PCB assember criticism of layout

Status
Not open for further replies.
T

treez

Guest
Hello,

Our PCB assembly house have criticised the small distance from a surface mount capacitor to a PTH footprint of a connector. The exact critisism words are as follows.....

Too close distance between PTH toeprint to bottom side SMT components which will affect PTH solder barrel filling during wave soldering process, also it will be hard for the PTH components rework.
Click to expand...

Here is a picture of the offending component "C61" which is said to be too near to the PTH holes.
https://i40.tinypic.com/10ofl2s.jpg

They say they need a spacing of 3.81mm, but does that mean from the edge of the PTH pad to the component case, or from the edge of the PTH drill hole to the component casing.?

Also, do you know what is "solder barrel filling"?
 

The assembly house is correct. These days, through-plated components on a mixed assembly SMD boards are soldered with selective wave technique. A solder nozzle is moved below the board to the respective pin positions. Depending on the applied nozzle size, a certain distance of bottom side SMD components to through holes is required.

There might be special cases, where the distance rules can't be kept. The respective through hole components must be hand-soldered then.

"Baffle fill" is a term describing the correct soldering of through-hole pins. It's required according to IPC standards that the solder rises in the through-plated hole (or "baffle") to e.g. 75% of total heigth,
 
Reactions: treez

    T

    Points: 2
    Helpful Answer Positive Rating
Thanks, should the PTH's also be a certain minimum distance inside the board edge? I mean, if the PTH's are too close to the board's edge then will that render the "barrel filling" as being poor in quality?...

...in another critisism, the assembler says that a PTH pad should be reduced in size and that a "3 mil SM web" should be ensured......here are the exact words.....


Do you know what "3 mil SM web" means?
I suspect it means that the PTH should be slightly oversized in relation to the actual pin that is to go in it...but i dont know?
 

There will be a minimal copper feature and drill hole to board edge clearance specification, but it's not primarly related to "barrel filling".

"Solder mask web" - the minimum solder mask structure width. You'll find pretty much about it in PCB design tutorials.
 
Reactions: treez

    T

    Points: 2
    Helpful Answer Positive Rating
You can offset the nozzle of a selective solder machine and still get a good joint. Depending on the size of the selective solder nozzle and wave size you have to use a circular keep out round the pads to be soldered, generally keeps outs are based on 6-10mm circles, the larger the wave though the more stable it will be. I have found that an 8mm circle gives the best compromise between density of placement and selective solder wave stability, a 6mm nozzle is quite small and produces quite a turbulent wave, whereas 8 & 10mm nozzles the wave is more laminar and is better than a 6mm m nozzle. Again this circle can be centred on the pad to be soldered or offset to allow components to be placed near the pad at one side.
 
Reactions: treez

    T

    Points: 2
    Helpful Answer Positive Rating
Status
Not open for further replies.

Similar threads

Menu
Log in
Register
Cookies are required to use this site. You must accept them to continue using the site. Learn more…