Converting a PADS Library to Allegro

[PRoehl]

Hello-

My Company is considering upgrading our OrCAD Layout licenses to Allegro. We also use PADS and have a much larger library. Is there a way to import a PADS library or translate it to Allegro?

Thanks in advance-

Paul

[Skip Yutkus]

It can be done and you may be able to find vendors to do it for you, should you choose to translate your Pads library yourself it's not hard to do but a real pain in the ass, the biggest problem being that Pads does not use discrete "pads" no pun intended! when you translate a part the different size padstacks will come through as pad1 pad2 pad3, ad infinitum, these are useless for use in building future Allegro parts as they have no descriptive info, you must edit each one and save it with a descriptive name IE: pad125c106d.pad, (.125 pad with .106 drill). You also need to fix things like missing soldermask clearance and pastemask, and last but not least the ref-des only comes thru on the assy dwg. layer and must be copied to the silkscreen layer. We are currently doing it on an as-needed basis and for me personally symmetrical parts like BGA's are so easy to build using Allegro's wizard it's not worth the work to translate.

Skip

[PRoehl]

Thanks Skip-

We have a smaller library in OrCAD Layout, that may be easier to import into Allegro. OrCAD uses individual padstacks, and defines soldermask and paste. That might be a better way for us to go.

Paul

[cadpro2k]

Hi Proel,

It's actually pretty easy, but it WILL be time consuming for a couple reasons.

1) Allegro uses padstacks in their library parts, PADS doesn't
2) Your layering will probably have to modify.
3) Renaming stuff takes time. Blah, Blah, Blah.

Here's how:

1) Make an excell file containing all the parts in your PADS library. 2) Make a 'parts' file (text file to import into PADS).
3) Place all your library parts in a PADS board file.
4) Create an .ASC file from this board file (make it at v3.0 or 3.5). 5) In allegro, translate the .ASC file into an Allegro .brd file.
6) 'Dump_library' routine from the Cadence toolset (shell command dump, you'll find it in the HELP section).
Now you have all the parts from PADS. Next is to make them 'useable'. THIS is what takes time.

Been there; Done it. BUT, it does work. I've even converted PADS boards to Allegro.

Now, if you want to purchase the latest IPC-7351 library... see www.pcblibraries.com I'm sure you know that.

Good day.

Mitch

[Skip Yutkus]

Mitch,

That had to have taken months - what about the pad1 - padxxx problem, and the fact that thru hole pads will have invalid shape definitions for thermals, that's an enormous task unless you standardized while building your Pads library to minimize the number of pad sizes. If there is an easy way to correct those problems I'd really like to know, I could be wasting a lot of time.

Thanx!

Skip

Hey, have you built a part with the LPWiz and read it into Allegro? It's really entertaining to watch! Kind of reminds me of my old DOS software recordable macros.

[cadpro2k]

Hi Skip,

Yes, it can take some time. Depends on how "Golden" your PADS lib is. But, I converted a PADS layout last night, replaced the 'converted' parts with Allegro library parts, replaced the plane layers, and sync'd it to the Capture schematic in a matter of a couple hours (including all the 'reference' layers - i.e. fab/assy stuff). It's not at all 'automatic', but once you know the conversion process, it's doable.

Yes, the padstacks and naming are a problem, but it could be streamlined by using a SKILL contractor (not me) to script the routines.

I personally wouldn't do a whole library, but would take it on a boardXboard basis to begin.

Good day.

[Skip Yutkus]

Yup!

Same thing we're doing here, I was just hoping there was an easier way, funny how it sounds so automatic when they sell it to you!! LOL

Thanx,

Skip