PCB123 Part Creation Tutorial.
Assumptions:
1. You have the most current version of the software.
What you will learn:
1. How to find PCB footprint specifications
2. How to modify the grid
3. How to renumber pads
4. How to create silkscreen
5. How to insert library parts
In the current BETA, we have made it fairly easy to create your own custom parts.
However, it is a good idea to start off with a good understand of the utility’s
strengths and weaknesses. This tutorial will focus on PCB Layout, but the basics
can be used in either application.
To be successful with any type of part creation, be it Schematic or Layout,
you need to start off with good specifications. Listed below are some generic
guidelines:
1. Know the units that the part was designed in, Mils or Millimeters (standard
or metric)
2. Pad to pad spacing both X and Y
3. Drill hole size
You can always create a part if you are holding the physical package in your
hands. You can make the required measurements with calipers.
We will start off with downloading the PCB Foot print specifications from the
manufacturer. I use www.Google.com as a rule to find what I am looking for.
Basically I type the part number or package description in and usually a few
dozen choices come up to choose from. After poking around a bit, I find what
I need. If you know the 3 items above, you are almost guaranteed a good part
when you are done.
I prefer the *.PDF (Adobe Acrobat document), as these documents are easy to
print and be saved for later use. I highly recommend printing the part because
it is VERY difficult to continue to alt-tab between the web page and PCB123.
To repeat, PRINT the specifications out.
Once Layout is open from the toolbar select “Libraries” then “Part
Editor”. You will notice a small square on the screen next to the text
“Draw part symbol here”. This small square represents the insertion
point (i.e. where the part will be inserted) when you place it in to your design.
You will always start your design here.
We will be creating a standard dip 16 PCB socket, so type in to www.Google.com
dip 16 PCB socket. Look what we get…. See how easy it is.
For this example I have included the required information below.
We know the following from looking at the pictures: (see below)
1. The part is on a .100 grid spacing (mils)
2. The pins are spaced .100 apart and .300 across
3. The package is .800 long and .400 wide.
In the part editor, we want to be sure we are working with the correct grid.
From the part editor toolbar, select “Settings” then “Grid”
then pick from the list “0.100”
So why are we doing this? Setting the grid to the most common spacing allows
you to make easy calculations and the placement of pads goes quickly.
Now that the spacing is set to 0.100, we can place our first pad. From the
part editor toolbar select “edit” then “insert object”,
then “pad”. You can also press the “C” key or the red
donut from the toolbar, and then simply place the first pad on the square.
This will be pin one.
You have now placed your first pad of your new part. You should notice that
your screen is broken into 0.100 grid points. Now place the next 7 pads in this
row from left to right on top of these points. Now from the part editor tool
bar, click on the “draw to fit” icon (light blue magnifying glass
with a square in it).
You should be able to see things much clearer now. Pads are numbered from 1
to 8.
Now right click anywhere on the screen. This will get you out of place mode
and in to the default select mode. Also known as Select/Edit mode. You will see that your mouse cross hair has changed to an arrow pointer. ... Select pad # 4, it will be selected when a dotted box is around it. Now delete it.
Go back to the toolbar and select the green donut again (pad object), place
a pad in the empty space where pad 4 was. Notice that it now says 9. This is
done automatically to prevent pin duplication. But now you are saying “I
don’t want my pads miss-numbered” so let’s fix it. Select
pad 9 and right click on it. A small dialog will come up. On the bottom is the
text “pin number”. Enter 4 in here and hit “OK”
Now that things are back to normal, lets place the next row of pins. If you
remember, we set the grid to 0.100. From our picture we know the next row is
0.300 from the first. So place the next pad 3 grid points below pad 1. Continue
placing pads until you get to pin 16.
Now we need to change the pad drill size to mach our part. The default drill
size on new pads is .02 but we want our part’s holes to be at 0.025. First,
make sure you are in select mode by right clicking on the screen. Now left click
and drag a box around all of the pins.
From the toolbar select “settings” then “pads”. This
will bring up a dialog box allowing you to globally change all of your selected
pads at once. Under the text “Hole” select 0.025 and click “OK”
You will notice that the drill holes are now larger.
Great!! We are almost done. Let’s create the silk screen. Go up to the
toolbar and select “Settings” then “Grid” then pick
from the list “0.050” This will allow us to draw a rectangle .050
from the pads. From the toolbar, select the rectangle drawing object. Now left
click and drag a rectangle around your part. Pay close attention that you are
just one grid point away from the pads.
You can be as creative or as minimalist as you choose when designing your silkscreen.
Now let’s add a description. In the left hand side there is a large text
box for you to type in your new part description. Put in “My first part”
It’s time to save your part. From the toolbar select “File: then
“Save”. A dialog labeled “save Package library part” will come
up with 2 columns of information. The first one is the library you will be saving
it to and the other is the part name.
In the first column type “mylib” and in the second type “firstpart”.
Select “Save Part”; it will ask you if you want to start a new library
called “mylib”; click “YES”
You are now returned to the part editor and to close, simply click the small
X in the corner or from the toolbar click “file” then “close”
to exit.
Now that you are back in layout let’s try out your newly created part.
From the toolbar, select “edit” then “insert object”,
“library part” or you can also use the F5 key. From the dialog that
comes up type in the Library column mylib then select it from the list. Once
selected it will refresh the right hand column. Select “firstpart”
then click “Load Part” The dialog will close and you can left click
with your mouse to insert your part as many times as you wish. Once you right
click anywhere on your screen you part (Or any part) will be unloaded from you
cursor. (End)
This tutorial was created by Todd Clifton AkA MrWizard
If you have questions, comments, or suggestions please let us know at support@pcb123.com
Discussions
Support
Downloads & links
Member Info
Membership:
Latest: 
New Today: 45
New Yesterday: 69
Overall: 44593
People Online:
Visitors: 26
Members: 0
Total: 26
Who Is Where: