Ok, her my next question. It is a little bit generally and for my understanding.
There is a Solder Paste Layer in KiCad. That what i know is that the Boardhouse create a stencil out of this layer, right?
I finished my first footprint in KiCad except the Solder mask layer. In the datasheet is the speech about stencil design. Is it the same? I guess so.
But how do i this in KiCad on the solder mask layer ?
btw. luckly i choosed a easy Footprint for the beginning… 
thx
Zh4ng
No.
Solder mask covered all remaining copper on board outside pads. The main goal of solder mask layer is define the shape of areas which shouldn’t be covered. Solder mask opening (You may see it in detail circle on your image) is in ~97% cases bigger than copper pad. Remaining ~3% cases is reserved for special cases: smaller than copper pad (for BGA NSMD or same size as copper pad (not recommended, but sometimes used).
The PCB fab houses uses solder mask layer to prepare offset printer sieve when applying a covering paint.
Paste mask layer define the stencil cutouts. Paste mask is always smaller than copper pad because of the phenomenon of surface tension. This way during reflow, all liquid tin remains on the pad. For bigger pad it must be divided into smaller ones because it must be a place for escaping flux and air. See stencil design for center pad on your image.
The assembly houses uses paste mask layer for laser cutting (usually) of metal stencil used for applying solder paste on pads only, before SMT components placement. Punched holes are not exactly perpendicular to easily separate the PCB from stencil and keep paste on pads.
Ok, i understand. In my case, the design seems a bit more complicated. But how i get this solder paste design in KiCad?
Check out the B./F.Paste layers during plotting the gerbers…
If you got SMD’s on your board and their footprints are correct, they will create a proper stencil mask.
I think, that using the rules
It is possible to create any solder paste layout you need. It might need an additional trick to get the right solder mask, thoughts @Joan_Sparky?
you may have a look at this thread
Uuuuh, very interesting. Thx for the link 
Maybe this is the issue of wrong optical perception of scale, but I suspect your holes are bigger than recommended. They look like 0.4mm.
You are right. The holes are 0.4. I change the hole size to 0.3. Now it is datasheet confirm.
I also checked the soldermask clearance and now it even ok.
But i think 0.05mm soldermask clearance will be a Challenge for the Boardhouse.
Has anyone experience?
Depends on how much you are willing to pay, How thick your copper layer will be, …
You can increase the clearance a bit but be aware that there is also a minimum width for the resist.
(Just read the design rules of the manufacturer of your choice)
Another unrelated point:
I would change the silk layer a bit.
It does not really make sense tho have silk all around your part. (You do not add information this way.)
I would do it similar to this: (Light green is my suggestion.)
I would delete those silkscreen stubs almost touching the pads and extend the line by pin 1, IPC style rather than using the circle
Not to forget that some Chinese board houses aren’t able to do circles in silkscreen (in case you order from them)… quite funny if the boards come back and you can’t see the pin 1 mark.
And yes, that’s experience talking 
I just had a board come back with four large arcs that should not have there in the silkscreen. Some CAM software has problems. I am now thinking complex graphics have to be on the copper layer
Oh, that is nice 
I’ll take it.
Maybe i exchange the circle with a square or like davidsrsb a simple line.
