Re: New to Pads 2007.4
I'm a long-time user of PADS, so to me, it's a pretty simple package to use.Their Help is decent, though sometimes you have to think like a programmer to figure out where some of the help items that relate to what you need to do are...
Personally, I rarely if ever use the wizard to create parts, but it is a handy tool.
A couple of things.
1. All footprints (called Decals) are built from the top (aka as if you have it in your hand right side up). PADS knows to push things to the appropriate associated Bottom layers when you move parts to the Bottom side in the Layout editor.
2. Silkscreen image, reference designator, and Attributes should all be placed on the Top layer. Not <All Layers> (IMHO, nothing should go on that layer).
3. Any silkscreen text other than the reference designator should go on the Top Silkscreen layer. FYI, in PADS, the Silscreen layers are mostly used for things like logos, board ID stuff, and any non-attribute text, not for actual Decal silk images or designators. You
CAN put the outline and stuff there, but there are some minor problems if you do.
4. You should also create an image on the Top Assembly layer. My practice is to make it 1:1 to the part, showing as much detail as is necessary. I use this image for my assembly drawings. Add a second designator to this layer.
5. Build your Decals with complete pad stacks (pad, soldermask and solderpaste for SMT parts, pads and soldermask pads for THT parts).
6. PADS' default anti-pads tend to be larger than they need to be, so you would want to edit those on THT parts.
7. The "Plated" box in the pad definition (not done in the wizard, but after you go to the newly-crated Decal) should be unchecked for SMT parts.
The Decal Wizard..
Looks like this (I chose the SOIC tab, but they all basically work the same way):
Starting from the upper left -
-
Decal -
-- Vertical and Horizontal are the orientation you want the part to be (see sample image in window on right side). That's your preference per your standards and procedures.
-- Pin Count - How many pins you need. This MUST be an even number for the SOIC. Other types have some different rules. You would have to manually add an extra pad for parts with slugs under them. You can use the SOIC section to create 2-pin devices if you want.
-- Origin SMT parts should have their origin in the center, THT parts traditionally have their origin on pin 1.
-
Silkscreen creates the silk image. What the wizard creates is more appropriate for the Top Assembly layer, so I would set the image to that layer and add a silk image later. Use the defaults, because the way they set up how it places the image was silly. Any Decal you create in the wizard WILL require some cleanup after you're done anyway.
-
Pins PADS has a bizarre method of creating pads (they call them pins...). It is Length x Width x Rotation instead of X by Y. The Length MUST always be longer than the Width. You do have a choice of Oval (which is really oblong) and rectangle for SOIC parts. In the regular editor, you have a few other pads type choices.
-
Width - How wide should the pad be? In the example, it is 24 mils.
-
Length - How long should the pad be? In the example, it is 74 mils.
- The rotation is covered by the rotation you chose in the Decal section.
-
Pin Shape - I prefer Oval pads for my SO type parts, but that's up to you and your standards (and the assembler you use).
-
Pin Pitch - Is the pad-to-pad spacing.
-
Row Pitch - Is the side-to-side spacing of the pads.
- You then have some choices on how the pins are spaced. Personally, I always use "Center to Center"
-
Units - Obviously, the unit type you are creating the Decals in. This would probably be the firat thing you would set in the wizard.
Basically, you crate your basic Decal, then finish. A Decal will be created. Add the Silk data. then go into Setup - Pad Stacks to clean some of that stuff up.
You can also add attributes that act like the designator (the Reference Designator is actually an attribute), add the silk image, etc.
If you'd like, I can send you a sample Decal.
Added after 2 minutes:
edaedaeda said:
One more thing. Orcad Capture can output a pads netlist no problem. PCB Matrix has a netlist tool that will generate a pads netlist from Orcad. on the flip side Mentor Graphics has a free tool that will convert an Orcad schematic to Logic. It is pretty easy to use.
Eda
Actually, PADS Logic, even the demo version will open an OrCAD schematic (.dsn file) directly, just use File-Open, and select the OrCAD .dsn as the input type.