Following the same way that we did with the previous articles, we now have to design the component PCF8563, which is a real-time clock module. This time, I didn’t find any component like that on Sparkfun’s or Adafruit’s library. This time you really might need to draw the component!

The complete list of this series:

First steps

First of all, open the datasheet here. Go to section 15 – “Package Outline”. There you find how the component is, and where is located each pin. All we need to do is to design the footprint according to this drawing. We are going to design the SO8 package.

Open EAGLE, on the main window, left panel, open your library folder. If you configured correctly the library on the first tutorial or you did the second tutorial, you should have a folder! Now select your name on the library panel and go to “File”, then “New” and finally click on “Library”. Before anything, save your file. Go to “File”, “Save as”, and save the file as PCF8563 inside your library folder. Great, let’s begin.

Designing the package

Click on the “Package” button and a window will appear. On “New” box, write the package name. This is the name of package size, i.e. for the PCF8563 that should be SO8. Select “Yes” to create new package with that name. Before drawing the part, go to the “View” menu, then “Grid” and change your units for millimeters, place the “Size” to 1 mm and “Alt” to 0.5mm.

Click on the “Wire” button from the toolbar, select tDocu from the layers’ menu and draw two rectangles. After that, click on the button and change the properties from the geometric figure to fit on the package size defined by 5 mm x 6 mm. This layer won’t be printed on the PCB, but it helps you when designing the part. If you have any doubt about how to draw the piece, consult the datasheet dimensions. For example, the outer rectangle will have origin on the coordinate: (0,0), then go to (6, 0) to (6,5) and finally (0,5) to (0,0). The inner rectangle will have origins at (1, 0) and then (5, 0) to (5, 5) to (5, 1). Your drawing should look like the image. Put an inner rectangle at “tPlace” layer to show where the component will sit and draw a circle in it, near the pin number 1.

Now draw the pads. Click on the SMD pad button . Insert one pad anywhere on the screen. Click on the information button again and change its proprieties, like the place and size of it. Put it on the coordinate P1 = (0.3 , 4.5) with size 1 x 0.5 mm, a little larger than on the datasheet. Now copy that pad with the copy tool . Place all the other 7 terminals around, right clicking it to rotate, when placing the pads on the sides. After that, just position each one on the correct place. It will look like this image.

Click on the name tool and change the pin names for 1 to 8. Beware to put the pin 1 on the upper left pin, and that the pin 8 is on its right side (top view – looking through). At last, select the text button and write “>Name” and “>Value” over the tNames and tValues layers, respectively. OK, your package is ready! Save and get out!

Adjusting the symbols

Now go back to the device creation window. You might need to open your new library file again, and click on the “Device” button. Write it on the “New” dialog box PCF8563. Save the file as PCF8563. Now this part is easier. The module has 8 pins, and all are connected. Click on the wire tool and select the Symbols layer. Draw a box of any size you want. After that, select the pin button and place all 8 pins. Remember that you can change the pin size on the top menu, as the image shows. Also, remember to right click when placing the pins if you want to change the side that the pin is. By right-clicking you can rotate it.

After putting the pins, you can name them! Select the name tool once more and name the pins according to the datasheet. Now select the text tool and write “>Name” to the Name layer and “>Value” to the Value layer. Simple as that. There you go! Your schematic should be ready like the image below.


Still, you might notice my pins are noted as “io”, or “pwr”. You are probably thinking I set some configuration to each pin, and you are right. You can click on the correct tool for this, as on the image, and set each pin type. This will help when EAGLE checks the rules from your circuits.

Connecting the pieces

Save again your work and you are ready to connect the pins and pads. You can do that by clicking on device the button. Name it PCF8563, and create it. First of all, on the new window, click on “Prefix” button (down there) and write a big and capital “U”. Now “OK”. Select the “Add” button and put your new PCF8563 you just created. Above the “Prefix”, click on the “New” button and select your SO8 package. After all this work, you will see an exclamation mark near the package name.

Select the “Connect” button and associate each pin to a pad. Of course, as this pressure sensor has unused pads, some of them won’t be assigned to any pin. There’s no problem on that. However, if this was the opposite, a pin without a pad, you would have problems. The final step is to add a description to your device. Save it and we are done! Cool!

Conclusions

This time we don’t have any other library to compare our component, but as we followed correctly the datasheet, this design should work just fine!

Where to go from here

  • Designing The Parts V (Or Downloading) – AT24C64;
  • Schematic I – The Arduino Pro Mini;
  • Schematic II – The Sensors;
  • Schematic III – Other Modules;
  • Board Designing;
  • Generating Files.

Leave a Reply

Fill in your details below or click an icon to log in:

WordPress.com Logo

You are commenting using your WordPress.com account. Log Out /  Change )

Google photo

You are commenting using your Google account. Log Out /  Change )

Twitter picture

You are commenting using your Twitter account. Log Out /  Change )

Facebook photo

You are commenting using your Facebook account. Log Out /  Change )

Connecting to %s