EEVblog Electronics Community Forum
Electronics => Manufacturing & Assembly => Topic started by: mrpackethead on September 24, 2018, 06:40:16 am
-
Whats your top tips for designing PCB's that are manufacturable?? or improve cost and reduce faults.
-
(1) Spend lots of time on reviewing solder stencil apertures. Really take the time to understand how they should be set up.
(2) Reduce the BOM as much as you practically can.
(3) Double sided placement is somethign you really want to do for a good reason. If you can fit it on one side do that. Even if it requires some extra board space. (4) A 4 layer board might end up signifincatly smaller than a 2 layer, and end up being cheaper.
-
I have the luxury of a full automated DFM service at the local shop I work for. :) Good for checking footprints, primarily.
Tim
-
Keep in mind stress on ceramic caps.
Do not put ceramic caps near the edge of the board;
Do not put ceramic caps near screw holes;
Do not put ceramic caps next to wire screw contacts;
Do not put ceramic caps in the preferred flexing direction of the board (happens with long thin boards);
The list continues...
Rule of thumb: Keep some very well made boards (a couple of Motherboards/embedded boards, some PCBs from an LCD TV, something from a smartphone, something industrial, etc.) on your desk and periodically check if your board looks like them. If you see major differences, you are probably screwing something up. :-D
-
Any traces under SMD resistors/capacitors should be dead center. Same goes for any traces between pins on SO-8-14-16... packages. (You wouldn't believe how many designs I see where you have a trace hugging one of the 2 pads to the minimum spacing manufacturing rule...)
Keep vias drill hole to either board manufacturer's recommended hole size, or larger by at least 1 full mil, keep extra angular ring around the vias. If you do not need a test point, tent the vias.
Space out traces to 8 mil spacing at least unless you really need the occasional compact point, or are paying for a high spec PCB.
Keep everything away from the edge of the PCB and do not fill planes of place traces, except for an optional single ground trace, under or inside mid layer around mounting screws.
Run multiple parallel vias when feeding high current power traces.
-
For SMT:
Put fiducials on your PCB, do not place them symmetrically and keep them at least 5mm away from the edges (conveyors and fixtures cover at least 3mm of the board).
If you panelise it, put a border on the panel, put fiducials on that too.
Fiducials are not defined using silkscreen or soldermask.
Define fiducials as components so their locations are automatically included in the pick and place file.
Make any individual panel over 50mmx50mm (which is still pretty small).
If you have connectors that overhang the board rout out underneath the overhang in the panel border so the border can be safely removed without breaking the connector.
Weird and wonderful connectors often need special tooling, or a harder to source specific part number with a pick assist tape/clip, don't use them just for the sake of it.
Surface mount is a != cheaper, sometimes it is both mechanically better and cheaper to use a conventional PTH part, at least until you get to high volumes where this might change the economics.
Thermally balance the copper traces to your components if you have a tiny trace to one end and a huge trace to the other you risk tombstoning or jauntiness.
If you follow current IPC & guidelines for footprints you should be fine when it comes to creating your stencil layer. Be sure to break up large pasted areas into smaller ones however - this is usually covered in the datasheet.
Read your datasheets! For some devices (QFNs seem to be the primary suspect) the package might not match the one you have in your CAD library even tho' it might seem the same at first glance. The center pad might be bigger/smaller and the outer pads might be shorter/longer.
For PTH:
Check your apertures and pad sizes.
Keep things away from the edges if it needs wave soldering.
In general:
If your board is an odd shape put it in a square panel with routing and scoring as appropriate, don't leave huge gaping holes in the panel, particularly if that PCB needs to go through wave solder later - keep it nice and rigid.
If you can avoid a custom cable, do so.
At scale some of these rules change, special tooling will remove some DFM requirements and introduce others - work with your manufacturer.
Thermally balance your board: top and bottom should have similar copper coverage, if one has way more than the other, your board WILL warp. That can cause stress on the components as well as being a pain to handle and looking bad.
Specify parts that exist, there is no point asking for a 1uF NPO 0805 100V capacitor just because the datasheet has suggested NPO is better.
If assembly looks fiddly, it will cost you more and increase the risk of build errors, costly rework and maybe even damage.
-
Not mentioned yet (oddly...): make sure the parts in your BOM are not unobtanium.
Digikey and/or Farnell are not the Holy Grail but if they don't stock it there's a decent chance it should not be on your board.
-
Not mentioned yet (oddly...): make sure the parts in your BOM are not unobtanium.
Digikey and/or Farnell are not the Holy Grail but if they don't stock it there's a decent chance it should not be on your board.
