going to charge you per panel they determine a cost per panel based on the score that they create when they establish a report card for you higher scores means you're going to pay more per pound lower score means you're going to pay less per panel notice that fr4 has a score that's one-third that of polyamide do you need polyamide well unless you do i certainly wouldn't specify it unless you truly need it for temperature reasons which is typically why people would spec it obviously polyamide is classically used in flex boards and there are many reasons for that but i'm talking about rigid boards in this case if you need something that's really high-end like rogers taconic or arlon material or one of the high-end izola or nelco materials or something from metschusta who's panasonic or any number of other companies there are a lot of companies that make high-end materials if you need these high-end materials then you have to specify them but understand they do have a cost weight associated with them a number of holes in the panel number of layers number of layers per panel max trace space and so on all of these things look at this table they all have a weighting factor and that factor will determine what you're going to pay for that board very important to understand the impact these things have read this paper by happy you will learn a lot and we're going to talk about some of these items today pc board fabricators don't build boards they build panels of boards and they cut the boards out of the panel at the end so that you won't have the aggravation of having to do it the reality is until that very last step where they excise the boards from the panel everything is done in a panel what you pay for each board is a function of how many panels they have to run to build your lot of boards as an example if you order a hundred boards from a fabricator and they're able to fit 10 boards in a panel and they're able to to produce only 10 panels to produce your 100 boards because they're really confident they're not going to have any scrap then you'll get charged for 10 panels if they think that your board isn't that well designed and they need to make 10 extra 5 or 10 extra and they would just make 10 extra they wouldn't make 5 extra in that case they will run an extra panel they'll run 11 panels if your board or my board or whatever is so poorly designed that they need to run 12 panels because they're really not confident about the ability to build it without fallout without scrap then you're going to we're gonna pay for 12 panels nothing's free in this world the number of panels they run is what you will pay for the boards and they will divide the number of boards into the number of panels and that's where the price per board comes from and remember the weighting factor for each panel is a function of how well you do on the report card keep that in mind something that is common at every board house on planet earth is an 18 by 24 inch panel now it it's still thought of in most parts of the world as an 18 inch by 24 inch even though the lion's share of the world is metric because it started out that way and to this day they still produce material at laminate suppliers in three foot by four foot sheets when the when the fab house receives the laminate the three by four sheets they will cut it into four equally sized panels of 18 by 24 inches and they build boards in those 18 by 24 panels well what if you've got a small board and you don't need a whole panel they can build sub panels they'll build a half panel they'll build a 12 by 18 panel for example because that will still fit in all their machinery their machinery is sized in the early days not so much now but was sized in the early days for a maximum panel size of 18 by 24 and that's where this came from all the equipment they bought the drill machines the plating line the image line the etching line everything was sized around an 18 by 24 panel they can run smaller panels and often do they can even run a 9 by 12 if they need to really only build one or two medium-sized boards or several very small boards this is something they can do easily in the 1970s a bus style called the vme bus came along i was in the industrial controls world in the 1970s and the first half of the 80s and we put equipment on factory floors that was in large cabinets single and double bay cabinets and sometimes in pizza boxes but usually in larger cabinets and we would these cabinets would talk back and forth to each other and all the exchange of data that took place in the cabinets uh was done using a bus called the vme bus it was a very wide bus i don't remember if it was 64 128 or maybe even 256 bits but it was a wide bus really wide and the line cards that plugged into the back planes for the bme bus were a brilliantly sized circuit board the people that designed them really really really thought about their size and they knew that if they sized them correctly they would fit perfectly in a sub-panel of of of circuit board material and there'd be almost no scrap they made the circuit boards 14 between 14 and a half to 15 by somewhere around 16. they were ballpark in that vicinity that was roughly the size they were fabricators soon realized that if they cut a three by four foot sheet into six panels they would get 16 by 18 sub panels which they could also run on their 18 by 24 sized equipment and they would they could fit one vme board perfectly perfectly into that 16 by 18 panel with so little scrap that almost nothing got thrown away i mean this was brilliantly done unfortunately there was another company at the same time who designed a very a board that became very popular uh and a company called ibm i'm sure many of you have heard of these guys they're the ones who came out with the initial personal computer the first version of the pc was an xt design was called the xt computer and the motherboard for the xt was sized at 12 inches by 13.8 inches well i'm going to show you in a minute why this is true but that board size panelized terribly i mean terribly in everything that fabricators had that they could produce the closest they could get to getting reasonable production with the 12 by 13.8 motherboard was in the 16 by 18 panel that we're talking about well for the first few years the first few months to a year or so that the pc existed everybody who bought them whether it was ibm or the clone manufacturers that were making other versions of that same design anybody who bought a motherboard paid too much for the motherboard because they didn't panelize well in these panels and the majority of the material from the panel got tossed into the trash and you pay for what they use not for the board you buy you don't pay for a board based on its size you pay for a board based on how many panels they have to run to produce the number you request it's as simple as that it all comes down to what they have to use to make your design and ibm's motherboard was a terrible size and again we'll talk about why in a moment the only thing that was good in ibm's favor back then was the fact that at some point the pc took off i mean like a shot the pc took off and became such a popular item as everybody of course knows that they went from making a few hundred per week to a few hundred per day to a few thousand per day to a few tens of thousands per day and all of a sudden the people producing motherboards said you know there's a big market here and there's a real