Utility for package creation

I recently bought the new & improved PCB Footprint Expert (FPX) from PCB

Libraries. For $200 you get an excellent script generator that is

IPC-7351C-compliant in pads/lands/silkscreen/nomenclature, and other stuff.

It produces a .scr file you can then run in Eagle to synthesize the part in

your open Eagle library.

I don't work for PCB Libraries, but have provided debug feedback for the

helpful and courteous developers. I expect them to issue a patch or update

soon for the current 2012.23 release, so be sure to check with them to

ensure you get the latest. Make you sure you spec the EAGLE-output version,

and pay by Paypal/Credit Card if you don't want to wait a week for the

e-check to clear.

/AT

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

cosborne2000 wrote:

Does Eagle have a utility for the creation of typical packages?

 

I'm looking for something that you input pin pitch, row spacing,

total pin count, and other standard dimensions and have the program

generate a good starting point. I tried the createsymsmdpackage_rel2

ULP but it aborts with a syntax error (Eagle version 6.2).

There is an error in the CreateSymSMDPackage_rel2.ulp and associated file

that you can correct to make this ulp run.

The problem is a variable name in the ulp that equals the function name of a

new function that arrived with v6.

i.e. mic2u

In the following files find the instances (5) of mic2u and replace with

Mymic2u

globals.hul

functionMisc.cul

I didn't test beyond getting the first dialog to open but looks promising.

After you get a package created, measure it to be assurred it is the correct

size.

Good luck.

Warren

--

Viewed / responded via the newsgroup at

news.cadsoft.de

I wrote some simple C programs that prompt some questions about the desired package, and it will auto-generate an EAGLE script file.

It was only for personal use, but maybe you may wish to use them, or adapt for your purposes.

It is quick to use, and I use it all the time now, instead of manually creating packages.

It only does it for surface mount (because that was all I needed) but could give you ideas for through-hole too. If you do enhance it, please share the source and executable (and maybe even the generated script files) with others : )

It works for all dual-in-line style SMD packages (SOP, SSOP, etc), quad packages (QFP, etc) and also single-in-line style packages (e.g. flex cable connectors). For example, if you run it as shown here (it provides "hints" to help answer the questions it asks), and respond to it at the '>' prompts:

** SMD Tool ***
All dimensions in mm
Pad width
---------
TQFP:0.29 TSSOP:0.40
>0.5
Pad height
----------
TQFP:1.35 TSSOP:1.30
>1.2
Style (number of sides)
-----------------------
TQFP-like:4 TSOP-like:2 SIL-like:1
>2
Distance to opposite side pad centers (Ax or Ay)
------------------------------------------------
TQFP48:8.45 TSSOP:6.10
>3.1
Pin spacing/pitch (e)
---------------------
TQFP:0.5 TSSOP:0.65
>0.95
Number of pins
--------------
TQFP48:48 TSSOP16:16
>6
Overall package width
---------------------
TSSOP16:5.0
>2.9
Filename
--------
example: my_tssop.scr
>my_tsop6.scr

Then, the generated script file will contain:

grid mm
grid 1
set wire_bend 2
layer tPlace 
wire 0.127000 (-1.450000 -0.569000) (1.450000 -0.569000)
wire 0.127000 (1.450000 -0.569000) (1.450000 0.569000)
wire 0.127000 (1.450000 0.569000) (-1.450000 0.569000)
wire 0.127000 (-1.450000 0.569000) (-1.450000 -0.569000)
circle 0 (-0.950000 -0.069000) (-0.650000 -0.069000)
set size 1.27
layer tnames
text >NAME (-1.450000 -4.420000)
layer tvalues
text >VALUE (-1.450000 3.150000)
layer top
smd 0.500000 1.200000 '1' (-0.950000 -1.550000)
smd 0.500000 1.200000 '2' (0.000000 -1.550000)
smd 0.500000 1.200000 '3' (0.950000 -1.550000)
smd 0.500000 1.200000 '4' (0.950000 1.550000)
smd 0.500000 1.200000 '5' (0.000000 1.550000)
smd 0.500000 1.200000 '6' (-0.950000 1.550000)

And when you run that in EAGLE (create a Package as normal, then select File->Script), it will generate the package:

Here are some other examples that are possible:

The windows executable and source code is available here (the source is in the pdf). There is also code to create outlines for toroid transformers.

On 10/06/2012 07:09 PM, shabaz wrote:

I wrote some simple C programs that prompt some questions about the desired package, and it will auto-generate an EAGLE script file.

It was only for personal use, but maybe you may wish to use them, or adapt for your purposes.

It is quick to use, and I use it all the time now, instead of manually creating packages.

 

>

The windows executable and source code is available here (http://badcafe.co.uk/category/eagle/) (the source is in the pdf). There is also code to create outlines for toroid transformers.

 

Nice web page resource, thanks!

bill m.

I can see that buying another program to create packages is one answer, other programs of half the cost include great package creation as standard. Again I state that Eagle should include within the package editor a menu item to create pads by X and Y size entry, pad count in either rows or colums, and pitch of pads. I use a much less expensive program just for the reason of it's package creation abilities whenever possible. I know Eagle is much more capable in most other areas, but package creation is not one of them, but should be.Why should we have to call up a scrip, buy another program, constantly need to change grid sizes or any number of other items just to build a package?

I understand this post is better in the suggestion area, but when I see people having such problems with package creation, I can't help but throw in my two cents worth.

Thanks,

Bob Moreno

I was a PADS user for a number of years, and almost nothing could be clunkier in the building of schematic and PCB entities. Despite this PADS remains a great favorite in the OrCAD-PADS mixed environment.

With the worst of the EAGLE script-generation bugs worked out of the FPX 2012.24 release, it's a time-saver now to generate best-practice PCB lands, and good and consistent silk and assembly art.

NB the requirements of the IPC-7351C standard are actually pretty useful, one of them being that silk screened under the placed package is useless, so why draw it in the first place? Also pin 1 ID is needed for engineers and techs to get oriented for instrumentation, and for inspectors to quickly verify correct placement rotation. I might point out that the C-generated script SMD footprint images posted earlier fail on both these counts.

Hi Alex,

For those that are hand-soldering, a footprint that draws the outline of the package (call it "under the package" if you will) is actually quite important for the simple reason that it acts as an aid to be able to visually center the package to the footprint. The C program asks for the width of the package to achieve this.

I understand that pick-and place machines do not require an outline.

If one desires the outline around the package, I don't think it takes a genius to modify the C code, since I provided the source. In fact you may not need to do anything for the quad style packages, because you could type a width greater than the package size.

You've missed the main point of the code, which is to generate all the pads in the correct position. Moving the round spot which marks pin 1 is

a trivial affair that I can achieve with my mouse and a single click-and-drag operation. Or modify the source code. It is code written in an

afternoon; hardly difficult, but they save a lot of time.

And getting practice with the EAGLE scripts is no bad thing, because you can generate complex shapes if needed - I like my toroids to exactly fit PCBs.

Maybe third party products do that, but I don't know.

Or one could spend $200 on a package, but for now, I'm very happy with the time I'm saving (and I've created hundreds of boards).

But yes, I totally agree with the poster earlier that we should not need ancillary software to achieve this purpose. It is functionality that should

be in EAGLE. I posted such a recommendation here.

Thanks for the info here and the link to the blog. Very useful information. Nice work.