In a similar vein, avoid single source, where possible all your parts should have available generic alternatives (or at least multiple vendors) that fit in the same footprint.
-
Not mentioned yet (oddly...): make sure the parts in your BOM are not unobtanium.
Recently most of stuff is turning into unobtanium...
My tip:
make sure the circuit can tolerate (not necessarily function at) input voltage in the entire range from zero to the intended voltage level. I.e. if the board is normally powered by 24V, you should be able to safely apply any voltage in 0-24V range for prolonged time without entering any unstable states, erratic or undefined behavior. Helps with testing production units.
-
1. keep in mind that parts are three-dimensional and think about how the board is going to be assembled to make sure you can reach all pads with multimeter and soldering iron. Learnt this one when I had a short on some pads of a QFN which I couldn't reach with my iron without touching other parts, so I had to take these parts off first. Utilize 3D view capabilities of whatever eCAD you use for that.
2. when you place connectors along the perimeter of the board remember that in many cases connecting cable is wider than the actual connector. Otherwise you might not be able to connect all cables at the same time if you place several connectors too close to each other.
-
Maybe using multiple nested footprints so a shortage won't stump you?
-
Any traces under SMD resistors/capacitors should be dead center.
If you have a leeway to put a trace under them, either those are large components or your footprint is crap prone to tombstoning. EDIT: or your PCB is expensive to produce.
Example of crappy footprint many people make v. Unless adhesive is placed under component, such a large gap should be avoided.
(http://store.curiousinventor.com/media/catalog/product/1/2/1206_done.jpg?scale.width=56)
-
My top tip is to assemble your own designs.
I have learned a lot from my own bad ideas leading to various manufacturing challenges.
-
Any traces under SMD resistors/capacitors should be dead center.
If you have a leeway to put a trace under them, either those are large components or your footprint is crap prone to tombstoning. EDIT: or your PCB is expensive to produce.
Example of crappy footprint many people make v. Unless adhesive is placed under component, such a large gap should be avoided.
(http://store.curiousinventor.com/media/catalog/product/1/2/1206_done.jpg?scale.width=56)
Although taking that too far is equally bad. If you can't route at least a thin trace under an 0805 or larger, your rules are wrong. That's one pet peeve of the aforementioned DFM tool I use: it contains a SM-782 land pad gap maximum check. Which is superseded by 7351, and the DFM guys know it. They just leave it in as information. So, even a full enterprise tool like this, you cannot follow blindly, you must use good judgement, as is always the case.
Just as well, tombstoning isn't a risk on 0805s and up. It is a moderate risk on 0603, and a serious risk below there, and you probably won't get a trace between pads on those sizes.
Tim
-
Although taking that too far is equally bad. If you can't route at least a thin trace under an 0805 or larger, your rules are wrong.
0805 is what I consider on a large side. But I would not suggest routing under 0603. BTW 0805 tombstones quite easily. Different thermal mass on the pads and components like ferrite beats, and here you go. I had an issue with certain 0805 ferrite bead on certain PCB (it's fine on another PCB with the same footprint), simply switched to ferrite bead from different supplier and it became fine.
-
make sure the circuit can tolerate (not necessarily function at) input voltage in the entire range from zero to the intended voltage level. I.e. if the board is normally powered by 24V, you should be able to safely apply any voltage in 0-24V range for prolonged time without entering any unstable states, erratic or undefined behavior. Helps with testing production units.
Ideally nothing should be damaged by short overvoltage at a few volts over too.
Also consider what happens if polarity is reversed. Not always important, but sometimes it's cheap enough to add a diode or other protection even if it shouldn't matter.
-
>Put fiducials on your PCB, do not place them symmetrically and keep them at least 5mm away from the edges (conveyors and fixtures cover at least 3mm of the >board).
the symmetric bit is important. If you accidently load a panel into your Machine around the wrong way, or even upside down it is good if the machine cant' find the fiducial, and errors out. My yamaha's will give or take look in the general area +/- about 2mm to find the fid.. Its good to put fids on both individual PCB's and the panel itself. Some of how this shoudl be done will be dependant a little bit on how your PNP system is se tup. I use 2mm Fids on my panels, and 1mm round fids on my PCB, and have a decent amount (.5mm ) of solder mask pull back on them to make sure its easy to find. You can also set up bad block fids as well. Again, this is all stuff that you will never learn in a book.. Ask your PNP contractor or ifyou are doing it yourself, figure it out.
>If you panelise it, put a border on the panel, put fiducials on that too.
