Eagle Design Aid - Ruler Library

Example 1 - 300When laying out a circuit board, it's essential to select the proper footprint for each component.  This can be complicated because different manufacturers have differing ways of referring to package sizes.  An handy example is the simple SOIC-8 surface mount package. The Eagle Microchip library has 3 versions of this package:

  • SO-08
  • SO-08M
  • SO-08W

Apparently, these are for narrow, medium and wide packages.  Which footprint should be used for the op-amp I'm using?  The first step is to check the dimensions on the manufacture's data sheet.

SOIC-8

Knowing the package dimensions is the first step.  To aid in selecting the correct footprint,  I've created a Eagle library containing a number of rulers.  I can place a possible footprint next to a ruler and quickly evaluate the size.  The illustration below shows the above mentioned package sizes.

Example 2

From the data sheet drawing, I can see that the pads should be about 4 mm apart in the center, and extend to about 6 mm from top to bottom.  The SO-08 footprint on the left above looks like the best option.

The next question is the pitch of the leads.  The data sheet says the pitch is 0.05" between centers.  In the rulers library, I've created some pitch gages at common spacings to quickly check the spacing.

Example 3 copy

This seems kind of trivial, but it's important to remember that PCB footprints are of varying quality.  Many of the Eagle (and other PCB packages too) libraries have been created by users and mistakes do show up from time to time.  The TQFP packages shown below should have a pitch of 0.80 mm.  The pitch on the smaller package lines up with the pitch gauge but the pitch of the larger package does not; in the span of 16 pads, the spacing is almost half a pad-width off!  The footprint would probably work alright but it would be difficult to align and solder.

Example 4

Errors like this occur when a footprint is created using Imperial measurements when it's based on metric or vice versa.  Data sheets show dimensions is both sets of units for convenience; the pitch of the SOIC package above is shown as 0.050" (1.27mm) but the conversion is approximate.  Over a number of pads, the rounding error becomes significant!

 The illustration below shows the various rulers in the library at this point.  It's very much a work in progress.  I hope it will be helpful in your circuit board designs.  Please let me know of any additions that should be made, or better yet, share your improvements here!  The library may be downloaded below.

Example 1

 

 

The library files have been updated as of February 3rd, 2013.  The origin of each element has been moved to be the lower left corner to make moving and deleting the element easier.

Ruler Library for Eagle 5

 

Please comment if you find this library or idea useful.

 

 


Posted: 5 years 7 months ago by Jon Chandler #12900
Jon Chandler's Avatar
I revised the library files to move the origin to the lower left corner of each ruler. This makes to easier to select the ruler for moving or deleting.
Posted: 5 years 7 months ago by Jon Chandler #12915
Jon Chandler's Avatar
I made one more change to the Ruler library. I added a 0.2" / 5mm pitch tool. This is handy for measuring the pitch of terminal blocks - the two sizes are very close, but not close enough to work well if the wrong size is selected for a circuit board.

Posted: 5 years 7 months ago by mai-au #12954
mai-au's Avatar
Hi John,

This is a great idea. But while I understand Eagle is a popular and capable PCB program, would you consider also sharing these as a PDF, DXF or maybe a Gerber file for those of us who are committed to using other PCB software. Of course I could apply myself to drawing my own, but it would be great if I could just "borrow" yours...

Thank's very much,

Martin.
Posted: 5 years 7 months ago by Jon Chandler #12956
Jon Chandler's Avatar
Hi Martin,

I think these are most useful as library / footprint symbols and less so as PDFs or Gerbers. I'm not sure if it's even possible to pull a Gerber file into an Eagle board layout (although that would be handy!). I think the layout program's native format is going to be the best to maintain resolution.

The hard part is done. Why not re-create them in the layout software you use, and post them here for others to use? It's your chance for fame and fortune....well, a little recognition at least . I don't want to hog all the credit!
Posted: 5 years 7 months ago by mai-au #12973
mai-au's Avatar
Hi again John,

I have re-read your original article (I must have just skimmed it the first time) and now I see that you are looking at these rulers from a whole different perspective to me. I thought the idea was to print these rulers out actual size then use them to interpret or verify the dimensions of the physical components in the real world, but now I see you are suggesting using them within the PCB CAD package to check the component footprints "on-screen".

I guess using them to check details "on-screen" is quite useful, though surely most PCB packages will let you easily measure and verify the distance between features on-screen with a few mouse clicks ? But I can see that sometimes positioning an appropriate ruler against a footprint on-screen could definitely be reassuring.

Still, I am interested in having a printed out (and perhaps laminated) version. Having taken an interest in this I will probably get on and draw up my own, which I may eventually share here, but you might like to consider uploading a "ready to print" PDF version of your rulers for people who don't use Eagle but might want to use your rulers in the way I suggest.

Best wishes,

Martin.
Posted: 5 years 7 months ago by Jon Chandler #12974
Jon Chandler's Avatar
I will admit when I needed to quickly measure something the other day, I created a new board, put down a 6" ruler and printed it out. There must have been a dozen rulers or tape measures close at hand, but I couldn't find one as easily as I cold print one


Using Eagle, it's surprising difficult to measure the width of a part or size of a pad. As far as I know, the only way to accurately do this is to open a part in the library editor, which of course means figuring out which library the part is in and where the library is saved before viewing the part. I need to find the ULP (user language program) that automates this again. But if you just watpnt to check the width of a footprint against the data sheet, the rulers are quick and easy to use.

By the way, the rulers are drawn in the TDOC (top document) layer in Eagle, so they are not normally included in the Gerber silk screen layer.
Posted: 5 years 6 months ago by fez #13092
fez's Avatar
Jon: thanks so much! Eagle has this really annoying discrepancy where can't knowingly zoom to 100%. I have to hold up a ruler to my computer screen and zoom in/out in eagle until dimensions start to match, only then am I made aware of the actual size of my layout and the involved components. Your library will assist me instead, now.

Forum Activity

Member Access