PCB stencil, aperture size and Gerber files

Go To Last Post
10 posts / 0 new
Author
Message
#1
  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Hi 

 

I am working on a PCB and will need to get a stencil made.

 

I have been advised that on components such as QFN with a GND pad , that i should create small squares or circle, so that paste does not cover the entire pad.

 

What layer would i need to modify the component this  on as i can see a "Top Paste" and "Top Solder"

 

Should the solder paste cover the entire pad of a component all the components such as passives?

 

I am using a old version Altium designer

 

 

Thanks

Regards

DJ

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

djoshi wrote:
I have been advised that on components such as QFN with a GND pad , that i should create small squares or circle, so that paste does not cover the entire pad.

Most likely you will want some vias so any excess solder can flow to the other side of the board, or else your smd part will float on this pad and prevent some pads on the perimeter from making contact.

Make some "test" pcbs with different size vias to see what works best for your particular smd part when run though the pick-n-place + reflow oven.

 

Jim

 

 

 

(Possum Lodge oath) Quando omni flunkus, moritati.

"I thought growing old would take longer"

 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

ki0bk wrote:
Most likely you will want some vias so any excess solder can flow to the other side of the board

I was told the very opposite by a PCB supplier. If you do have vias in the central mounting pad these should be "tented" to use the official word. This prevents all the solder wicking away causing poor soldering of the large pad.

 

For a large pad under say a QFN64 I make an 3x3 array of solder dots which allows good process control of the amount of paste applied. One large aperture would cause the solder to not be evenly applied and the amount would vary.

 

This NXP App Note illustrates my comment: https://www.nxp.com/docs/en/application-note/AN1902.pdf

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Most IC manufactureres have a recommended footprint and that then includes the paste openings and vias to be placed. Best check them.

 

On a standard smd component the solder paste is as big as the actual copper pad.

 

Depending on the PCB manufacturer you need to have a solder mask opening that is a tiny bit larger than the copper pad.

Note that the manufacturers we use tolled us that we should just make the solder mask opening the exact pad size and that they in their process will create the bigger holes needed as it is done automatically.

So here too best check what their preferences is.

 

But the solder paste should not exceed the copper area and the solder mask opening size. .

 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

meslomp wrote:
Most IC manufactureres have a recommended footprint and that then includes the paste openings and vias to be placed. Best check them.

Absolutely! 

 

 

(Possum Lodge oath) Quando omni flunkus, moritati.

"I thought growing old would take longer"

 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

ki0bk wrote:

djoshi wrote:
I have been advised that on components such as QFN with a GND pad , that i should create small squares or circle, so that paste does not cover the entire pad.

Most likely you will want some vias so any excess solder can flow to the other side of the board, or else your smd part will float on this pad and prevent some pads on the perimeter from making contact.

Make some "test" pcbs with different size vias to see what works best for your particular smd part when run though the pick-n-place + reflow oven.

 

Jim

 

 

 

Yes there is vias at the bottom

Thanks

Regards

DJ

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

So should the solder past cover the whole pad, or should this be about 95% reduces in size?

 

 

Thanks

Regards

DJ

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

I am using Altium, does anyone know to make the Top paste layer smaller then then actual pad? It seems when i change the size size of top paste then entire pad changes it size.

Thanks

Regards

DJ

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

I am note sure if this is the correct way, but i found a rule that would allow me to reduce the top paste size as shown below.

 

 

This results in the grey (Stencil cut out) over the PAD(RED)

 

 

 

Thanks

Regards

DJ

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

djoshi wrote:

So should the solder past cover the whole pad, or should this be about 95% reduces in size?

Again it depends what 'pad'  you describe here. on a normal pad normaly the paste opening is the size of the pad.

For the Thermal relieve pad ( big pad under a component ) normally the parts manufacturer has in their datasheet a picture showing what the recommended opening is.

If you make that full size the part will potentially not be soldered correctly as the tin mixture on that big pad is used to pull the component onto the PCB and thus ensuring a good solder connection on all the outer pins.

That you want to include in your footprint as it is part specific in combination with the vias to be placed.

 

Reducing your paste mask can be done in the footprint of the component.

There is a paste mask opening extension parameter somewhere when you select a pad.

As I run a very much later version of Altium it makes no sense to make a screenshot as I know they massively changed the entire layout a couple of times.

Again. Normally you do not want paste mask expansion as it will impact solder quality.

Bigger opening might lead to short circuits, smaller will lead to bad solder joints.

Solder mask is a bit different. The amount of clearance between the edge of the solder mask and the edge of the copper is a manufacturer tolerance thing and thus depends on the manufacturer you use.

With that being a PCB manufacturer tolerance thing, most of them will be more than happy to do the modifications on the solder mask film for you as then they can make it optimum for their production process.

I am drawing PCbs for over 15 years now and only had to change the clearance once in that time period and that was because the factory had discovered a fault in their software and were working on a solution. As we did not have time to delay the production we asked them what they wanted, updated the design( then you just create a rule in the DRC agent and run a plane update and DRC check. then run the gerber output and all is done.  It kept us on schedule and later that month we were tolled that the expansion problem on their side was solved. So before you start messing with that... contact your PCb manufacturer on what they like best.