Other thigns worth doign. Fids for paste stencils, On the tooling strips ( yes, please use a tooling strip so you dont' have parts hard up against the rails ). Do useful thigns like text that says.. " TOP SIDE " / " THIS SIDE TO FRONT" Very helpful as you load into the line. Even consider using Big Arrows etc. Make it easy for operators. On My Yamaha line, to make it easy , i have an alignment hole that is 5,5mm from the bottom left corner of the board. Again this is specific to the line its going to be made on. everything you can do to make it easier results in high quality output. Less faults.
>Fiducials are not defined using silkscreen or soldermask.
BUZZ if you do. Minus 10points. Go Straight to Jail do not pass Go. Do not collect $200.
>Define fiducials as components so their locations are automatically included in the pick and place file.
Yes, this is a very good idea. Add them as parts in yoru default templates so you dont' forget to put them in! In my automation scripts, which build my PNP files, i have mine set up to be called FIDTOP1 FIDTOP2 which means it cand find them and deal to them directly. Your vendor may use them differently.
>Read your datasheets! For some devices (QFNs seem to be the primary suspect) the package might not match the one you have in your CAD library even tho' it >might seem the same at first glance. The center pad might be bigger/smaller and the outer pads might be shorter/longer.
And dont' trust librarys that you got from the internet, make sure you've checked them!! or better still actually do them yoruself. After a while you'll get resonably good at it, and its not a big issue. ( QFN's are my fav IC package, they just work so well and are the easiest to reflow if you do it properly. )
>If your board is an odd shape put it in a square panel with routing and scoring as appropriate, don't leave huge gaping holes in the panel, particularly if that PCB >needs to go through wave solder later - keep it nice and rigid.
yeah.. again, talk with whoever is going to run the boards, and see how it will work together.
If you can avoid a custom cable, do so.
> yES. THATS just a way to spend lots of money or time.
>At scale some of these rules change, special tooling will remove some DFM requirements and introduce others - work with your manufacturer.
>Thermally balance your board: top and bottom should have similar copper coverage, if one has way more than the other, your board WILL warp. That can cause >stress on the components as well as being a pain to handle and looking bad.
As a general rule and there are times to break this.. if you are doing a four layer board, keep your two internal layers with as much solid pour on them. and our outside layers with just signal traces.. Its a good starting point.
>Specify parts that exist, there is no point asking for a 1uF NPO 0805 100V capacitor just because the datasheet has suggested NPO is better.
>If assembly looks fiddly, it will cost you more and increase the risk of build errors, costly rework and maybe even damage.
And check that they are availalbe. At design time, take the time to see if the parts are widely avaialble from multiple suppliers.. If only one has it, better think hard.
-
For mounting holes where you will be screwing against the board, put a ring of Vias where the screw head will rest, It will lessen how much the PCB can flow away from that point over time,
Standardize your drill sizes where possible to a smaller subset, if your doing large runs it means less cam time for the operators,
Inside (concave) corners on pcb edges should be rounded of have a designed cut in for a 2.5mm routing bit,
If you have wire solder pads, reinforce the pads with vias to reduce the risk of pad tearing.
Remove solder mask under QFN's where possible, Technically they are more reliable long term if the fillet is thicker, but its harder to get production yield.
Use a good revision naming scheme for your design files, so if you have to do an update because the fab cannot source a certain part, Its clear which is the latest that should be used.
-
Don't put silkscreen overlay under QFN or other leadless parts that have no standoff.
I have had a part sit not quite flat because of a thick silkscreen, causing soldering issues. The footprint generator in AD often places silkscreen under parts that should fit flat.
-
We're doing very small runs of special equipment, here is my list:
- Avoid cables with special connectors. If you have enough space and your signals are low frequency just use solder pads.
- Solder pads for cables should always be clearly marked, use a bigger font than normal for those. The same applies to connectors.
- Test your PCB with the housing it will go into, either in CAD or by printing it on paper and glueing the print to a piece of cardboard. I've seen many projects that had to be redone cause some parts did not fit at the last assembly test with many 100s of units already scheduled for production.
- Make sure all parts of the PCB that need to be touched after assembly (e.g. for wires, test points, headers for firmware updates, ..) can actually be reached without tearing the whole thing apart or breaking your fingers.
- Select a housing that is bigger than your PCB if you want to use watertight PG fittings for you cables. Many manufacturers do not leave enough room so connectors can not be installed correctly. This leads to leaks an damaged PCBs.
- Do a basic thermal test for each project, not just the PCB. Housings and other stuff will have a big impact on airflow and your whole thermal management.