opportunity to make some big big money in this market but we're never going to be able to do it running 18 by 24 panels that just isn't going to work so they contacted the equipment suppliers and they said hey equipment suppliers can you make etching lines plating lines drill machines imaging equipment all this equipment can you make these lines and baths so that we can put larger than 18 by 24 panels in them can you make them so we can put panels of 21 by 24 18 by 26 21 by 26 and even other sizes beyond that these are just samples examples of sizes that fabricators requested and why did they do this so that they could cost effectively produce the xt motherboard and it wasn't just the motherboard there were plug-in boards there were periphery boards that plugged into the motherboard called originally called xt plug-ins and then eventually the a t and the a t plug-ins the a-t and x-t plug-in boards were approximately the same size as one another and they too did not panelize well in 18 by 24 or even 16 by 18 panels the word ibm the point i'm making is the ibm engineers either were clueless or naive or arrogant and i'm not sure which it was but when they chose the motherboard they clearly didn't do it with manufacturing in mind they were either so arrogant they didn't care and honestly believed they were going to rule the world and the world would change to meet them which is what happened by the way the world ended up changing to meet the demands of the pc market and eventually fabricators all over the world started producing other panel sizes the point i'm making here is simple you have a list of fabricators that your company uses they may be buying boards through their contract manufacturer they may be buying boards through your purchasing people directly however it's done you have a list of suppliers that you use and i can guarantee that your suppliers don't all use the same panel sizes they will use some of the panels that you see here and they might even use other panel sizes that aren't here before you design your next project you should find out all of the panels that all of your suppliers can can run can produce with and pick a panel size or panel sizes that is common to all of your suppliers so that you can pick board sizes and i'm going to tell you in a minute how to do this that panelize well for produce ability if you want to minimize cost and minimize scrap and minimize what you pay for boards don't choose the cheap vendor that's not the solution that's what purchasing does they choose the cheap vendor because they don't have the knowledge to do otherwise work with the fabricators get to know their processes and use panel sizes that all of your vendors can can build and design your boards to fit in those panels fabrication panel must accommodate these there are things that have to go in that panel besides the circuit boards they have to accommodate the boards themselves we just talked about that there have to be tooling holes in the panel the panels get drilled plated etched image these things all happen in different machines so they have to pick the panel up move it to another machine and when they put it down and align it up and line it up it better be nearly perfect the alignment better be within a few ten thousandths of an inch or good luck you're not going to get alignment of these processes so they have to have very tight accurate tooling holes in them to be able to move from station to station they need an outer perimeter area for thief copper beef copper i will explain thief copper in a short while and it'll make perfect sense but for now take my word for it they must have an outer edge of the panel with thief copper in it or they can't produce your board accurately understand that we'll explain why in a minute they need a routable area between the boards and based on these next two bullet items they also need to be able to put coupons in the board micro sectioning and etch coupons in the board as well as impedance coupons if you're doing impedance controlled design they don't test the impedance on the board itself they test it in the panel that contains the boards they look at micro sectioning coupons from the panel knowing that the boards themselves will pretty much match that micro section look and how well the holes are plated how well they're drilled how well things are imaged and etched and so on they can tell all of these things from the coupons we'll talk more about that as we go all of these things need to fit into that panel all with minimum scrap the less scrap you have the lower cost your boards will be and if you don't design them right you put yourself in harm's way when i first went to l3 avionics i'm sorry not l3 goodrich aerospace in 1990 i was talking to the mechanical engineer in the company and he said to me rick you're going to be working with me on an upcoming project called ttcast tactical collision avoidance uh anybody who's a pilot knows what that is we had landed a contract with the navy to equip x number of the navy's planes on a trial basis with t cast and wade the mechanical guy said to me he said we know where the equipment bay is in the aircraft we know how big our box is going to be and that equipment bait and based on the box size and the area we have inside we know that the circuit boards that are going to plug into the back plane can be anywhere from five to seven inches wide and can be anywhere from 11 to 13 inches long he said i recently found out that fabricators build 18 by 24 panels and so based on that i thought oh perfect let's pick a board size that maximizes yield in this 18 by 24 panel so i made the boards six by 12 to fit into this 18 by 24 panel well that's all fine and dandy except unfortunately what he wasn't aware of is you don't get the whole panel as i said a minute ago there are other things that have to go in the panel most of all there has to be a thief area around the edge i checked with the fabricators that goodrich was using at that time and i found out that all of them required three quarters of an inch band all the way around meant they were going to lose an inch and a half off of the 24 inch side and an inch and a half off of the 18 inch side so the usable area that was left was 16 and a half by 22 and a half and the circuit boards all had to fit into that area well unfortunately six by twelve inch boards can only fit a few boards into here he was hoping to get six boards per panel and that was his goal with this six by twelve but the sad reality is only three boards of that size would fit in that panel and it meant that a lot of the panel would be wasted all the material outside of the area those boards was going to get thrown in the scrap pile and they were going to charge us based on how many boards we bought and how many panels they had to run so if we bought 300 boards for example they'd have to run a hundred panels or more 100 100 100 and 205 depending on just how well we designed our boards and that's what they would charge us for these boards the time we were buying these we were buying fairly low quantities at the time because we were doing pilot production and early production runs and our we were paying about 150 per panel for six and eight layer boards that was our typical cost per panel in in these boards at that cost with three boards per panel they charged us fifty dollars aboard because they could only get three boards in a panel so i said to the mechanical guy if we could change the