I'm designing a footprint . in this pictures we have vias and pads and i want to know is there any problem with that? i mean I've heard somewhere that something like this is a technology named via-in-pad and it is not much recommended because of some reason. i just want holes with certain radius and pads for them.
Considering this is the datasheet you pointed out and the component is SDF-009-US91-95.
This is what is called a Through Hole Connector or THT Connector. There is no need to include a SMD pad touching the pad hole. You only need to ensure the hole size is big enough for the pin and the pad hole is big enough for the solder. In this case you could use a 0.8mm drill hole and 1.3mm pad size
Something like this.
About the Via-In-Pad technology.
There are some misconceptions around this technology. In general, via-in-pad involves some kind of via plugging. This is the via is filled with a conductive or non-conductive material. Otherwise there will be some problems during the assembly proccess.
In general, this technology is not recomended unless you are willing to pay for these extra process.
Seems many of the comments to Anonymous's answer hit the nail on the head.
"Via-in-pad" is indeed a technology that is used but is generally not preferred for a number of reasons. The only benefit I can think of would be shorter signal paths which would help improve signal integrity in high-speed circuits, but its downsides are significant. 1) Solder can wick into the via so more solder would be required than usual. 2) If you use a reflow process, your stencil would need to reflect this, which would require either multiple processes (involving multiple stencils) or additional paste on other pads (not recommended if they don't have vias in them -- That could lead to solder bridges). 3) This would also increase the cost of the overall PCB (most board houses prefer to avoid via-in-pad technology if possible, because it's added time and resources to the build process. 4) Also, if the component pins are not properly soldered (solder is wicked down into the via) then it would take away from the solder on the pad and would leave a poorly-soldered joint that could cause intermittent failures.
There are a number of reasons I would avoid this unless you're sure it's absolutely necessary. I recommend not putting vias in the footprint at all, but place them during the board layout process. If you MUST put them in the footprint (I have no idea why you'd want or need to) then connect them to the pads using traces that are slightly narrower than the pads themselves (to prevent the traces from making the pads larger than intended) to connect to the vias (which are not placed on top of the pads).
That would be my recommendation.
Via in pad is actually recommended in some designs because they form shorter path.
This "via in pad" design may not be recommended for reflow and other automatic soldering methods because vias are filled with air before soldering, and when soldering starts, because of temperature increase, air in via expands, and may cause defects in soldering paste application, sometimes causing smaller parts to stand up on the board.
Based on the link you provide in a comment, you are making a footprint for a through-hole connector. In that case, we don't consider the holes in the pads as via-in-pad - via-in-pad only applies to surface mount footprints.
Since this is for a through-hole part (has pins that must go through the board) these pads are simply through-hole pads, and you get the holes as part of the pad definition - no need to place additional vias. You should not normally include the tracks (long pads?) you show when you make the footprint.