- Be careful if you use PCBs as mechanical references, for example for mounting displays that should be visible in a cutout in the housing. Use bigger screw holes so the production worker can adjust the two parts to match.
- Use proper screws and spend time on finding matching bits / drivers. It will really bite you if you have to use the screw more than once and the head is gone.
- Add proper test points to everything you want to test. It's a pain to get pogo pins that go on connectors and such to work reliable. Avoid having test adapters that need to have a 3D pogo pin structure cause you want to test on high connectors and stuff.
- Leave enough room between test points. It's a pain if you have to contact 6 test points that are spaced like a 1.27mm pitch header.
I have so much more on my mind regarding this, someone should write a book ;)
-
Set routing rules sensibly.
Dont push the envelope just because the design software allows you.
Think about diamond shaped fiducials.
-
Think about diamond shaped fiducials.
Why?
-
Apart from from "diamond fiducial" pulling the most interesting google image threads I've ever encountered, I don't see why a diamond shape would be preferential to any other, so long as the manufacturers tooling can recognize it?
-
Here's the list of defined fiducial types on an Essemtec machine. Personally I have only ever encountered round ones typically 1 to 1.3mm in diameter and they seem to work perfectly well for me.
I find the Annulus type quite useful for those boards where I have to resort to using mounting holes or vias in place of a true fiducial.
-
Visualize yourself building the product as fast as you can while checking documents as little as possible.
Make it easy to find and access anything that production people need (test points, programmer connections, mounting holes, etc).
When I worked in production the most common solution to problems was my generally very friendly boss yelling "read the production binder!" Don't assume people will read your instructions. They might read all of it on first build, could miss steps, and probably won't even glance at it for refresher the next day.
Try to keep fragile components away from screw holes. Boards dont always get gently placed straight onto mounting points and screwdrivers sometimes slip. If someone hits and cracks a ceramic cap when their driver slips, they might not replace it and it might still pass QA.
If you have parts that might need to be glued down (large parts with small connection to PCB), try to leave room for not only glue (rtv or whatever) but also for the glue applicator.
If the PCB is having a spray (conformal coat) applied, think about the shadows created by large parts when spraying on an angle. If you put a bunch of large electrolytics in a 'U' shape with some small parts in the middle of the 'U', theres a chance those small parts won't get coated.
-
Screaming Circuits, a prototype assembly shop in the Portland area (Oregon, USA), publishes the occasional newsletter ("Circuit Talk") that makes for good nerd reading material. They cover the many ways to screw up a board design, so future engineers can learn from others' mistakes. PDFs of each issue are available on their Web site:
https://screamingcircuits.com/about/news
-
Screaming Circuits, a prototype assembly shop in the Portland area (Oregon, USA), publishes the occasional newsletter ("Circuit Talk") that makes for good nerd reading material. They cover the many ways to screw up a board design, so future engineers can learn from others' mistakes. PDFs of each issue are available on their Web site:
https://screamingcircuits.com/about/news
I'm not sure they should be listened to. I opened up the last one and this is what they write:
In five years we may no longer have components larger than 0402.
Yeah right. Ridiculous. And they are supposed to be "in the industry".
-
In five years we may no longer have components larger than 0402.
Yeah right. Ridiculous. And they are supposed to be "in the industry".
LOL, you still have heat to dissipate. There is no way around it :palm:.
-
These are all great ideas ... I have a checklist right in my board-file template on a non-manufacture layer so each project has the list right there to look at. Some things that I haven't seen yet:
- Run the design rule check one last time.
- Make holes where wires will be directly soldered (especially when hand-soldered) about 25% larger than than the nominal wire diameter. Make the annular ring larger (by percentage) than for component pads. Think about strain relief (or its absence).
- Consider making your own footprint for every part you're using. Only use outsourced footprints after you've confirmed they're well designed.
- Ensure no pads make unexpected contact with the case metal.
- Look at the gerber files directly in local software: something separate from your design system.
- Open the drill file in a text editor and look for weird drill sizes (it's not a complicated file format, and each drill size is listed.) Go back to your design and confirm if you find two drill sizes that are almost identical—see if you can change them both to the same size.
- Round off the sharp outer corners with curves in the board outline so the boards are more pleasant to handle. (Except when there's a good reason not to.)
-
Wishing the DRC in Eagle could detect the absence of fiducials of some sort.
I forgot to put fids in a design a few months back which was a pain to deal with. There were no reliable features on the board, so I had to manually align the PCB on each pass through the P&P. Only had to do 30pcs and it was still enough pain to make a permanent mark.
I think I will make a Python script that parses the Eagle files to make sure each PCB includes fids and the in-house part number, and revision number. So easy to forget those.