size of this board and just reduce it slightly would take take four tenths of an inch off the entire perimeter of the board reducing the size to 5.2 by 11.2 could we fit all the components in we checked with the double e's yes we could fit the components could we route stuff comfortably yes we could route stuff comfortably we could get the connectors to plug into the back plane we could get everything we needed into this board size and the beauty of this board size is it would allow us as you can see in the picture to put six boards in the space that we had available and not only would there be six boards in that space there would be area for thief copper around those boards again i will explain thief copper in a short while and the end result is that with six boards per panel that also left us pardon me room for coupons in the panel between the boards and a routable area between the pa the boards themselves and reduce the cost per board to 25 dollars a board the cost of the board was cut in half half by changing the the board size by four tenths of an inch all the way around eight tenths of an inch on each of the major dimensions the boards have still worked perfectly and we're half the price if ibm had actually thought about the motherboard and clearly they didn't and had made it instead of 12 by 13 8 had made it 11 by 15. the components that they put on that motherboard would have fit they could have routed the board and they still could have mounted that board into the case that they were planning they wouldn't even had to have changed the case size for the xt it would have fit in that case and their board their price per boards would have cut in half because now at 11 inches wide they could have put two 11 inches in that in that 22 inch of 22 and a half inch available space inside the thief copper and could have gotten two boards per panel instead of one their board would have been half the price now as it turned out ibm won anyway because they are so large and they made so many of these that the market changed to set to to meet them the industry changed to meet ibm instead of the other way around but had the pc only become a normal selling piece of equipment not a phenomenon it became a phenomenon as everybody knows but had it just been a normal piece of equipment where they were producing at most a few thousand a week i can tell you with clarity fab shops wouldn't have spent millions of dollars to re-equip themselves just to satisfy ibm's needs the only reason they did it is because they saw quantities large enough to justify it these things don't happen for the heck of it they happen because they need to so understand when you design unless you're an ibm size company and truly believe that your product is going to dominate the marketplace when you design it make sure you design it to fit into the processes that the fabricator uses into their panels and into their processes understand that also oh yeah don't forget about assembly rails if you push components all the way out to the edge of these panel of these boards the assembler still has to grip the edge of the board to produce it and if you've got components going all the way out to the edges they have no place to grip that means you have to attach quarter inch half inch three quarter inch whatever they demand assembly rails on the edge of this and all of a sudden you're no longer going to get six boards in the panel you're only going to get four boards of this size in the panel if you have to add assembly rails and the cost is going to go back up by 50 percent you have to know these things and think of these things when you're making the decision if you're doing very small boards as shown in this picture here you may the assembler or the cm if you whether they're your in your house or a contract company may ask you to put two or three or four or however many boards into an assembly panel and they'll give you the sizes that they like to use this is an assembly panel i've used before for small boards and a lot of the small boards that we did at l3 would fit nicely three up in this seven and a half by eight and a half assembly panel and the beauty of this guy is it would fit six up into an 18 by 24 panel with room between them to route them out and we would simply put v-grooves or mouse bites around the circuit boards inside the assembly panel and all this worked perfectly and as i said it fit perfectly in the 18 by 24 panel but rick you've got the panels the assembly panels extending into the thief copper area yes i do notice the pc boards themselves do not extend into the thief into the thief copper area the assembly pallet or assembly panel can have thief copper on it because it'll over plate thief copper over plates and you'll see why in a short while it can over plate and have a thief copper on it because it's going to get torn off and thrown away so when you have to build things into assembly pallets you can do this but don't let your board extend into the thief area understand the processes work with the fabricators let's go through quickly how circuit boards are produced talk a little bit about how a four layer board is manufactured when you send a artwork to a four-layer board shop they're going to start with a center core of material there a lot of people think they will take two cores print match and laminate them together that's not how it works if you want to do it cost effectively they will do what's called foil lamination and to do that they will start with this center core that you see in this slide and the center core will be fully polymerized cured to the c stage meaning that it will never go to a liquid state when you put it under high temperature and high pressure in a laminate press it's fully polymerized and on either side of it is a sheet of copper foil and also one thing to notice about this particular picture it is inaccurate in the sense that when you're building a four layer board that center core will actually be about 25 times thicker than either of the sheets of copper above and below it this is just a drawing and the guy who drew it dan the guy who drew it drew it just to get the point across how boards are fabricated his intent wasn't to accurately depict the process and a four layer board that center dielectric will be much thicker than the copper but this is what they will start with the next step that they will do is to place what's called an etch resist on the surface it's typically a blue plastic material like you see in this upper left picture on the slide they add that to the thing after they have imaged and removed they will remove the etch resist in the areas where they want to remove copper they then put it into an and they they put it into an etching tank and that etches away the copper in the open areas of the estrouses they then strip away the blue material and when they're done they get what you see in the lower right picture here they get that center core with all of the copper printed and etched and they will then neutralize the acid from the etch they'll do a thorough cleaning they'll do a di water rinse as well as other steps and then they do what's called a treatment an oxide or film treatment to the copper surface why do they give it a treatment because they need to form a tooth a small tooth they need for it to have a little bit of a jagged edge across that entire surface of copper why so that the material we're going to laminate to it will adhere well if this