Silkscreen Sizer and Solder Practice Board

Let's make something simple to start to finish: a silkscreen size checker and component solder practice pad.

(Side note, if you don't have Greenshot for screen captures, go download that. It's amazing and free: http://getgreenshot.org/ It also comes with plenty of snap to window options!)

In Eagle we first create a project. (Right click on the eagle folder and click new Project)
This also creates a folder on your system. For me the folder is in Documents\eagle\SilkscreenSizeBoard.

Now let's add a schematic: (Right click the project and add new schematic)

It looks a bit barren, so add a quick frame to start off (Use the Add part button and look for the frames menu --> Choose the A3L-LOC option). 

After click okay, put the bottom left of the frame at the origin of the schematic:

 Now the schematic is ready for a quick description in the frame (most of the information is automatically added, but put in a bit more using the Text Tool) Also you'll want to change the Layer after adding the text to be on the Info Layer (in the top left of the GUI). This allows us to change the visibility of the schematic if we wanted to.

Also assign useful key combos to tools. Saves time on clicking the same tools over and over. Access these under the Options Menu --> Assign --> New to make a new shortcut. A few of the ones I have mapped are shown below: (Eagle tends to ignore previous version hotkeys so I'm always remapping them)

To make our board more interesting we need components. We will add some caps and some through hole parts. Use the Add Part tool and look for the resistors library:

I used the 0201, 0402, 0603, 0805 and 1206 resistors and caps from the C-US and R-US folders within the resistor library. 

After adding some identifying text and some copy paste, we have 5 of each package (while the size is the same for both, the tDocumentation is different). 

While resistors are fun to solder, ICs are also good to learn. How about some SOICs, TSSOPs and SOT23s? (Add using the Add Tool and search for the names)

The next step is to create the board. Click the Generate/Switch to Board tool:

If the board doesn't exists, Eagle prompts for the creation of a board. With the board, we now have to place all the components: 

On the right half of the new board we can see a black rectangle outlined by orange. The orange line defines the board outline (edges of the PCB). The light grey area is outside the board and is not valid for components. Move all the components inside the board area.

Move the board edge (orange) to be slightly larger than the right half of the SOIC chips.

I've also added dimensions using the Dimension tool 

 

Click the two points to measure between. Also use change the Dimensions to inches and set the layer to Document. DO NOT SET THE LAYER TO DIMENSION!!! This will mess up the Gerber files as the PCB manufacturers could mistake the rulers for part of your design! Osh Park is one example of this! After this we will add some Silkscreen to the board to identify everything. Use the Text tool and set the layer to tPlace (placement of Silkscreen on the top layer of the board). Everything looks pretty good! (It looks clean because I turned off the Unrouted, tNames, and tValues layers). 

Now to make it look even better, we'll use a ground pour. Use the polygon tool and create a rectangle the same size as the outline. 

If the polygon is closed, hit ratsnest to finish the board and make the red pour appear!

For the bottom, I added a bunch of silkscreen sizing and a ruler in inches and mm. All of the silkscreen is easy to size using the size parameter when placing the text or afterwards by using the Info tool. The ratio of the silkscreen can also be changed to make the text appear bold. This is helpful is you're trying to add a top or bottom indicator in copper. 

This has a number of different sizes of silkscreen, traces and components. All of this is to get a size reference for everything. The last steps are to check the rules, then export for the board house, in this case OSH Park. 

Some manufacturers offer Design Rules (DRUs) to check the board for any errors before manufacturing. OSH provides the rules here: http://docs.oshpark.com/design-tools/eagle/design-rules-files/ Look for the Design Rules for the corresponding Eagle version. There also a number of tips for designing boards in Eagle here: http://docs.oshpark.com/design-tools/eagle/   

Since I'm including a bitmap (like shown in this tutorial: http://www.instructables.com/id/Adding-Custom-Graphics-to-EAGLE-PCB-Layouts/), I had to check my bitmap against what OSH recommended here: http://docs.oshpark.com/submitting-orders/import-bmp/ 

The original image I used was here: Scorpion Image After downloading in .png, it had to be converted to a monochromatic bitmap via Paint of all programs. After resizing it a bit in Paint, the import in Eagle was easy (make sure to set the scale to 2  mil per pixel to match what OSH says!)

The layer for the bitmap also needs to change once you're happy with the image. Select everything in the bitmap and the the Change Tool --> Layer to accomplish this. Choose the layer to move the selected bitmap to. Then CTRL + Right Click the selected bitmap (to move everything to the other layer). It should then move to the new layer. In this case, the bitmap is on bPlace.

After downloading the rules file, Eagle has to be told to use that file. Open the DRC (Design Rule Check) tool. Then click the load button in the bottom right. Browse to the .dru file downloaded from OSH. with the .dru file loaded, click Check to check the board with the new rules. 

This opens the results of the design rule check. For this board, the only errors are unrouted "airwires." Normally this is a MAJOR problem and should be addressed (as something in the design is unconnected)! However for this design, there are no valid circuits on the board and we can leave them unconnected. 

If there are no important errors, the next step is to generate the gerbers (the board manufacturing files). OSH provides a specific file called a CAM job that exports these automatically for us. It is found here for 2 layer boards: OSH Park CAM Job

After downloading that, use the CAM processor to open the job:

After opening the job, we need to make a quick change to the Top and Bottom Silkscreen parts of the job. If you click on the tab for Top or Bottom silkscreen, we want to unselect tNames and bNames from each tab. That way the tNames and tValues do not get counted as silkscreen. 

With that done, now process the job to generate the gerbers. After that we need to zip up the gerber files for export to OSH's site. Select all the .ger files and the .xln file and send to compressed .zip. These files are generated in the same folder as the schematic and board file. 

Finally upload the gerbers to OSH here: https://oshpark.com/uploads/new 

The first page after uploading the gerbers shows the whole board and gives approximate pricing for 3 copies of the board. Give the board a good name and description and put in an email for the order.

On the next page, carefully look over each layer! Here we can see the logo on the bPlace layer!

When you are sure the board is ready and no errors exist, then go to checkout an order those boards!

For a normal 2 layer board, the turn time is around 12 days and free shipping usually takes 3 to 5 days on top of that. So I hope to see these boards in about 2 weeks! Thanks for working through this demo!

UPDATE 12/18/17:

Boards are finally back and look really good!

Note that OSH sends boards back with small nubs that space the boards out in the overall panel they get from fab. Looks like they don't support less than 8% ratio on silkscreen, but this was a test. The silkscreen scorpion looks awesome!