[SOLVED] Weird mounting hole footprint

On a PCB in a video (https://youtu.be/qyDRHI4YeMI?t=7s) there are three oddly shaped mounting holes on the main board, apparently with 6 vias arranged symmetrically around them. What's their purpose? I assumed it would have something to do with relieving mechanical stress, but the daughter board on the same panel has "regular" mouting holes without them.

Any ideas?

That's pretty standard for electrically conducting mounting holes on regular wave soldered board (not selective wave). You find it on most PC main boards. The center hole is unplated and kept free of tinn, saving an additional rubber mask.

Hi ArticCynda,

3 big holes : 2 purposes

i.) Act as guiding when pass through SMD machine and during pcb level testing.

ii.) Fix to cabinet during casing


6 vias surround big hole :

To avoid copper plate torn off from substrate

Roger

FvM said:

That's pretty standard for electrically conducting mounting holes on regular wave soldered board (not selective wave). You find it on most PC main boards. The center hole is unplated and kept free of tinn, saving an additional rubber mask.

Click to expand...

Sounds logical, but in the video the main board is SMD (thus I assume not wave soldered) while the daughter board does not have the vias but is presumably wave soldered (only through hole components). So that is contradicting your theory, FvM!

Is there any reason to have these "via style" mounting holes on a reflowed SMD board at all?

The board is not completely reflow soldered, it has many through-plated connectors. If they ahall be wave soldered and the mounting holes provide electrical connection, some means to prevent solder filling of mounting holes is required.

Thanks for the clarification guys, I was completely unaware of the existence of temporary washable or peelable latex solder masks, so I learned something new today! I'll keep this in mind if I'll ever get to the point of designing boards for mass production!

vias around a mounting hole is common practice for another reason, even if the mounting hole is plated the plating can be removed easily by using bolts machine screws etc, the thread can easily scrape plating off. The vias ensure continuity even if this happens.

Hi,

For your interest, if this board will go through mass production :

It is a good practice to put a small dot ( e.g. 1mm dia. ) near a multi pin component ( e.g. cpu ). The purpose is to let ' Pick and Paste ' machine set origin ( use laser beam ) so that all SMD components will put to right place with mininum offset.

To let this board pass through both reflow and wave solder machine, following design should be considered :

It's better to let all components ( SMD + through hole ) placing on same side of pcb while designing the board ( if possible ) .

Reason :

SMD components do not need to glue ( or use high melting point solder paste ) when passing through ' Pick and Paste ' machine and oven, otherwise :

i.) Some component may drop off, offset, mis-align etc ( because through hole component metal pins and SMD component are now on same side ) when pass through wave solder machine.

ii.) Touch up process also needed ( residue solder may causing short circuit between SMD compnent and metal pins )


Gluing smd component is a very time comsuming process and use of higher melting point solder paste is expensive.


From manufacturing point of view, it costs !

Roger

Having at least two fiducial's (preferably 3) is the way to go for P&P, a lot of todays pick and place machines use cameras to check the actual pad positions and the devices pins as it is held to check for any change in delta (angle) and thus place the component exactly in the required position.