copper is too smooth the material we add to it won't adhere well after this is done they will lay it up as shown in slide 12 in a laminate press along with plies of prepreg material and they'll put a sheet of copper foil above and below all of that what is preprint prepreg is the same material as that which is in the center of the core except it has not been fully cured or fully polymerized it's only been cured to the b stage meaning when you put it in a laminate press under heat and pressure it'll go to a high viscosity liquid state it'll go to a syrupy state where it'll flow like a thick liquid and the idea is to fill in all the valleys where we've removed copper on the center core and at the same time have that prepreg adhere to the sheets of copper foil that we put on top and bottom of the stack up they put it in the press pressure temperature for a given amount of time over time the prepreg cures to the sea stage at which time the core is fully cured i mean sorry the entire stack has been fully cured and we now have what you see in slide 13 in the upper left we have a fully completely cured four layer stack up with all of the inner layer copper printed and etched the next thing they do as already seen in this picture is they drill holes wait a minute rick they drill holes before they image the traces and pads absolutely the next thing they do is drill the holes they also will do what's called smear removal of in these holes when you push a drill bit down through this circuit board and it encounters the epoxy and fiberglass the fiberglass is really really tough stuff and it heats up the drill bit these are diamond tip drill bits but they still heat up from the friction caused by the the fiberglass the drobik gets hot as it pushes through the epoxy it melts some of it and when you pull the drill bit back out it pulls epoxy along the whole wall and creates a smear as it's called along that whole wall if we attempted to plate the holes in the board at this point in time the plating would not stick to the inner layers because there is an insulator covering those insert later in inner layers the epoxy smear so the next thing they have to do is what's called a d smear or etch back process where they attack that smear with an aggressive chemical to eat that smear out of the hole now once that has been done they then add as you can see in the bottom right a thin copper thin layer of copper it's chemically deposited on the walls of the holes in this panel now the cot this thin copper layer also gets added to the surface copper they don't really care about that they don't need it on the surface copper but it doesn't matter that it gets added there as well where they really need it is in the holes why because they need the surfaces and the whole wall to be fully conductive so they can electroplate the copper in the whole wall you can't electroplate unless you have a conductive surface and that's why they make this conductive so that they can have a fully conductive surface all over and through the holes sometimes they use what's called a carbon deposition whether they're using electrolysis or carbon either way this deposited material is only a few microns thick a micron is uh is a thousandth of a of a mil it's a it's a millionth of a meter i couldn't think of the right way to say it it's a millionth of a meter so it's a really thin a thousandth of an inch is 25 microns to give you another perspective what the people in the u.s refer to as a mill a thousandth of an inch is 25 microns this material is only a few microns thick very very thin material in the old days before the days of what's called i'll think of it in a minute in the days gone by they used to do what's called always called pattern plating pattern plating is what we do today to plate the the extra copper on the board back in back in time in the early days of fabrication they would do what's called panel plating they would take this panel just as you see it in this lower right picture and they would put it into a plating tank as shown on slide 14 in the upper left now this is a cartoon that i got off the internet just to show how electroplating works i didn't want to show a circuit board house plating tank i wanted you to really understand the process not what the plating tank looks like imagine that this circular object is the panel that we just put electroless copper onto if they put that into this tank and attach the negative electrode from a power supply to it a dc power supply and attached the positive side of the of the power supply to a copper anode that's in the plating bath and they had a copper sulfate solution in the plating bath as current i should say as energy moved from the anode to the cathode the cathode is now our circuit board panel as energy moved from the anode to the cathode cathode through the plating bath it would carry copper in the solution to the uh to the panel in that we're trying to plate and over time we would plate copper all over that panel and that's how it used to be done that's called panel plating and i'll tell you in a few minutes why they don't do that anymore they now do what's called pattern plating and i'll explain pattern plating in just one second but anyway this is how electroplating works the fields move through that bath evenly from the anode to that they're they're attracted by that entire 18 by 24 panel they're attracted to that entire panel and copper wants to plate evenly all over that panel and again we'll talk about why in a minute today they do what's called pattern plating as shown in this lower right image on slide 14. they will put a material on that panel that we have just put electroless copper in the holes they'll put a material called a plating resist why because they don't want copper to plate everywhere if you plate copper everywhere then you have to etch through the base copper and the plated copper when you want to etch traces and pads unfortunately we make images today that are so small it's hard to plate through copper that thick and still be able to produce narrow traces and that's why they don't panel plate anymore they now pattern plate so they put this plating resist material on and they then drop it into the plating tank as you see in the upper left picture and if our circuit board imagine our circuit board looked like the right side image on on slide 15 as you can see it here if i designed a circuit board like this and sent it to a fab house the fab house would immediately call me up and they would say recruit correct what are you thinking we can't build this board and i would say naively why can't you build this board and they would say because this board has uneven copper all over it we can't plate it evenly because you haven't distributed copper evenly remember we're going to put let's say six or eight of these into an eighteen by twenty four panel let's say we're going to put eight of them in a panel when they draw that drop that panel into that plating tank we just looked at the fields from the copper anode conducting to the panel are going to attempt to couple evenly all over this entire panel why because there's copper underneath the plating resist imagine that this black material is plating resist and the and underneath that is a solid sheet of copper and the fields will be attracted all over this panel to that solid sheet of copper so the fields are trying to plate copper evenly all over this panel but unfortunately when the energy gets to