Teach me how to build a part from scratch in Pads 2007.4

[jon_eda]

My boss recently got a computer from an old partner that owed him some money. The computer came with Pads 2007.4. I have only worked with Orcad Capture and CAM350 (to view finished gerbers). We have been having our designs laid out and routed by someone else.

I have been messing around with it in my free time since we don't do a huge amount of design work all day. I have read through a few super basic tutorials for creating parts. I guess I don't understand exactly what box does what when dimensioning. My parts come out with weird shaped outlines and pads too long/skinny/fat etc. using the pin wizard.

I did drop a 7404 through hole on a layout page and was able to convert it to a SMT and edit a few properties outside the wizard. So basically what I am asking is if anyone could give me a quick overview on creating a part from scratch and help me interpret dimensions given in datasheets and how to enter the values properly.

The part I was having trouble creating was a STP16CP05 SMT. Once I learn how to build this part I should be able to make any others hopefully

Any help would be great as this software is very daunting to start out on. Even Pads Logic is nowhere near as smooth as Capture ( to a novice).

 

[edaedaeda]

New to Pads 2007.4

My first suggestion would be for you to go to pcbmatrix.com and download the specifications they have available. also they have a land pattern calculator tool that is very good. If your company cannot spring for the tool you can still get the demo version. This will help you understand how build a part from a datasheet. with the demo you will not be able to extract parts but it is still useful.

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

 

[jmatt]

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:

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.

 

[jon_eda]

Re: New to Pads 2007.4

How much does the PCBMatrix Land pattern calculator cost for the full version?

Added after 28 minutes:

@jmatt


Ok the wizard explanation makes a bit more sense now. So without using the wizard could you do a rundown of how to make the STP16CP05 SO-24? I would really appreciate it.

 

[edaedaeda]

New to Pads 2007.4

Jmatt has covered this subject pretty well. If you really need more assistance what I would suggest is to review existing library parts. I believe this is would be a very good way for you to learn how to create a part in pads.
There might even be an existing SO-XX part in library you inherited wehere you could modify it to fit your needs.

Eda

 

[jmatt]

Re: New to Pads 2007.4

What edaedaeda said. If you have the default libraries from PADS loaded, you should be able to find a SO_24 in there.

Now, I personally do not like the provided libraries, as there are no pads stacks, the silk outlines are on the wrong layer, and the pads are often too large.

For the part you specify, a standard 300-mil SO-24 will work. But just for you...

--> Because I think that way, all the dimensions are in mils (1 mil = 0.001").
I build with pad stacks, so I'm including that data.
--> FYI, in case you were wondering, PADS does a nice job jumping back and forth from English (mils) to Metric units with little or no conversion slop.
--> Another FYI - Go to Help-Modeless Commands... and print out the list. Until you get used to PADS, this is a VERY useful document. You probably won't use that many of the modeless commands, but the ones you do learn and use can speed up your work a bunch.

Assume part is created with a vertical orientation (Pin 1 @ upper left).

Part Origin: Center/Center. Everything is centered on the origin.

Pads:

Setup - Pad Stacks...

Top Pads (Mounted Side): Oval, 80 long X 20 wide (can be wider if you insist, though its not really necessary. If you do go wider, I wouldn't go past 24-26 mils wide).
Inner Pads (Inner Layers): Round, 0
Bottom Pads (Opposite Side): Round, 0
Drill Size: 0
Uncheck the "Plated" box.
Soldermask (Solder Mask Top): Oval, 86 long X 26 wide - aka 6mils over the Pad size (create your Gerbers with the soldermask oversize set to 0)
Solderpaste (Paste Mask Top): 1:1 to the Surface Pads. Let the assembler worry about any tweaks, seems like every shop is different.

Pad Spacing:

(All numbers are from pad center to pad center)
Pad Pitch: 50
Row Pitch: 370

Assembly image (used for the assembly drawing, and for 3D stuff):

Top Assembly layer: Closed rectangle 300 x 614; 4 mil thick line.
Circle inside body, at pin 1; 4 mil thick line.
60x6 designator, Center-Center, Orthogonal, centered on the origin.

Top Silk:

On Top layer. Top and bottom bar 6-8 mils thick X 300 wide. Place just outside the assembly image top and bottom extents.
Top bar can have a polarity "dimple" if you like. I normally don't (I do show one on the sample image).
60x6 designator, Center-Center, Orthogonal, centered at top of part.

Add the following attribute (Edit - Attribute Manager...): "Pin1", use an asterisk for the Value.
Set the Geometry.Height attribute to 104.

Add any other attributes you like, common ones are MFR, P/N, Decal and Description.

Back in the editor, add the Pin1 attribute (Add New Label, select "Pin1") on the Top layer and set it next to Pin 1 of the part.
Make the asterisk 80 x 8, Center-Center, Orthogonal.

Save as the name of your choice. Make sure it's going to the library you want it to.

Now, all that is based on how I make a Decal, which may or may not match exactly what you want to do.
A couple of things I always tell people when they're building libraries are:

1. Get a naming convention in place. It doesn't matter what it is, but you should figure out what you want and stick to it. BE CONSISTENT!
2. Build all your parts the same way. Get a standard methodology in place and stick to it. Don't make things up as you go along. There will be exceptions at times, but you can set up some general rules and stick to them it will make your job much easier. And make your board and documentation much nicer.
3. Use the PROPER standard reference designators and schematic symbols. Nothing says "amateur" like using the wrong designator or symbol for a part.

See ASME Y14.44-2008 for proper designators symbols, and their use. This is a reissue of the old IEEE 200-1975, also known as ANSI Y32.16-1975. Why the mechanical engineering group has taken over this standard is a mystery, but it is the relevant standard (though a copy of one of the old ones is just as good).

FYI, PADS has some naming and character limitations:

--> Illegal characters for PART and CAE (schematic symbol) names :

Ampersand ( & )
Asterisk ( * )
Braces ( { } )
Comma ( , )
Period ( . )
Question Mark ( ? )
Space

40 Character Limit.

NOTES:

1. Despite being listed, it does not appear that the period causes problems in Part names.
2. Despite not being listed, square brackets ( [ ] ) sometimes cause problems.

*****

--> Illegal characters for DECAL (footprint) names:

Asterisk ( * )
Colon ( : )
Comma ( , )
Question Mark ( ? )
Space

40 Character Limit.

NOTES:

1. Despite not being listed, square brackets ( [ ] ) sometimes cause problems.

*****

--> Illegal characters for SIGNAL Names:

Asterisk ( * )
Braces ( { } )
Comma ( , )
Question Mark ( ? )
Space

47 Character Limit.

NOTES:

1. Despite not being listed, square brackets ( [ ] ) sometimes cause problems.

*****

--> Illegal characters for Reference Designators:

Asterisk ( * )
Braces ( { } )
Comma ( , )
Period ( . )
Space
Tilde ( ~ )

15 Character Limit.

*****

--> Additional limitations:

Alphanumeric Pin Number: 7 Character Limit.
Layer Names: 40 Character Limit.
Attribute Name: 256 Character Limit, attributes may not contain spaces.

 

[jmatt]

Re: New to Pads 2007.4

I just came back and re-read this. I realized I designed the footprint to a minimal configuration. It might be better to lengthen the pads a bit, say to 85, with the soldermask 91 mils long.

And I would change the row-row spacing to 365.

This still gives you a minimal-impact foortprint with a good heel joint for the soldering (essentially the most important part of the solder joint).

If you're hand-soldering only, I would leave the row-row spacing at 370 and make the pad length 90 and the pad width to 24. Soldermask would be 6 mils over the pad size (96 x 30).