-
Round off the sharp outer corners with curves in the board outline so the boards are more pleasant to handle. (Except when there's a good reason not to.)
I like to take this a step further and add rout slots around the board as well, and specify v-score through the tabs. The board depanels very cleanly with minimal burrs. :)
It is more steps, though.
Where a rough, rectangular board is all that's needed, I'll still spec v-score. Ugly but cheap.
Tim
-
Lots of good advice here.
-If your board uses many leadless or very small components, place a few test point in strategic signals, and label the signal names.
-annotate your board as much as possible. I know, I know, some components are way too small to be annotated individually.
-always include the board part number and layout revision level. Allow an area for a sticker label which has the BOM and software revisions.
-connectors, specially those which connect to the outside world, suffer from lots of stress. Use ALL of the provided anchor pins.
-
-annotate your board as much as possible. I know, I know, some components are way too small to be annotated individually.
I would say annotate for a reason. dont' do it just because you can.
-
Plenty of test points, annotated on the silkscreen. More so for prototypes. Don't forget a few scope ground points too.
Connect any unused MCU/FPGA pins to test pads, just in case.
Pads and alignment holes for bed-of-nails jigs for test and programming.
Unless your resist is white, put a rectangular block of silkscreen somewhere, so you can mark boards with a permanent marker ( number, tested, programmed, faulty, whatever). If your silkscreen is white, put an outline box so you know where any pen marks should go.
Don't put traces on an inner layer if it can go on the surface - you never know what you may need to track-hack.
If possible, sleep on a layout before ordering.
-
Plenty of test points, annotated on the silkscreen. More so for prototypes. Don't forget a few scope ground points too.
yes. vias are useful for that, until you tent them. better to be deliberate about it, and mark them up. Remember that you need to be able to get a scope tip into the test point! You might want to consider putting in test pins/loops.
Connect any unused MCU/FPGA pins to test pads, just in case.
Or even a header pin if you have space. As you say, just in case, and some time down the track you might just need it for somethign.
Pads and alignment holes for bed-of-nails jigs for test and programming.
yes, think about how you are going to test and program. I'm love the cables from http://www.tag-connect.com/ (http://www.tag-connect.com/)
If possible, sleep on a layout before ordering.
have lunch and dinner.
-
If possible, sleep on a layout before ordering.
This may be the most important tip of them all.
Seems like every time I order at the end of the day, those are the ones with the dumbest mistakes.
-
Check the soldermask layer, esp in Eagle. You can easily tent/untent vias unintentionally.
Check paste layer to make sure you aren't putting paste on pads where you don't want it.
Check "unrouted traces" layer all by itself. Sometimes the ground plane doesn't quite reach areas, and you can't see it until you do this, leaving a 0.1mm gap between a pad and the ground plane. (Done this, and... uh.. where's the engineering inquiry when you need it?)
If you are doing any ongoing dev with the firmware, you can lay down a small area of solid white silkscreen for annotating with sharpie.
Beware that any insigificant but carelss things you leave on the board may turn into "engineering inquiries," otherwise known as questions. You don't want questions, because questions add time/days to your turnaround. If you're intentionally doing something that looks goofy, try to preempt a question by including that info when you submit the quote/RFQ.
Write down the dimensions of your board. You're going to fill out the form halfway and find out you don't know the dimensions. And the quote page will timeout.
If you're using a new manufacturer, be sure to put in multiple quantities, even some many times larger than what you originally anticipate. Some manufacturers have huge price changes over certain quantities. Once you find that magic number, it might save you tons of money in the future. 500 pieces might cost less than 400.
-
This thread should be sticky
yes, think about how you are going to test and program. I'm love the cables from http://www.tag-connect.com/ (http://www.tag-connect.com/)
Didn't know those existed, I usually make my own with pogo pins from mouser, a PCB board, a broken drill, and a small amount of epoxy
-
Didn't know those existed, I usually make my own with pogo pins from mouser, a PCB board, a broken drill, and a small amount of epoxy
That is an impressive amount of effort. nice. I have been using the tag connect ones for some time and programed Lots of boards with them
-
yes, think about how you are going to test and program. I'm love the cables from http://www.tag-connect.com/ (http://www.tag-connect.com/)
They look so cool, I immediately want to order. But when I think about it for a minute, what value does this bring in? My standard is 5x1 0.1" header. When space is limited I go with 5x1 2mm, and when it is super limited I use 5x1 1mm. 1mm is PITA to work with, but it is even smaller when the tag-connect. 2mm is about the same area as TC and quite comfortable to work with. For production I can leave pin underpopulated. I like to double the two pins in a center as a serial port output for debugging. So if I have to I can solder in two pins and get debug info out of the board. 5x1 also can be installed on either side of the board, but 2x3 can't, because the piount will be mirrored.
