1
\$\begingroup\$

I'm tring to make some sort of shield board (it's not an arduino):

  • first board was made in orcad, I have source files gerbers and so on...
  • I'm making a 2nd board in eagle.

When trying to align the 2 boards mount holes and connectors I am having some trouble.

I tried exporting pdfs of each board and importing into gimp and inkscape, but the boards get rezised and im afraid it doesnt work.

Sometimes I get huge files and computer crashes...

I would apreciate ideas on how I could align the boards. What would be the right way to do this?

\$\endgroup\$
5
\$\begingroup\$

Use DXF... (it's designed for this)

DXF is a file format. It stands for Drawing Exchange Format... as in exchanging CAD data between systems.

  1. Export your OrCAD PCB outline and drill holes as a DXF drawing
  2. Import your new DXF as a layer into your EAGLE layout
  3. Use the new layer to align your EAGLE parts (you may need to do this inside of a part if you are footprinting a shield template)
  4. Remove or disable the drawing layer (it's just a reference, EAGLE can't do anything else with it)

DXF import in EagleCAD

Try the importdxf ulp that's up on www.cadsoftusa.com -> Downloads -> User Language Programs

All you have to do to use it is type RUN followed by enter in one of the editors. Browse to the ULP and hit open. The ULP will now run and present you with an easy to follow dialog.

Alternatively...

...use an in-between format. I found that inkscape (freeware) is good at reading DXF and can convert to HPGL format. HPGL format is easily converted to EAGLE script format.

| improve this answer | |
\$\endgroup\$
4
\$\begingroup\$

The mount holes are likely to be a specific drill size and there's usually not many of them. Open the drill file (usually Excellon format and it'll be supplied with the Gerbers) in any text editor and read the raw coordinates, they won't be too hard to find.

I don't know Eagle so I won't tell you how to place your new holes on exact positions.

When you're done, generate a drill file from the new board and compare holes for the appropriate drill size with the original. (Use a spreadsheet to subtract offsets if your new board has a different origin position)

| improve this answer | |
\$\endgroup\$
1
\$\begingroup\$

You can open the Orcad design file (probably the .MAX file for the PCB) in the (free, downloadable) viewer and look at the mounting hole coordinates. Or use Orcad itself if you have it installed. Click on one of the pads, then open the spreadsheet for 'footprints' and you will see something like this (the one you clicked should be at the top and highlighted):

![enter image description here

If you want to use Brian's method, the default Orcad Excellon file name is a text file named THRUHOLE.TAP and the relevant section would look something like this:

T12C0.138F200S100
X001000Y002750
X001000Y022750
X026000Y002750
X026000Y022750

This is tool 12 (T12), diameter (in inches in this case) of 0.138 with some more-or-less random downfeed rate (200 inches per minute) and spindle RPM (100,000)- those numbers will be replaced by the PCB manufacturer most likely anyway. The tools are in sequence from T1 onward, not necessarily sorted by size. This file was (as usual) done with absolute coordinates, not incremental, and the holes are at coordinates (in inches). The number of digits may vary, as may the units, but inches are still most common.

In inches, the coordinates are as follows: (0.1, 0.275),(0.1, 2.275),(2.6,0.275),(2.6,2.275)

If you are trying to align connectors, I suggest using the pad locations rather than the component locations.

This is a big pain, especially when switching EDA systems. Recently I saw hundreds of boards scrapped because the designer misaligned a couple mounting holes by a bit over 1mm. Not much, but enough. Fortunately, it was caught before the boards were populated. So I suggest listing and double/triple checking all the critical alignment coordinates. Comparing the Gerbers might be worthwile.

| improve this answer | |
\$\endgroup\$
  • \$\begingroup\$ thanks for your answer : how do i access the footprint spreadsheet on orcad 16 ? \$\endgroup\$ – Cristian Mardones Apr 21 '16 at 16:19
  • \$\begingroup\$ The icon that looks like a grid and has a rollover tooltip "View Spreadsheet". That's assuming Layout. If it's another Orcad PCB program, I don't know. We switched from Orcad before converting. \$\endgroup\$ – Spehro Pefhany Apr 21 '16 at 16:22
0
\$\begingroup\$

The trick was: -take reference coordinates from orcad -make a calculus in excel , to transpose to eagle relative coordinates -apply relative coordinates to eagle board. -export to DXF in eagle -LASER CUT the eagle board in Plexy glass

this way i was able to test 100% of alignment: mount holes + connector pins !! marvelous , board arrived , NO SURPRISES !!!!! i slept like a million dollars !!

| improve this answer | |
\$\endgroup\$

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.