the panel we don't have an even distribution of copper and what would happen if they tried to build this board as you see it the upper area would tremendously under plate because the amount of energy coupling to it would get spread out across a lot of copper and the bottom area where there's only a few copper features the energy and the the solution that would be carried to that area would only be spread out over a very few features the bottom would tremendously over plate lines would over plate holes would over plate and if we left it like this we would probably also end up with holes that were shaped like ice cream cones they wouldn't be cylinders like we want they would be conical in shape conical shaped holes have uneven knees and uneven knees have a are too thick on one side and too thin on the other and other and they're prone to failure this kind of board would be extremely prone to failure and would cause major reliability problems so they're going to call me up and they're going to say rick we can't produce this board what are you thinking man and i'm going to say to them what do you need to do to produce it and they're going to say well we need to to even out the copper on this board oh how you going to do that and they would say to me we're going to put thief copper on this board so that we can create even copper plating all over this board oh so what are you going to do we're going to put thief dots in the area where you only have a few traces we're going to fill that area up with dots of copper and most people say to them yeah that's okay go ahead and do that you know what's wrong with that those thief dots will attract fields oh rick they aren't attached to anything they won't attract fields want to bet you do not have to have something attached to you do not have to have copper attached to anything for the fields in the dielectric to be attached to be attracted to them the energy in a circuit moves in the fields not in the voltage and current and when the fields move through the dielectric below those thief dots they will couple energy into those thief dots as seen in this picture if you had thief dots in this board the fields in the in the dielectric under it would would create current flow in those thief dots and that would in turn create a magnetic field and the fields would then potentially couple into other circuits on the board is that what you want to happen to have unattached copper coupling fields into places where you don't want them well of course not so when they call you and say hey we need thief cop or you say no i'll fix the problem don't let them fix the problem you fix the problem trust me when i tell you they could not build this board unless someone fixed the problem either they're going to have to add thief copper or i'm going to have to do something else to the design because as you see it they cannot produce it properly can't be done so it's up to me in this case to fix this problem what i should do is add copper pour all over the bottom area of this board the under the bottom half of it and attach it to something to ground to power to something so that the copper is balanced so the copper will plate evenly in and on the board and you need for it to be balanced on both the top and bottom of the board not just all over each surface copper needs to be balanced all over the outer surfaces and not only the outer surfaces unless you want your circuit boards to be to be warped and twisted and look like a potato chip you need copper evenly distributed all over the inner surfaces you should be adding copper port to every surface of your boards and if you want to know how to attach them properly attend one of lee richie's classes on power delivery or attend one of mine on power delivery and we'll tell you how to properly attach that copper so that it does its job as it's supposed to a lot of people think pouring copper on the surface of a board is an automatic cure for emi not true it may help but it may not you have to attach it to the right voltage or ground depending on the other layer so the point is know what you're doing pour copper all over the board and attach it to something don't leave it uneven and oh by the way the reason they need thief copper around the outer perimeter imagine the top edge of this board is one of the boards at the outer edge of the panel if there was no thief copper outside of these boards the entire edge of that board about a half inch in would over plate because again the fields are drawn to that area and they need to have even plating they put thief copper there so the thief copper will over plate because they're going to throw it away they don't care if the thief copper overplates they don't want your board to overplay that's why they need thief copper on the outer edge of the panel design the board so it's balanced anyway getting back to this picture they have added plating resist and we've got a balanced panel right because you've put copper everywhere or in this case i've put copper everywhere to balance the board so they then put it into a plating tank and they will end up with the board as you see it in this lower right image on slide 16 they will end up with a board that has plating on all the outer layer features and in the hole and in the hole that's the key here they have plating both on the surface and in the hole and that's the secret to success in this particular case after that they will as shown on slide 17 put a thin layer of tin and or tin lead on the plated copper i don't want inlet on my board they're not going to leave it there they're putting it there for a reason they will then strip away the plating resist that they had on the board leaving what you see in the lower right picture on slide 17 and they would then put it into an etching tank and etch away all the copper except the copper that's underneath the 10 or 10 lead oh that's the reason for the 10 or 10 lead it's a it's an etch resist exactly that's why they put it on there some fabricators don't use 10 or 10 lead they use something else the point is they put something on there as an edge resist and then as shown in the bottom right of slide 18 they strip off the edge resist they're sorry the etch resist and they now have a fully finished board other than the few final finishes that go on it as shown in the upper left of slide 19 they would add a solder mask to the board if you're doing solder mask over bare copper and then as shown in the lower right of slide 18 19 they would then finish put some kind of finish on the features that show in the board electroless nickel immersion gold which is enoch and oh by the way i think i might have mentioned this talking about happy's report card unless you need eating on a board because of re needing really flat pads you shouldn't be using it it's one of the most expensive finishes there is if you only have medium density surface mount components meaning medium if you don't need really really flat pads because of very fine pitch parts you don't need any use something like immersion 10 or immersion silver or maybe even an osp finish which is an organic finish only use enig if your assembler tells you yes you absolutely need it because it's more expensive it will add cost anyway final finish and then the board is completely done i mentioned coupons in the circuit board itself imagine if you will it as shown in slide 20 that they in that coupon area of the panel used once they had extracted the boards