Hi....first post on this forum.I'm new to OrCAD, working on a fairly simple design. I have my schematic complete in Capture and I am currently working on designing footprints for all parts in order to generate a valid netlist to port over to PCB Editor (v16.2). 90% of my parts are SMT...I found the design process for SMT symbols pretty straightforward. I'm now getting into designing footprint symbols for my thru-hole parts and I'm getting stuck.In pad designer, I'm not quite sure how to properly define the sizes for thermal relief and anti pad. Looking through some of the supplied .pad files in the ...pcb/pcb_lib/symbols directory, I see many thru-hole .pad files, but they all vary so much, I'm not sure what a good "standard" would be.For example, say I am designing a simple two layer board. I have a part with two leads that will mount thru hole. Say the nominal lead diameter is 24 mils. I'll add ~6 mils to the nominal to find the proper hole diameter, which works out to 30 mils. So I figure a good pad diameter for the top and bottom of the board would be twice the finished hole, or 60 mils. So now I attempt to design a .pad file for this:- two etch layers, two mask layers, type is "through"- hole type is circle drill, plated, with a 30 mil drill diameter- for the top layer ("BEGIN LAYER"), I define regular pad as "Circle 60" and anit pad "Circle 70" (since I want a 5 mil annulus around the pad, right?). Does thermal relief need to be defined here?- What do I enter for the "DEFAULT INTERNAL" layer, regular, thermal relief, and anti pad- I define the bottom ("END LAYER") the same as the top ("BEGIN LAYER").- How about SOLDERMASK_TOP/BOTTOM, PASTEMASK_TOP/BOTTOM? Does anything need to be defined there?I've had a hard time finding a good tutorial on thru-hold pad design. Any help/comments would be much appreciated.
You won't get an *exact* answer from me (on purpose since I charge for that).
What you need to look up is the standard drill sizes that a fabricator uses (mil/mm).
Plated holes -- the fabricator looks at the finished size, the plating and oversizes the drill to achieve your print requirement.
The oversized drill (typically finished + 4mils) then needs to be clearanced. Planes typically need more antipad than signals but I make mine the same.
A through-hole connection that ties to a plane for a mounted component is different than a via.
It's *nearly* impossible to solder a multi-layer board without having a flashed thermal spoke mount at the pin. The fabricator can usually guide on how to make these (Allegro has a flash symbol maker that you use).
Soldermask -- your choice here. You can choose to cover vias but you need to tell Allegro how big you want the mask (keepout) to be. Typically you need to be 3 mils or more from any plated hole edge.
Pastemask -- some parts are now paste-in-hole and they would need a mask definition. Most through-holes do not use a pastemask.
A lot of fabricators have their own rules for low-cost, standard, and advanced processing. Keep that in mind and be sure you review your fabricator's rules before sending them a Gerber file.
I can tell you my way of defining most of the pads.
if I had lead size of 24mils I add 6mils in defining drill size the I add 10mils annular ring so the actual pad having 30mils drill and 50 mils pad size. add 10 mils in antipad and thermal relief and then copy this stuff in all layer except solder mask. define solder mask 10 mil larger then pad size.
It is my practice I am also relatively new to allegro. so if any one knows the better way correct me.
Check this out. Its an excell spreadsheet with a bunch of common through hole sizes and recommended drill/land sizes from the IPC-7251 doc.
In reply to arcwilson:
that's awesome, thanks!