the distance between two PIN is less than 0.25mm，can not make the solder bridge.

[carl0s]

What do you think PCBWay mean here?

The pins are 0.2mm apart (or 0.19 in their measurement), but I have specified 0.6mil gap which is around 0.15mm, so what's the problem?

Are they saying I have specified a solder mask where it's not possible or something? I did wonder about that, but I presumed they would just apply mask wherever possible and leave off if too small?

This will be my third re-upload, after missing drill file, followed by missing keepout definition, and now this. I don't want to get blacklisted





Altium is giving me DRCs for the soldermask in a few areas, so maybe that is it. I just thought they did a best effort on that though.

[ataradov]

They are saying that they can't make solder mask between those pins. Just tell them to remove any solder mask they can't make. What they will actually do is try to make it anyway, but it will not come out 100%, but that's fine for hand soldering.

This is such a common issue that they should have really asked some native English speaker to write a canned explanation of what they want. Be thankful they did not call it "green oil" this time

[carl0s]

 

They are saying that they can't make solder mask between those pins. Just tell them to remove any solder mask they can't make. What they will actually do is try to make it anyway, but it will not come out 100%, but that's fine for hand soldering.

This is such a common issue that they should have really asked some native English speaker to write a canned explanation of what they want. Be thankful they did not call it "green oil" this time

hahaha green oil. I can imagine spending days trying to figure out what they meant :-)

Thanks for explaining it to me. I had 99% realised it was soldermask, and I have been applying fills to the soldermask layer, and moving vias a little bit.. basically I think I need to listen to the DRC errors and put them right :-)

[ataradov]

I just started listening to the last The Amp Hour podcast and right off the bat Chris complains about exactly the same thing

[carl0s]

I just started listening to the last The Amp Hour podcast and right off the bat Chris complains about exactly the same thing

Success!

[carl0s]

I just found this in my Junk Mail folder (even though their main website emails didn't go to junk).
 
It suggests that if I went for green instead of black, then it would have been OK. ?

I'm wondering if I should have gone with green now and got a finer solder mask :-/

[ataradov]

Black is a bit worse, but I doubt it would have make that much of a difference. Thin slivers on solder mask are not very robust, even if they claim they can make them, so I would not count on them to do anything useful.

[carl0s]

Black is a bit worse, but I doubt it would have make that much of a difference. Thin slivers on solder mask are not very robust, even if they claim they can make them, so I would not count on them to do anything useful.

Good to know.

Also good to note that PCBWay did communicate well.. if it wasn't for my Office 365 Junk Mail filter.

It looks like the person at the other end (called Smile ?) mentioned the solder mask problem right from the get-go - when I had missing keepout.


Anyway, I await my reflow oven kit (Controleo3), trinocular thingy (geez that was expensive), and my 50 circuit boards :-) Back to sleep and work for a few weeks.

[bson]

What did you use for the layout?  Seems like it was set to keepout areas way too narrow.  The mask is never perfect, and if you set the tolerances too tight you risk getting mask on pads.  This in turn means either they have to remake them for you, or you get boards that are potentially very difficult to assemble.  Not so much for ICs, but e.g. 0402 caps are gonna be a PITA to place and reflow if the mask between the pads encroaches even the slightest.  In these cases it's much preferable not to have any mask at all.

[T3sl4co1l]

FYI, it is acceptable to shave pads a bit.  Some pins are overly wide as well, so that a positive side fillet is somewhere between undesirable and impossible.

IPC-7351 is fine with slightly negative side fillet, and I haven't found problems doing this in practice.

Example: 0.5mm pitch, 0.25mm max pin width.  Don't use 0.3mm pad width.  That leaves 0.2mm space, of which 0.075mm on each side must go to copper-to-mask-opening clearance, due to the typical 0.075mm positioning error between copper and mask.  That leaves 0.05mm for the actual mask web width, which is far too little.  At that size, it won't work at all, or it will flake off during manufacture or assembly.

To get 0.075mm or better gap and web width, you need 0.225mm or more between pad edges.  If you use 0.25mm pads, a web width of 0.1mm is quite manufacturable.

Most 0.5 and 0.65mm pitch components have pin widths equal to half the pitch, so this is straightforward.

I've seen a lot of VSSOP/MSOP parts where the leads are wider.  In that case, it's your call whether to size the pads accordingly, or keep them around half pitch.  At least the ones that are 0.65mm pitch, the pad gap can still be comparable to 0.5mm-pitch, half-width dimensions.

I've been told by one assembler, that they only look for one good solder fillet, preferably toe where it's easily inspected.  Sides don't matter, and heel is optional.  More is fine of course, but it's good to know the minimums.

Tim

[carl0s]

What did you use for the layout?  Seems like it was set to keepout areas way too narrow.  The mask is never perfect, and if you set the tolerances too tight you risk getting mask on pads.  This in turn means either they have to remake them for you, or you get boards that are potentially very difficult to assemble.  Not so much for ICs, but e.g. 0402 caps are gonna be a PITA to place and reflow if the mask between the pads encroaches even the slightest.  In these cases it's much preferable not to have any mask at all.

Hi. It was Altium, but it was my first time and I was learning as I went.. and there's a lot I don't understand, so I was going with defaults.

FYI, it is acceptable to shave pads a bit.  Some pins are overly wide as well, so that a positive side fillet is somewhere between undesirable and impossible.

IPC-7351 is fine with slightly negative side fillet, and I haven't found problems doing this in practice.

Example: 0.5mm pitch, 0.25mm max pin width.  Don't use 0.3mm pad width.  That leaves 0.2mm space, of which 0.075mm on each side must go to copper-to-mask-opening clearance, due to the typical 0.075mm positioning error between copper and mask.  That leaves 0.05mm for the actual mask web width, which is far too little.  At that size, it won't work at all, or it will flake off during manufacture or assembly.

To get 0.075mm or better gap and web width, you need 0.225mm or more between pad edges.  If you use 0.25mm pads, a web width of 0.1mm is quite manufacturable.

Most 0.5 and 0.65mm pitch components have pin widths equal to half the pitch, so this is straightforward.

I've seen a lot of VSSOP/MSOP parts where the leads are wider.  In that case, it's your call whether to size the pads accordingly, or keep them around half pitch.  At least the ones that are 0.65mm pitch, the pad gap can still be comparable to 0.5mm-pitch, half-width dimensions.

I've been told by one assembler, that they only look for one good solder fillet, preferably toe where it's easily inspected.  Sides don't matter, and heel is optional.  More is fine of course, but it's good to know the minimums.

Tim

Hi Tim. I'm going to keep coming back to that post each day until I understand it. I think I'm beginning to..

[carl0s]

boards have come out looking reasonable, and the pads line up too

[JS]

0.2mm clearance between each pin? Easy with toner transfer! 0.5mm pin pitch just last week...

Soldermasks in those tiny spaces are a usual problem, Dave talks about that every other video.

JS

[jmelson]

I'd make those pads a bit thinner.  It will be hard to solder without causing solder shorts.  I usually try to make the gaps between pads about the same as the width of the pins.  For really fine-line stuff, I sometimes make the gaps larger than the width of the pads.

Jon

[carl0s]

I'd make those pads a bit thinner.  It will be hard to solder without causing solder shorts.  I usually try to make the gaps between pads about the same as the width of the pins.  For really fine-line stuff, I sometimes make the gaps larger than the width of the pads.

Jon

That is the footprint file that Samtec provide. The boards are made now anyway so we'll have to see how they turn out after reflow.

[carl0s]

0.2mm clearance between each pin? Easy with toner transfer! 0.5mm pin pitch just last week...

Soldermasks in those tiny spaces are a usual problem, Dave talks about that every other video.

JS

Good work :-)

[jmelson]

That is the footprint file that Samtec provide. The boards are made now anyway so we'll have to see how they turn out after reflow.

Well, if you are real careful with part alignment, and very sparing with the solder paste, it probably will work.  But, if the alignment is a little off, or there is too much solder paste, then you will get shorts.  This is a constant problem for me, too.  SOIC are pretty easy, but SSOP and .65mm TQFPs are a problem, and 0.5mm TQFPs really give me fits.

Jon

[chris_leyson]

0.5mm or less pin pitch and you're not going to have room for soldermask so it's important to get the paste and placement part of the build spot on. I've seen problems on 0.5mm Hirose DF12 connectors that were machine placed and they had shorts in the heal area. Looking at the profile of the pin the heal is quite abrupt, not like the gentle slope of a gull wing pin, so there is nowhere for the paste to flow. The problem was solved by tweeking the paste stencil, reducing the width and shortening the heal.

@carl0s. Nice layout and take care placing those Samtec connectors, they're good HF connectors with the ground connection running down the center. The back of the pin is nicely curved so the solder will form a good heal and I've never had solder shorts when using them.
Spotted the little buck converter, is that inductor a Wurth TPC 3816 ? looks like it. If you want small buck converters then try these http://www.ti.com/lit/ds/symlink/lmzm23600.pdf They also cost less than a discrete switcher, diode and inductor, got some on order and I can't wait to try them out.

[carl0s]

0.5mm or less pin pitch and you're not going to have room for soldermask so it's important to get the paste and placement part of the build spot on. I've seen problems on 0.5mm Hirose DF12 connectors that were machine placed and they had shorts in the heal area. Looking at the profile of the pin the heal is quite abrupt, not like the gentle slope of a gull wing pin, so there is nowhere for the paste to flow. The problem was solved by tweeking the paste stencil, reducing the width and shortening the heal.

@carl0s. Nice layout and take care placing those Samtec connectors, they're good HF connectors with the ground connection running down the center. The back of the pin is nicely curved so the solder will form a good heal and I've never had solder shorts when using them.
Spotted the little buck converter, is that inductor a Wurth TPC 3816 ? looks like it. If you want small buck converters then try these http://www.ti.com/lit/ds/symlink/lmzm23600.pdf They also cost less than a discrete switcher, diode and inductor, got some on order and I can't wait to try them out.

Thanks Chris. Yes good spot - that's a Wurth inductor. Quite an expensive part overall.
It's a step up converter for the LED backlight. This is to fit a largish round MIPI-DSI LCD display on the Stm32L4R9i-discovery

[janekm]

Black is a bit worse, but I doubt it would have make that much of a difference. Thin slivers on solder mask are not very robust, even if they claim they can make them, so I would not count on them to do anything useful.

It's a lot worse. It's the difference between die-based soldermask used for low-coverage colours like green, yellow, purple and pigment-filled colours like white and black which have much lower adhesion, causing small solder mask slivers to flake off easily.

My recommendation is to always stick to green if the colour doesn't matter as that is the colour that the PCB fabs use day-in day-out so the process is very well tuned in.

On the other hand, the yellow colour at JDB/PCBWay is rather nice as it has a really good contrast for the traces, so great for debugging, it's like the opposite of black 

[carl0s]

Black is a bit worse, but I doubt it would have make that much of a difference. Thin slivers on solder mask are not very robust, even if they claim they can make them, so I would not count on them to do anything useful.

It's a lot worse. It's the difference between die-based soldermask used for low-coverage colours like green, yellow, purple and pigment-filled colours like white and black which have much lower adhesion, causing small solder mask slivers to flake off easily.

My recommendation is to always stick to green if the colour doesn't matter as that is the colour that the PCB fabs use day-in day-out so the process is very well tuned in.

On the other hand, the yellow colour at JDB/PCBWay is rather nice as it has a really good contrast for the traces, so great for debugging, it's like the opposite of black 

Funny you should say that. I've only looked at a few of my 50 PCBs, and one of them had a chunk/flake of the soldermask missing off the bottom.