they're going to route all the boards out of the panel and now they've got the leftover panel material they will take the area where they put the coupons and they will cut out a coupon like you see in the upper picture on slide 20 and they will then cut through the center of the holes with a very sharp saw so they don't create burrs on the copper they will then uh clean that very well and buff it and then put it in a dish and fill the dish with epoxy let the epoxy fully cure then they take that round slug out of the dish and those holes are now up against one edge they buff that edge where the holes are until it is smoother than a baby's bottom i mean they they they buff this thing until it is just perfect and they then put it under a microscope and look at it with at 100 or 200x magnification as shown in the picture on the right side of slide 20. what you see in that is that cross-section of a hole they can tell so much from this coupon it is unbelievable they can tell just how well the hole was drilled if the drills were dull how can they tell if it was dull one they're going to get tearing of the fiberglass at the edge of the hole and two notice the inner layer copper where it comes up to the edge of the hole notice that that copper has a little bit of a look of a nail head it's got an elongation to it right at the edge that makes it look a little bit like a nail head that's called nail heading and when they see nail heading start to become extreme they know aha our drill bits are dull or becoming dull and need to be taken out and sharpened or replaced if they've been sharpened more than a few times they will only sharpen drill bits so many times and then they pitch them because they can only do so many sharpenings before the drill bit becomes useless drill bits are very expensive one of the most expensive operations in a fab house and if you're going to fab houses that charge you a low price there's a good probability that they're pushing their drill bit beyond normal usable life i could tell you stories for days about that i mean i have so many stories about doll drills and failed equipment in the field because because our company bought boards from from the cheapest vendor i could tell you stories forever about doll drill bits know what you were getting by the way every fabricator will put coupons in the panel tell them you want these coupons shipped to you and you want evidence that the coupon came out of the panel that made your boards don't let them send you someone else's coupon make sure they're your coupons you want certified proof that that's a coupon from the panel that made your boards because you want to look at them you can tell if they've pushed real life you can tell if they haven't done an adequate job of d smear you can tell if plating is even and if it's the right thickness plating on the whole wall should be between eight tenths of a mil to one point four mils ideally it should be 1 to 1.2 mils on the whole wall and that has to do with long-term reliability i'm not going to get into that now it's all in the ipc standards that's what they will build to because that's what you need to design understand these things ask for the coupons examine them utilize their benefit anyway they can tell so much from these coupons it's remarkable learn that if you don't know these things do your own studying figure out the advantages and the value of coupons and then request the coupons and look at them yourself etching will reduce traces on outer layers on inner layers sorry by about a mil and a half when you're using one ounce copper which means what which means they're going to take your artwork if you're asking for a four mil trace and and it's one ounce copper they're going to increase that trace to five and a half mils if it's on an inner layer so when they etch it'll etch back to four mils oh shouldn't i be doing that we'll talk about that in a minute on outer layers it's going to reduce the copper on the edges by a mill on each side or about two mils overall so a four mil trace will get widened to six mils what does that mean that means if you're asking for traces that are too close together like two mil lines with two mil spaces there's a high likelihood they can't produce them and oh by the way if you're asking for two mil lines in two mil spaces on a four or six layer board on the outer layers there's a high high probability they can't produce them at all without changing copper weights and if they have to go to a really thin base copper weight to be able to produce your two mil lines on the outer layers of that four or six mil uh six layer board you will pay extra for that that's a special order they're not going to be using standard materials which means uh oh they can't build what you've asked without a special build and you will pay extra for it the point is don't put two mil lines in spaces or even three mil lines and spaces on the outer layers of four and two four and six layer boards when they're using standard copper weights because they can't produce it effectively know what can be done talk to the fabricator drink in their knowledge ask them the questions what can you do and what can't you do can i do this can i do that we're going to talk more about that in a minute multi-layer pressing will cause what's called resin gathering in areas where there aren't a lot of traces it's cause and those areas are called resin rich areas resin has a dielectric constant of about three and and and fiberglass has a dielectric constant of about six so when you get a lot of resin in an area that will lower the dielectric constant for the traces in that area by as much as a half a point well what does that do when you change the dielectric constant that traces c it will it will in this case you're lowering the dk it will raise the impedance what yes it will raise the impedance of the traces well shouldn't i compensate for that no don't ever as this bottom note says on this slide don't ever compensate for the fabricator's needs make sure you design so they can produce your board don't put two mil lines and spaces on the outer layers of two four and six layer boards unless you're prepared to pay a lot more for them because that's not producible know what they can and can't produce and design around their absolute needs and then send them the design and leave them alone i have worked with an engineer once in a major company who loved making lines bigger so that we could compensate for etch factors oh my god it took me forever to drive into this guy's head we don't want to do this we want to leave the fabricators alone and let them do their job they know what they're doing don't don't camper in there in their in their field stay out of their business let them do their job never ask a fabricator what is the smallest hole or trace or space or feature that you can make i mean you want to know that but don't ask that only what you should ask instead is what's the smallest hole or line that you can make without a cost adder ask them if i make 10 inch wide lines and quarter inch diameter holes and i start reducing those holes in diameter and start making those those 10 inch lines narrower at what point is the price going to go up and by the way they're going to give you different numbers for different types of boards they'll give you different numbers on inner layers than outer layers they'll give you different numbers on two four and six layer boards than they will on 8 