Adjusting tstop size in footprint editor

Hi,

When you need a special shape pad, you draw the copper with a polygon and add a smt pad, smaller of course, inside the polygon. Eagle will automatically associate the pad and the polygon.

Then you disable the 'cream' and the 'stop' of the SMD pad (properties of the pad).

Then you draw the cream aperture, as with polygon (or recatangle, or circle... ) in the tcream layer.

Do the same for the stop mask (tstop layer).

That way you can do define all the shape you need, and the shape of the cream and the stop could also be different from the copper shape.

The DRC must be adjust in order to define how the the mask will be adapted by eagle : DRC -> MASK.

For the size of copper, stop....

Keep in mind how the PCB is build. The stop is done after the copper, and the mask used to do the stop, is applied a on the board, and must be aligned. There is always a little alignment error between the stop mask and the copper itself, and there is always dimensions variation between the two.

Even if theses errors are tiny, in the end, even if you design use the same shape and dimension, the superposition will no be exactly OK.

So there is 2 ways to do this:

- stop defined pad: the pad is larger than the stop aperture, and the final size of the pad will be defined by the stop (the solder will be stopped by the stop mask).

- copper defined pad: the pad is smaller than the stop mask, the final size of the pad will be defined by the copper (the solder will be stopped by the edge of the copper).

In both case: the difference of dimension of the two shape ( all around the shape), need to be adapted to maximum alignment error the board house can guarantee... So you have to check with the board house. If you don't respect that, you may have pads that are limited by copper in one direction, and by the stop mask on the opposite direction (and they will have a strange shape).

Now you will ask which one is the best...

There is no better/worse. You have to select witch one is best for each pad...

Example #1: device with very small pitch : you can not use an aperture a little larger than the pad for each pad, because the distance between the 2 aperture is to small (check the minimum distance between 2 stop mask aperture, of your board house). So you you will have a single aperture in stop mask, that will cover several pad -> copper defined pad.

Example #2: on a big thermal pad, you need to have a huge GND plane, without thermal, and you certainly don't want to limit the size of the pad to the solder area: you draw a big pad or polygon, larger than the pad of the device itself, and define the solder area by drawing a polygon on the tstop : stop defined pad.

So have a look to the part application note of your device, sometime there is some solder information.... and ask to your board house they will certainly give you a document with all the limit you have to respect....

and then you can start wondering how to deal with cream....

Guillaume.

On 12.10.2015 17:16, Michael Basford wrote:

Hi all,

 

I am looking to create a footprint for this component:

http://media.digikey.com/pdf/Data%20Sheets/NAVMAN%20Wireless%20PDFs/Jupiter%20SE880%20User%20Guide.pdf

 

However, the footprint (in section 6), requires custom shaped pads. To

do this, I was planning on adding some very small pads, and then drawing

out the real copper pad size and tstop layers with the polygon tool.

However, it seems by default tStop is 0.1mm added onto each side of the

pad. This means if I need a pad of size 0mm to get the correct tstop

size (0.2mm from the above datasheet). Is there a way to adjust this

tstop size?

 

Furthermore, I was wondering what your opinions are of having the copper

pads larger than the tstop area? This is what the datasheet seems to

suggest, but I would've thought this was a bad thing to do? How would

others here create a footprint for such a component?

 

Many thanks for your time, it is most appreciated.

 

S

Check the NOTE:

"The area in yellow is not the actual size of the solder land and it is

governed by the PCB design rules defined by the device integrators"

In practice, a professional PCB manufacturer wants to have control of

this size. They usually ask me to make it exactly same stop the same

size as the paste, so they can tweak them all on a global scale.

For less professional work, just make sure there will be some stop

between pads to keep some solder flow tension.

Hi,

In practice, a professional PCB manufacturer wants to have control of

this size. They usually ask me to make it exactly same stop the same

size as the paste, so they can tweak them all on a global scale.

 

It's true that the paste need to be adjusted to the solder process, (in case of the use of a paste mask, the aperture depend on the thickness of the mask, if the paste is applied by micro jets, you have others parameters...)

Usually, I try to follow the advices from he company that will solder the board and the components manufacturers. Then the company that will solder the board do final adjustment (with their experience they do better, and during prototyping, they run some test). In the end, the mask is not exactly the same than my original version, but it's for the best .

But they never ask me to do exactly the same dimension for paste and cream.... I  discus that point (last month) with a guy who is in charge of that (adjusting), he told me that my design was fine enough that way. (I don't know if it's really true, or if it's because he didn't want offend a good customer...)...

Guillaume.