The plastic hooks on TC seems to be subject to frequent breaking.
-
yes, think about how you are going to test and program. I'm love the cables from http://www.tag-connect.com/ (http://www.tag-connect.com/)
They look so cool, I immediately want to order. But when I think about it for a minute, what value does this bring in? My standard is 5x1 0.1" header. When space is limited I go with 5x1 2mm, and when it is super limited I use 5x1 1mm. 1mm is PITA to work with, but it is even smaller when the tag-connect.
I also was looking for a 5-way in-line version for the standard PIC ISP header but they don't seem to do them.
I use 2.54,2 and 1.27mm versions depending on size constraints - with an in-line header it's fairly easy to solder some pogo pins to some protoboard to get similar functionality.
You don't need the board locks for production programming, and for development you can just solder a header on.
-
Wishing the DRC in Eagle could detect the absence of fiducials of some sort.
I forgot to put fids in a design a few months back which was a pain to deal with. There were no reliable features on the board, so I had to manually align the PCB on each pass through the P&P. Only had to do 30pcs and it was still enough pain to make a permanent mark.
Buy a K40 laser from China for $400 and you can burn some sort of feducials after and at the same time print a unique pcb or barcode on the pcb to differentiate individual pcb's.
-
Wishing the DRC in Eagle could detect the absence of fiducials of some sort.
I forgot to put fids in a design a few months back which was a pain to deal with. There were no reliable features on the board, so I had to manually align the PCB on each pass through the P&P. Only had to do 30pcs and it was still enough pain to make a permanent mark.
Buy a K40 laser from China for $400 and you can burn some sort of feducials after and at the same time print a unique pcb or barcode on the pcb to differentiate individual pcb's.
When I did it, I just used some calipers to scratch a cross a fixed distance from the PCB corners, which was good enough
-
When I did it, I just used some calipers to scratch a cross a fixed distance from the PCB corners, which was good enough
On 30 consecutive pcbs within 0,1mm accuracy :-//
-
When I did it, I just used some calipers to scratch a cross a fixed distance from the PCB corners, which was good enough
I simply take a couple of 0603 parts closer to corners of PCB and use them as fiducials. Though after having to do that a couple of times you learn not to repeat that mistake :)
-
yes, think about how you are going to test and program. I'm love the cables from http://www.tag-connect.com/ (http://www.tag-connect.com/)
They look so cool, I immediately want to order. But when I think about it for a minute, what value does this bring in? My standard is 5x1 0.1" header. When space is limited I go with 5x1 2mm, and when it is super limited I use 5x1 1mm. 1mm is PITA to work with, but it is even smaller when the tag-connect.
I also was looking for a 5-way in-line version for the standard PIC ISP header but they don't seem to do them.
I use 2.54,2 and 1.27mm versions depending on size constraints - with an in-line header it's fairly easy to solder some pogo pins to some protoboard to get similar functionality.
You don't need the board locks for production programming, and for development you can just solder a header on.
I dont' use the ones with the plastic locks on them. Kind of defeats the purpose for me. as i'm wanting somethign small. Big advantage i see is that they are just single sided, so you dont' consume lots of board ). Makes layout easier. and it often means you can get them very close to the relevent IC. I started out with .1" headers as well, but am using these a lot. Where i need to have a test jig as well, i have just used some standard pogo pins and created the layout.
Mike, Microchips ICSP port is technicallyk not 5 pin, its 6. I know lots of times the 6th pin is not used. Look at a Pickit it has 6 pins. I've pretty much ditched usign Pickits because they are just too slow, and use the ICD3 and ICD4.. Sadly the ICD4 does not have support for all the older IC's yet.
We've programmed thousands of parts using them and they work.. Not the only answer to the problem of course.
-
Yes, Pickit is 6 pins, but I'm yet to encounter an MCU that requires 6th pin to be programmed. I worked probably with like 30-50 different one including pic24, dspic, pic32
-
Yes, Pickit is 6 pins, but I'm yet to encounter an MCU that requires 6th pin to be programmed. I worked probably with like 30-50 different one including pic24, dspic, pic32
Most of the new pics support Low voltage programming, which requries the use of the 6th pin (PGM ). There are times that you wont' want to use HVP ( High voltage programming ). LVP allows programming to occur at the VCC level of the Chip ( 3.3V / 5V or so ).. Its worth a read up on this topic.