10 12 and so on layer boards going up because they'll use different copper weights oh i see yes where is there a break point and then you ask the next question if i keep making them smaller still where's the next plateau once you know these plateau levels stay above them as much as you can once you know the maximum trace width or the minimum trace width they can produce at virtually no cost adder make your traces that wide when you can i mean if you have a controlled impedance and can't do it well then you can't do it but if you're not doing controlled impedance work make your traces that wide if you have room for it i've met people who will put four and five mil lines on circuit boards where they only have 20 or 30 traces think about the images that were on that that picture that i that i showed you when we were talking about plating the image from euro circuits back on i forget which slide it was think about that image how uneven that copper was one of the things the designer could have done is make the traces much wider in the area where there was no copper pore why not think about it people don't think about i've seen people put four mil traces when they only have 20 or 30 traces on the surface on a surface of a board what are they thinking again if it's impedance controlled yes then you have to but if it's not don't do that once you know the answer never go below that width unless you have to and when you have to minimize the usage this last bullet item on slide 22 shows an example of the last time i asked a fabricator and it's been a while so the numbers may be different now the last time i asked what's the minimum trace you can produce without a cost adder they said six mil lines and what's the minimum hole size print a plated hole that you can produce without a cost adder they said 13 mils finished whole or larger talk to your fabricator ask those questions don't assume and go above those sizes when you can make their job as easy as possible if you have to have two mil lines in the area of a .65 millimeter pitch bga so that you can get some of the lines out of the pin field then use them but only use them there don't use them everywhere understand the impact you have on design talking about slide 23 for a minute things you need to know or things you need to ask what are the what ipc class are you designing to well what is ipc class by the ipc standards and you'll know it's a produce ability level if you're building toys or appliances you're probably ipc class one which is a very producible class it's easy to produce class one because their their potential failure isn't isn't oh my god if it fails if you're building medical equipment that absolutely can't fail or military equipment that absolutely cannot fail fail-safe equipment then it might be class three if you're almost anything else in the world you're probably class two when i was at l3 we designed and built avionics equipment some of our av avionics equipment was for the military and some of that was class three the majority of what we produced including some of the military gear was class two meaning it could fail without the the world falling apart because there were backups within the equipment or backup equipment to take over for it should it fail most equipment in the world is class two if you're going to design to class two don't ask them to build to class three and don't pay for cla don't design the class three and then only ask them to build the class too because you'll be over designing the board you'll be doing more than you have to and you'll be you'll be just constraining yourself unnecessarily understand the needs designed around them what are the pad to hold ratios that your fabricator can live with what's the whole this is a very important one we talked about it earlier hole to board thickness aspect ratio what is the board to hold the board thickness ratio they can live with and where does a premium start to kick in and where does it get so small they can no longer do it you need to know all of those numbers and live within the numbers what's the minimum line width what's the minimum space feature spacing what's the plane to hole clearance ah if you have power and ground planes in the board and put an anti-pad an open hole in the plane that you're going to have your drilled holes go through what is the minimum clearance from the edge of that hole to the plane it's probably going to be bigger than you think talk to the fabricators i mean if you're doing for example 10 mil plated holes in a 62 mil thick board um they probably had to drill a 12 to 13 mil hole before plating and they probably need eight mils all the way around in the ante pad so that's 16 mils plus 13 they need a 29 mil diameter anti-pad in the plane for that 10 mil uh drilled and plated hole what very likely again i may be living in the past maybe eight mills is bigger than they need the point is ask the question you have to know you can't assume that what you're doing it is producible think about it do they silk screen do they need solder mask you know what text size do they need minimum for silk screen in case you're forced to use really small characters and letters know what the what the art of the possible is live within their needs when doing two and a half and three mil lines i mentioned this a moment ago only use them where you need and make sure that you can only you only put them on outer layers if you're willing to pay an extra cost for low layer count boards you can put them on outer layers of high layer count boards because they're going to use thinner copper anyway but if they're forced to go to quarter ounce copper instead of half ounce copper on your 8 10 12 layer board then you're still going to pay a premium whenever you do these things you probably incur a premium know that understand that live with it minimize the use of these features when routing never space two and a half and three mil lines apart by two and a half to three mils because remember they have to make it wider to etch it back and if they get the two mil lines say let's make let's say they make them three mils wide in order to produce them and you've got them separated by two mills you have so little area between them they can't put a plating resist between them without it flaking off which means you're going to get shorts between those two mill lines no recognize the needs that they have to have and live with them when a pcb is uh is uh two four or six layers utilizing standard copper weight do not use two and a half to three mil lines understand the needs always use the widest line that the design allows when you have imbalanced copper like in this design fill that area in with something don't leave it open either make the lines wider or fill it in with copper fill of some kind don't allow unattached copper in that area we talked about that earlier use the largest via hole that spacing allows good design rules for vias only use vn pad when nothing else will do it makes a repair and assembly harder so do it only when you need to only use blind or buried hdi vias when you have no other choice because of feature size or pin pitch of bgas or whatever or when it can reduce cost if you're doing 40 and 50 layer boards as some people do you may be able to actually lower cost by going to hdi look into it understand the needs the wants and so on non-filled vias need an opening around the vehicle not around the pad just around the hole why because if you try to put solder mask over a non-filled hole and you're using lpi mask the mask material will collapse into the hole and when the mask is cured you will trap chemicals in that hole that can potentially cause board failure over time understand the impact that you have on the design be as properly sized can be can be assembly test points we used to use vias and on certain areas of the board where we had room we would make the pad on one side of the board or the other a 35 or 40 mil square pad with a nice big opening solder mask opening around the pad we did that so we had test points for vias i mean if you've got a via there anyway make it a test point if it's in an open area of the board why not we did this a lot 100 test point coverage on circuit boards is absolutely mandatory if you expect them to be able to ship you boards that they can guarantee will come up every time you fire them up if you can't give 100 test coverage they can't guarantee that they're going to be able to supply you boards that work perfectly every time assemblers need full coverage to do full in circuit testing we used to spend weeks after prototyping putting test points in really high density boards at l3 because we knew that before we shipped that thing for final final production runs that we needed to have a hundred percent test point coverage if you can't do that well i'm sorry you can't be guaranteed it's gonna function is it costly oh man is it costly to design those in do you want them to be producible or not you have to decide um hdi micro via technology should only be applied when you can do it cost effectively this is a cost effective this picture on slide 27 is a cost effective hdi design because they're going to build a thin four layer board print plate etch everything just like they would any other four layer then they'll add a layer of laminate top and bottom they'll ablate the veal wells and then they'll plate all the copper on the surfaces and in those vias after everything has been ablated this is an inexpensive way to do this if as the bottom note on this slide says if you have to add through vias after you put the blind after you put the hdiv is on that's going to add cost that will make it more expensive try to use all hdi vias from layer 1 to 2 and have all your through vias from layer 2 to in this case layer uh five so that you don't have to pay extra for through drilled vehicles when you this is something on sla on this next slide 28 that we did at el or at goodrich aerospace in the early 90s with a lot of our rf circuits we would do blind depth drilling from layer one to two and from the bottom layer up to the next layer above where when so that when we drilled all the through vias they could do blind depth drilling to the blind vias and then they would wash plating solution into these via wells at the same time they plated the through holes and this worked extremely well this gave us very good process control uh and very inexpensively there was almost no cost adder to do this versus a standard through-hole board when you have to use hdi via this next slide shown on slide 29 is a perfect example of what not to do i mean if you're going to drill the center core and then plate an etch that's a plate and and and plate etch and plate that center core and then turn around and add two layers of via material to do two different uh blind berry via layers and then put through holes on top of it into this oh man are you asking for an expensive board this will be the fact that you can connect any layer to any other layer doesn't mean you should having drilled holes after the hdi build up layers really adds cost as noted in the bottom bullet item on this slide this is an expensive board don't go there unless you must this is what people used to do in the days of blind and buried vias before there were hdi or blind depth drilling this is called sequential lamination they would build for example if you needed an eight layer board they build a thin four layer center core and they do all the printing plating etching blah blah just like any other four layer board they would also make two fully built two layer boards with plated holes one for the top and one for the bottom so far they've made three circuit boards then they'll laminate these together and then drill the through holes all the way through all of these layers and plate all of that you can only imagine what this cost and there are people today still doing this this is called sequential lamination it's a very expensive way to produce a bare circuit board and there are people today still doing this avoid it if unless you absolutely must this is very reliable and there are some military suppliers that still do this but don't do it unless you really need to get to know the the some the person in your fab shop that knows all the processes get to know the person who knows all these bullet items talked about here impedance control some knowledge of electronics artwork layout mechanical processes chemical processes testing test coupons talk to the person in it's probably someone in engineering that understands these processes well get to know the person uh in that that knows the fab processes and the impact they have on panel sizes that your fabricator will use their preferred structure for each board stack up the impact of copper balance on plating and warp and twist aspect ratios land to hole minimum no cost adder alignments you need to know answers to all these questions you need to know the person at the fabricator that can answer these questions for you talking about assemblies for just a minute get to know the person at the assembly shop the cm who can it can tell you how to best process your board try to figure out ways to have one ir reflow process if possible two ir reflows means it's going to cost more and you're going to subject the board to more heat when you subject the board to more heat you're going to be challenging the long-term reliability of the board because you're stressing it more than you absolutely need to if you suddenly realize oh we not only to need two ir reflow processes we need to expose to wave solder reef processing because we have through hole components in the board now you've exposed it to three heating processes and you've exposed some of the components to more than one heating process which means you're going to shorten their life the this slide on this this bullet list on slide 33 comes from happy's paper take a hard look at it read happy's paper go to altim's website download this paper it has all of these bullet items in it and talks about their importance and how what you need to know about them this picture on slide 34 and the one on slide 35 are also in happy's paper get to know all of this stuff and get to know it well and get to know the impact you have on fab and on assembly and know the breakdown that you will create at the fabin assembly house and the cost impact that you have you need to know those processes inside out if you don't you're you're compromising the overall quality of your circuit boards if you don't know these processes inside now know them respect them know what to do to minimize thermal stresses at the assembler stresses on components fab processes all of these things know how to design to minimize those effects thank you so much for your [Music] time

Channel: Altium Academy

Views: 17,393

Keywords:

Id: 0RyBCnowLsI

Length: 86min 6sec (5166 seconds)

Published: Fri Oct 30 2020