Step 17: The Design Rule Check

The Design Rule Check (DRC) checks the board you designed against a set of rules to determine if you made any errors.  While it isn't perfect, it will catch a large amount of common mistakes.

A quick description of all of the tabs:

File - Allows you to pick which DRC file to use.  If you are with a group, they might already have one, and services like OSH Park have a downloadable .drc file that you can Load here.

Layers - Since we are using the freeware version of Eagle, you can't really play with this one, but if you have one of the paid licenses, layers can be added by changing Setup to be something like (1*2*15*16)

Clearance - This tells Eagle how much room you want between the different types of electrical contacts on the board.  If you want, you can everything under Same Signals to 0.  OSH Park has a minimum clearance of 6 mils for everything under Different Signals.  If you are fabbing the board at home, 20 mils is a reasonable clearance.

Distance - Copper/Dimension is the distance from any routing to the edge of the board.  Drill/Hole is the distance from any routing to a hole in the board.  

Sizes - Set the minimum sizes.  Minimum Width is another number you pull from your fab house, OSH Park has 6mil, if you're etching it yourself, it should be around 24 mil.  Minimum Drill for OSH Park is 13mil, if you're etching it yourself, pick whatever the size of the smallest drill bit you have is.  Micro and Blind vias are far beyond the scope of this instructable

Restring - Restring controls the size of the through-hole pads/vias.  Typically I just leave these at their default values.

Shapes - Allows you to make pads have rounded edges.  Typically I don't touch this one either.

Supply - Remember Thermals from up above?  This gives you a bit more control over them.  The checkbox allows you to turn on thermals for vias, and Thermal Isolation lets you pick the length of the thermal traces.  Typically I don't touch these values at all.

Masks - When PCBs are fabricated, they have a coating that covers and insulates all of the board, except for areas designated by the stop mask.  After fabrication, if they are being assembled by a machine (or a person with a reflow oven), a stencil is created and solder paste is applied via that stencil to the pads/vias that need to be soldered.  Stop controls the size of the openings in the stop mask for the various parts, and Cream controls the size of the openings in the stencil.  Once again, the default values work just fine for our typical usage.

Misc - 
-Check Grid - When you lay out and route the PCB, everything you do is on a grid, whose sizes are determined by the Grid command.  If you changed the grid partway through layout/routing, this will ensure that all of your parts obey the new settings.
-Check Angle - If you routed anything with a different style than the 45- or 90-degree turns, or if you moved a part after routing, checking this box will make Eagle yell at you for doing that.
-Check Font
-Check Restrict
-Max. length difference in differential pairs - Differential routing is where two traces are routed side-by-side and carry a signal that is differential (when wire A is 1, wire B gets set to 0.  If A-B is greater than zero, a 1 is being sent, otherwise a 0 is being sent).  There are several advantages to this, one of which is what is called 'Common Mode Rejection'.  Essentially, most electrical noise more or less adds a voltage to a given wire.  If two wires are close enough, the same voltage (let's call it v) gets added to both.  With differential routing, we want those two wires to be affected by the same v, so that the v cancels out of (A+v)-(B+v).
Back on track to what this option does, we want the length difference to be minimal so that the wires pick up the same noise.  This allows you to pick what difference to choose.
Gap factor for meanders for differential pairs - For high-speed signalling, you want both wires in a differential pair to be the exact same length.  Depending on the routing, this may not be the case, so to make the shorter trace match the longer one, a 'meander' is put in.  The Gap Factor adjusts the size of these meanders.

After you get all the settings the right way, click Check.
(after setting all of this up, you can just type 'drc' and hit enter twice to run the drc again)
<p>The Display button is the icon with the &quot;layer settings&quot; hover-text, and looks like 3 colored squares. It is just below the Info button.</p><p>To run an Electrical Rules Check, click the &quot;Errors&quot; button, which looks like a yellow triangle with an exclamation point (!).</p>
<p>I followed your guide and found that it was very useful! Everything was easy to follow and straight forward! I've already been applying what you taught me to some my very first PCB's. Thanks for the great guide!</p>
thanks for posting! what pcbs have you made? have you posted projects around them?
I've made a dual 500W Motor Controller, above compass board (although I haven't had time to assemble it after I got it back from the fab a while back), a LED-based wireless quadrature signal transmitter/receiver pair (fabbed, assembled, in debug), and a wireless e-stop (failed first etching attempt and haven't had time to retry).<br> <br> <a href="http://www.youtube.com/playlist?list=PL56A0A84AC4CC037B&feature=view_all" rel="nofollow">Youtube video playlist of the full robot in action</a>

About This Instructable




More by killersquirel11:Arreglo fácil para auriculares con cables rotos PCB Creation with Eagle for Beginners Part Selection Guide for Building a New Computer 
Add instructable to: