10
\$\begingroup\$

What facilities does EAGLE CAD have for helping to do layout with matched length groups and differential pairs? Can you apply such a constraint in the auto-router? As a follow-on to this, what (other) free Electrical CAD tools support this type of feature?

Edit If you don't believe any free CAD packages support this design feature, what are some low-cost options that do support it?

\$\endgroup\$
6
\$\begingroup\$

Eagle actually has both of these features as of version 6. From their website:

Benefit from differential pair routing and automatic meanders

Special signals can be routed with exactly the same length. Differential pair routing is used for pairs of differential (equal and opposite) signals across the board to create a balanced transmission system. Creating meanders helps users automatically give a signal a certain length in the PCB. Meanders in traces are used to increase delay times in high speed digital circuits.

http://www.cadsoftusa.com/eagle-pcb-design-software/new-in-v6/?language=en (halfway down)

See for yourself.

The Meander button:

enter image description here

Length matching of a differential pair (from manual):

enter image description here

I don't actually know how to implement these techniques, but I can point you to the documentation. Check the manual (warning 300+ page PDF) on page 175 to 178 - http://www.cadsoft.de/wp-content/uploads/2011/05/V6_manual_en.pdf

\$\endgroup\$
  • \$\begingroup\$ awesome, I'm still using 5.11, but this may be a good reason to update! \$\endgroup\$ – vicatcu Feb 18 '12 at 3:46
  • \$\begingroup\$ Yeah, version 6 is really cool. You will probably get a discount for upgrading too. \$\endgroup\$ – Chris Laplante Feb 18 '12 at 3:49
8
\$\begingroup\$

Here's how I do equal length differential pair routing in Eagle CAD:

  1. Name traces D_P and D_N (or something _N and _P - seems like Eagle CAD needs the suffix).
  2. Create net class in schematic and add both traces to it
  3. Route the traces, either together (the default) or separately (type ESC and Eagle CAD will stop routing the second trace).
  4. In board view, type run length D_* in the command window
  5. In the dialog box that comes up, click on longer pair length, copy it (Command-C works on my Mac)
  6. Type meander [copied length]mm, but replace [copied length] with the value you just copied (Command-V to paste works on my Mac) into the command window. mm means millimeters, length.ulp measures in mm
  7. Click on the shorter trace to meander it.
  8. Move mouse to meander the shorter trace until its length is the same as the longer trace and the meander pattern is to your liking.

The Eagle Cad v6 Manual p175-178 helps.

\$\endgroup\$
  • \$\begingroup\$ run meander [length]mm throws an error: cannot open 'meander.ulp'. I was checking my ulp directories but I could not find any meander.upl. I usually use Eagle 6.1.0 but even with 7.6.0 no luck. Your answers sounded like it was already included in the default installation. Do I have to download it somewhere? \$\endgroup\$ – milkpirate Aug 8 '16 at 9:34
  • \$\begingroup\$ @user3097432 My instructions were wrong, just updated them - you don't need the 'run', just type 'meander [length]mm' but replace the [length] with the number of mm you need. \$\endgroup\$ – Adam F Aug 10 '16 at 4:21

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.