-
PCB Surface Selection.
HASL is cheap, but often problematic. ENIG can be a better alternative/
-
Yes, Pickit is 6 pins, but I'm yet to encounter an MCU that requires 6th pin to be programmed. I worked probably with like 30-50 different one including pic24, dspic, pic32
Most of the new pics support Low voltage programming, which requries the use of the 6th pin (PGM ). There are times that you wont' want to use HVP ( High voltage programming ). LVP allows programming to occur at the VCC level of the Chip ( 3.3V / 5V or so ).. Its worth a read up on this topic.
Many of the newer PICs (not sure exactly which but noticed when I was fixing some broken PICkits) don't use HV on MCLR, so LVP is redundant on those. I can't think of many scenarios where HV programming on MCLR is a problem - worst-case a series resistor may be needed. I've never seen a need to use LVP - as far I'm concerned the ISP header is always 5 pins.
Pickit is slow on larger parts but has the huge benefit of programmer-to-go mode for standalone operation, which AFAIK isn't yet implemented on PK4 ( last time I looked there wasn't even any mention in the docs).
-
Pickit is slow on larger parts but has the huge benefit of programmer-to-go mode for standalone operation, which AFAIK isn't yet implemented on PK4 ( last time I looked there wasn't even any mention in the docs).
yeah, its very slow. Too slow to be useful, for anything other than if you are doing some in the field upgrade thing. I have used it to send a to a customer, in an attempt to make it super easy. Though most times, customers are a long way away, and they perfer an update via file!
-
Hi All, NEWBY here, with a different perspective on PCB design;
1st off, understand the electronics assembly industry and how a blank PC end's up being an assembled PCB used in a device, understanding how all the parts go together is essential for a good board layout & design. Think through the entire process...Then design the board.
Secondly: Regardless if your building the PCB yourself or Outsourcing, absorb every response that is given in this forum, yes including mine. Understand that proper spacing of all bottom & topside SMD to PTH is critical in the manufacturing of the card and the final price! Will the card need a solder pallet, not just for the SMT process but wave solder (including Select soldering & Batch soldering), AOI & X-RAY, Press fit, Conformal Coating, etc, etc... Everything you design today will have a major impact on the future build of this PCB and the people that build it, along with the costs associated with building this PCB. Remember this: HANDLING KILLS A CIRCUIT BOARD.
3rd: See & Feel the design: Look at the parts being placed & inserted on the card, what role will panelization play when building the card, what extra expenses may be required to build the card (pallets), Look downstream man!! Look past the billfold and create a design a circuit board that can be built in the least amount of time, with the fewest defects possible. It can be done!
When I started in the electronics assembly Industry many moons ago, 85% of the people I dealt with were circuit board designers. At that time (mid to late 90's) design engineers realized that if they were to create a circuit board using guidelines established by the solder tooling world, they could create a board that can start at one end of the plant, pass through all QC checks and placed in a box at the end of the day. That never happens anymore, once a year I might hear from a designer looking for some advice on the proper spacing between SMD & PTH, but that's it.
Understand the process of circuit board assembly. Once the design is complete, get the valued opinion of at least three people (Manufacturing & Process Engineers that will build the product) and see what they have to say!
Then design a circuit board.
-
Hi All, NEWBY here, with a different perspective on PCB design;
1st off, understand the electronics assembly industry and how a blank PC end's up being an assembled PCB used in a device, understanding how all the parts go together is essential for a good board layout & design. Think through the entire process...Then design the board.
If that were the case....very few people would ever make a PCB.
I recommend....fail fast and fail often in the case of PCB design. In general, it is faster and cheaper to learn what you can, make a design, send it to the fab/assembly. Your mistakes will be called out and you will learn fast. The cost of the bad boards is less than trying to become an expert before you even try.
There are rules and regs that govern good PCB layout, but experience and intuition cannot be studied. Pick some easy-ish projects and make them. Get feedback from others and use the responses to make the next one better. Assemble them yourself as much as possible, there are a lot of lessons to be learned while staring at the PCB for 2 hours while you assemble it.
-
Hi All, NEWBY here, with a different perspective on PCB design;
1st off, understand the electronics assembly industry and how a blank PC end's up being an assembled PCB used in a device, understanding how all the parts go together is essential for a good board layout & design. Think through the entire process...Then design the board.
If that were the case....very few people would ever make a PCB.
I recommend....fail fast and fail often in the case of PCB design. In general, it is faster and cheaper to learn what you can, make a design, send it to the fab/assembly. Your mistakes will be called out and you will learn fast. The cost of the bad boards is less than trying to become an expert before you even try.
