Hi CSNeto, Welcome to EasyEDA. You draw the package PCB footprint outline in almost the same way you draw a schematic symbol outline. Do: **Document > New > PCB Lib** then, in the Layers panel, select and show the **Top Silk Layer** (click on the colour and on the visibility to toggle the eye icon on). Next select the **Track** tool from the **PCBLibs Tools** palette (or the `W` Hotkey) Draw your outline. ![enter image description here][1] Then add the pads and check the pad names and numbering. Please also see the EasyEDA Tutorial: https://easyeda.com/Doc/Tutorial/PCBLib.htm#CreatingThePCBLibs [1]: /editor/20151103/5638760a49d82.png

When you have finished, don't forget to fill in the **Package** and **Pre** Custom Attributes: ![enter image description here][1] and then Save it. The New part will then appear in your My Parts folder. It will also be publically searchable using the SHIFT+F search. [1]: /editor/20151103/56387851b2ccc.png

I appreciate your prompt reply, Andy Fierman. According to what was explained, the EasyEAD, from silklayer information calculates the spaces between the components. Thus, avoiding the possible overlapping of components. Right?

You can try it out and let us to check your compoents. just need to share them . We will check it for you to find problems .

Here's how it works. Starting from the dimensions given in the manufacutrer's datasheet, you have to work out an outline that encloses the maximum dimensions of the package so that if you place the outline of one part right next to the outline of another, they are guaranteed to not overlap. Don't forget that some parts may need more room above the PCB than at the PCB level. A simple example of this would be TO-92 packaged devices. So, you may need an outline that is bigger than the pins themselves may require. Or maybe you want to make use of the space under the body of the part. Then work out the pad dimensions. For through hole parts you also need to specify the drill hole dimensions. Remember that the finished hole size is a little smaller because it is filled out by a thin layer of through plated copper. You need to try to find out if the datasheet specifies finished (plated) hole size or drill (unplated hole) size. This is not always obvious so you may simply decide to oversize the holes. Unless you are tight for space or need to get tracks between pins, this is usually the safest solution. Parts may be a little loose until they are soldered but at least they will fit! Maybe for an 8 pin DIP you want the outline to enclose the pin pads. Maybe you only want the chip body inside the outline. These choices are yours. Be careful to not put silkscreen over the pads: leave gaps if necessary. Make it clear which way round a device is fitted. Mark the cathodes of diodes, pin 1 of chips and connectors, the + side of electrolytics and so on. It is good practice to make these markings so that they are visible after the part is fitted to the PCB to make debugging and repair easier. Once you have worked out the dimensions of the outline then you can set the PCBLib canvas **Units** to mil, mm or inch. Set a comfortable Grid and Snap size. Don't forget that you can change the snap size for example to help close a rectangular outline or to make sure lines are accurately oriented or aligned. Then draw the outline. Then size and place the pads. **Check that the pad numbers match those of the schematic symbol.** **Check that sure the pin numbers on the schematic symbol match those of the device you wish to fit!** ***Do not assume: check!*** Keep an eye on the XY co-ordinates to check regularity of pin spacings and symmetry. * **Note that EasyEDA does not calculate or check your dimensions: it just shows what you draw.** Remember that if you make a mistake then you pay for it in the cost of a 2nd PCB spin. :( Soooooooo, it is up to you to dimension your footprint correctly and to check it. Then check it again. Go away, make tea and then check it again. :) It is possible to autogenerate both schematic symbols and PCB footprints but as far as I know no-one has yet made a plugin publically available for these tasks: https://easyeda.com/Doc/Tutorial/new.htm#APIPlug