On 11:21 AM 9/03/2001 -0800, Phillip Welsh said:
>I am a new user with Protel.  I finally found out how to make my own
>footprints with the wizard.  But I have a three-conductor 3.5mm Phone jack
>for headphones I can't find the footprint for.  There is a figure for it in
>the schematic libraries called PhoneJack Stereo SW but nothing else.  If
>anyone could help me it would be appreciated.
>
>Thanks,
>
>Phillip Welsh
>UCF student

This is quite a long reply, those with experience at designing footprints 
can safely ignore:

You will most likely have to create your own footprint from scratch.  This 
is not too hard.  Most of the time all you need to do is place pads 
matching the pins on the device (allowing about 0.2 mm or a bit more 
oversize for leaded pins). You should also add lines on the top overlay 
layer to show the boundary of the device. That is the basics you can get 
more advanced with experience.

Have a look at some existing footprints in a library to see how they are 
made. The wizard will not help you with this sort of component and so you 
will need to make one from scratch.  Looking at existing components will 
show that it is not rocket science.

Before you start mucking about with PCB libraries make a copy of a suitable 
one that you already have - one of your own or an existing Protel 
one.  Open this copy and inspect a few components. See how they have been 
made and what elements they are made from (usually pads and top overlay 
tracks).

Part of they key to making good components is placing the pads 
accurately.  I usually set my grid to an appropriate setting for the type 
of component I am laying up.  If it is a simple dip, for instance, then a 
20 mil grid is fine.

A more complex mechanical device may have all sorts of off-grid pads.  I 
will usually set a moderate grid, place one of the pads on 0,0 and then 
approximately place the others.  Then I go back and, by double clicking 
each pad, edit the exact x and y locations to be correct.  Make liberal use 
of the Reports|Measure Distance function. Print a 1:1 check plot on the 
centre of a page (if possible) with a reasonable printer. (Why the 
centre?  tends to reduce a little some distortions that can occur with 
older laser printers.)

You will of course need an accurate data sheet for the part you wish to fit 
- and it is well worthwhile having a sample of the device to allow you to 
check dimensions.  A surprising number of mechanical drawings on data 
sheets have errors.

Step by step:
1) Find a suitable part from your preferred supplier.  Try to get some 
ASAP.  Get the manufacturers data sheet.
2) Open for editing the PCB library where you wish the new component to reside.
3) Create a new component - you can use the wizard to create a dummy 
component that you edit or you can simply create a new blank component.  If 
you do the latter you will need to find the newly created component in the 
browse list and rename it - the new component has a name PCBCOMPONENT_x 
where x is a number. You may have to search up and down the browse list if 
you can't see it immediately (is this bug fixed in SP6?)
4) Get the data sheet out and place and position pads accurately in 
position.  Since I assume this is a through hole part, place pads on the 
multilayer layer and give them a hole size about 0.2 to 0.5mm oversize - 
depending upon how accurate and how large the pins are on the device (rule 
of thumb - exceptions abound).  Take care to account for the real diameter 
required for square and rectangular pads.
5) Make sure the pad designators match the pin numbers (not names) in the 
sch symbol.
6) Add top layer overlay lines to show the boundary of the device - take 
care to break any lines that get near the pads.  I like to keep my overlay 
at least 10 mils away from any pads (rule to be broken here as well at times)
7) Did you remember to rename it?  This name must be put into the footprint 
field of the sch symbol.
8) Save the library.
9) Print the component as a 1:1 and check that it looks right and that the 
device will actually fit.  Recheck all dimensions especially hole 
sizes.  Check that pads are all set as plated (in the pad advanced 
properties) (again another rule to be broken at times) - Protel has a 
strange habit of remembering the attributes you don't want remembered (such 
as unchecking the plated attribute) and not remembering those you do want - 
so check those pads carefully.
10) Save the library - again!
11) Check it again - until you are experienced at this you have to recheck 
a lot.

(Slots - this is an aside.  Many DC connectors and 3.5mm stereo connectors 
have wide rectangular pins.  these can either be accommodated by grossly 
oversized holes (in which case they slop about during placement and make it 
hard to align to housings etc) or you can specify a plated slot.  There are 
a number of tricks with such slots that I won't go into but it is possible 
to make footprints with a reasonable sized router bit (good feed rate and 
fewer breakages) and still have the component fit snuggly - hint think 
offset the slots from the pins.)

You should be about right now.  Make sure this library is in the list of 
libraries available to the PCB you are designing and away you go.

Hope this helps,
Ian

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To join or leave this list visit:
* http://www.techservinc.com/protelusers/subscrib.html
*                      - or email -
* mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to