There are rules and regs that govern good PCB layout, but experience and intuition cannot be studied. Pick some easy-ish projects and make them. Get feedback from others and use the responses to make the next one better. Assemble them yourself as much as possible, there are a lot of lessons to be learned while staring at the PCB for 2 hours while you assemble it.
Exactly!
-
Whats your top tips for designing PCB's that are manufacturable?? or improve cost and reduce faults.
There are many good points about PCBs containing modern logic in: http://cache.freescale.com/files/training/doc/ftf/2014/FTF-SDS-F0198.pdf (http://cache.freescale.com/files/training/doc/ftf/2014/FTF-SDS-F0198.pdf)
-
If your prototype board doesn't work as it should, make it work by any means necessary (cut traces, bodge wires, dead bug fixes, etc) before you spin again. That is, do not be an idiot and just fix the first problem you found before you re-spin.
-
Its certainly a lot easier than it used to be!
-
I can't think of many scenarios where HV programming on MCLR is a problem
You have just received your new expensive PIC32 board, you connect it, you open the PIC32 project. However, the other PIC16F628A project is still open. You click the "make" button, the PIC16 project compiles, PICkit3 applies 13V to MCLR - bye bye PIC32.
The PGM pin is only needed for very old PICs - the new ones do not have it and still can do LVP.
-
If your prototype board doesn't work as it should, make it work by any means necessary (cut traces, bodge wires, dead bug fixes, etc) before you spin again. That is, do not be an idiot and just fix the first problem you found before you re-spin.
You mean "don't use Agile methods for hardware design."
-
If your prototype board doesn't work as it should, make it work by any means necessary (cut traces, bodge wires, dead bug fixes, etc) before you spin again. That is, do not be an idiot and just fix the first problem you found before you re-spin.
You mean "don't use Agile methods for hardware design."
Yes. I've just seen it done so many times, particularly by non-HW people who have been tasked with hardware dev. They are perpetually surprised when there is more than one thing wrong with their boards.
On the other hand, this isn't really a DFM-specific issue. It's just a don't waste time and money issue, which is pretty basic engineering.
-
I've been tasked with cleaning up a "REV G" board more than once... :popcorn:
Tim
-
The ends of a spectrum....
one end: hack & go @ $10/ea per iteration. The other: study, learn the theory, apprentice to the masters, grok the entire process
One gets you practical knowledge, a feeling for good enough, and a pile of drink coasters; the other, potentially, a product that can be produced economically at scale.
I'd guess that most of us are in the first category, trying to learn from the 2nd.
In many ways, good Design for Manufacturing is as complex as "feeds & speeds" and "tool & work holding" are in the shop - the concepts and practices are complex and hard for the novice to comprehend, until, that is, they have walked the path of enlightenment (aka coaster production) and see for themselves what that advice really means.
The competing wisdom in this thread would make a great "Zen of circuit board design" guide :-)
-John
-
The ends of a spectrum....
one end: hack & go @ $10/ea per iteration. The other: study, learn the theory, apprentice to the masters, grok the entire process
Unfortuantly its not $10/interation is it. Its $1000's of dollars and weeks of time.
-
I pride myself on doing "Rev B" designs: the first prototype is pretty close but missed a few things; the final build fixes exactly those problems and is ready for production.
Gotchas are sometimes my/our fault, but it's also often the case that the customer changes their spec -- it happens -- and then it goes up from there. (We've got one customer that's pushing rev 10 on some boards, but they're also a long time customer and their product is slowly but constantly evolving. That's fine, beats spinning a whole new product line after all. :) )
Tim
-
My plans normally work on three interations;
(a) A prototype
(b) A revision
(c) Production.
Sometimes i go a->c.. and sometimes theres a b.1
-
Depends on the customer... Not always there is a luxury of having full specs from the start. On recent project the final revision is rev 12, of which I actually manufactured 4... :palm: The last one was to fix EMI issues.
-
Depends on the customer... Not always there is a luxury of having full specs from the start. On recent project the final revision is rev 12, of which I actually manufactured 4... :palm: The last one was to fix EMI issues.
If the customer is paying then changes = increased costs to them.
-
If you ever get the chance to visit an assemblers factory you will get further insight into what can make boards easier or harder to put together. The grimacing from the operators is a fine indication of a problem board ;)
-
If you ever get the chance to visit an assemblers factory you will get further insight into what can make boards easier or harder to put together. The grimacing from the operators is a fine indication of a problem board ;)
Bringing assembly into our own environment made us think very hard about our designs. Seemingly minor changes can make a big improvment to how things work.