Solder paste layer padstack, remove for DNF components?

Hi All,

I have a component on a PCB that is simply a set of pads with no component fitted. The idea is that the processor will be fitted pre-programmed, but if I ever want to change the firmware any existing boards can be re-programmed using a test pin header using spring type contacts. This keeps the cost down of the main board by not requiring a header while still gives the ability to easily re-program.

Question: In the CAD I have padstacks that define the solder paste. I obviously don't want solder paste on these pads, so is it my responsibility to remove the solder paste layer for this component and give the assembly house the final stencil gerbers, or does the assembly house modify them to produce their own stensils? If the latter I presume they would also not paste un-fitted components. What is the normal way things are done?

Mark.

Reply to
markp
Loading thread data ...

You send them the gerber layer for the stencil as you want it. They will send that away to have the stencil made in the appropriate thickness ( thinness!)

>
Reply to
TTman

Also, if you can program/upgrade the CPU with ISP, why not have it fitted at assembly time and program it when you get the board back. The cost of ISP must be much less than soldering on by hand a CPU...

>
Reply to
TTman

OK, so presumably any do not fit components would end up being pasted and a layer of solder ends up on the pads, unless I explicitly remove the mask from the solder paste gerber?

Reply to
markp

The CPUs are ISP devices that pre-programmed by a programming house (automatically de-reeled, programmed, and re-reeled. Quite cheap to do that). The board is quite simple, and it will be tested in situ when it is assembled with other boards. So the cost of explicitly programming each one (thousands off) is quite high. However, I don't want to write off any boards that had been made already should i find I needed to change the firmware, so that's why it has pads only. To add an explicit programming header would add cost for a function thay will hopefully never be used.

Mark.

Reply to
markp

The way I read it was that a preprogrammed CPU would be mounted, but with an ISP option through a number of pads an a bed of nails like arrangement instead of an actual connector.

Have look in the CAD program for how test pads are normally done

-Lasse

Reply to
langwadt

Couple of ways... Depending on the density of the board, you can ask to have certain apertures physically masked out at production, by putting tape on the stencils.

Find a way to edit individual padstacks in the layout to derive a new one without a paste mask opening, Allegro does this easily. What package are you using?

Define a new padstack in your library without a paste opening, call it something meaningful and create or change your part footprint to use this padstack.

Go in nice and nasty and edit the gerbers manually before sending them out to the fab. It's like modifying a binary by hand instead of the source code. I would not do this unless it's a proto and even then I'd need to be drunk. Some might say I'm drunk anyways.

Reply to
a7yvm109gf5d1

Mark, Just curious, what spring loaded connector are you using to program these boards? I am currently working on a board, and have found that I need to connect to it to program it in situ. I am presently going to just try having through hole pins that will provide a tight fit to a .100 connector stuck through them, but wondered if there is a better way?

Charlie

Reply to
Charlie E.

Sprung loaded pogo pins (google) used extensively on ATE ( bed of nails)

Reply to
TTman

Microchip has a connector design that requires only pads and holes on the PCB.

formatting link

I haven't tried it. Some other folks have come up with a row of pogo pins that can be held against an unpopulated row of 1x6 0.1" header holes (the header is probably the most popular connector scheme for low volumes). Or a PCB fixture can be designed with pogo pins that actually holds the PCB in alignment and avoids having the get your hands near the programming cable.

Best regards, Spehro Pefhany

--
"it's the network..."                          "The Journey is the reward"
speff@interlog.com             Info for manufacturers: http://www.trexon.com
 Click to see the full signature
Reply to
Spehro Pefhany

As others have noted these are 'pogo' pins, although I think Pogo is a trade name and uses synonymously with this kind of bed of nails pin (like hoover is used for vacuum cleaners). If you do a search for pogo pins on Farnell you get some expensive pins, but searching for 'spring test pin' and you get much cheaper versions.

Farnell part example:

1313683

Mark.

Reply to
markp

Maybe your pad stack editor can define certain pads not to have solderpaste. My old Orcad DOS version can. (PCB386+)

-- Boris

Reply to
Boris Mohar

Mill-Max makes a variety of spring-loaded pins in various lengths and configurations:

formatting link

I've successfully done a home-made version with their

0906-0-15-20-76-14-11-0 (Digikey p/n ED8180-ND) soldered through regular 0.062 FR4. (maybe not how it was intended to be used but it worked great)
--
Rich Webb     Norfolk, VA
Reply to
Rich Webb

It looks like the non-free versions of ViewMate

formatting link
permit editing and then re-saving the modified Gerber files. Might be the cleanest way to "delete" those pads from the stencil Gerber.

Note to Pentalogix if you're reading: I would have purchased the damned thing instead of relying on your free version (useful tool, BTW) but I'm not interested in a node-locked license.

--
Rich Webb     Norfolk, VA
Reply to
Rich Webb

Yes, that is now what I've done. I've decided to design the PCB for production so the paste layer on the padstack for this component has now been removed. I spoke to an assembly house, they can do anything I want including masking on the stencil during manufacture or removing them from the stencil entirely. Best though to be in control, so I've removed it for them.

Mark.

Reply to
markp

Thanks, Sphero, That looks like a good idea, and I may incorporate it in my next design. I will stick with my present idea for now, as it allows me to even shut the case and do testing and programming, if it works... ;-)

Charlie

Reply to
Charlie E.

Why are you worried about solder paste on the pads?

Spring loaded test pins make good contact with solder-coated pads.

So much so that one very reputable contract manufacturer I have used specifically asked for paste to be present on test pads. They find that the test pins dig into the solder and make more reliable contact than with bare copper.

John

Reply to
John Walliker

Interesting. I've thought about this and have now decided to keep the paste! Thanks, it makes sense.

Mark.

Reply to
markp

ElectronDepot website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.