Going
from SCH to PCB
So now I have a schematic. How do I make a PCB layout?
1. Make your schematic in SCH. For help on how to do this, see the schematic
tutorial.
2. In the old versions of Protel, you had to go through an intermediate
step known as a netlist. All of that is hidden now, though people who want
can still use them.
3. In SCH, Go to Design -> Update PCB... You may be asked to
associate a PCB file with this schematic. Eventually, the Update
Design window will appear. Click Execute. If it warns you about
that it cannot execute all of the netlist, click no and look at the warnings
to determine the cause. Common warnings are:
-
Footprint
not found in library. A footprint is a code which specifies the
physical size and shape of the component, which is needed to make a layout.
Possible cause 1: the component specified does not have a footprint
in the shematic. To check this, go back to SCH and double-click the component.
In the popup window, see if there is anything in the "footprint" label.
If it is empty, you will need to manually assign a footprint. Zoe has made
a helpful table
of footprints to help you decide what to assign. Tip: You may want
to assign the footprints globally, if you have a lot of similar identical
components, rather than assigning a footprint to each component individually.
To do this, double-click on the component to bring up its properties.
Click on the "global" button. In the new window that pops up,
copy the Lib Ref into the Lib Ref under "Attributes to match by".
Then under "Copy attributes", copy in the footprint. Click here
to see an example of this in action.
Possible cause 2: The footprint specified is not in one of the
libraries loaded on PCB. Check what the footprint is specified in SCH,
and then look in the components list of each library you have loaded in
PCB to see if it is there. If not, choose another footprint or try to find
a library containing the one you want. Click here
for instructions on installing libraries.
-
Component not found. In my case, this problem was caused by improper
naming of the components in SCH. When you place a component in SCH,
it adds a label (e.g. "CAP"). You can then add a Lib Ref (e.g. "C3"), which
will appear above it in the schematic and be used by the netlist maker
to identify parts. Make sure there are no spaces in the designation.
For example, if you designate something as "R1 10K", it will think there
are two component: R1 and R1 10K, and basically get confused. If
you want to put more details about something on the schematic, you can
put it in the "Part Type" section of the properties. Click here to
see an example of the errors generated.
-
Node not found. This means something is wrong with the connection
on the component named. Causes: 1) using lines instead of wires for connections.
2) the wire overlaps the component. One indication of this is a red junction
circle right next to the component. To check, go into SCH, zoom way
in on the offending connection, and click on the wire. You will be able
to see if it extends past the end of the component. Click here
to see an example. If so, you can either delete it and redraw, or click
quickly on the end of the line until the cursor turns into a thin cross,
and drag the end to its new place.
4. Once you get the above to work without warnings, switch over to the
PCB. You will find all your parts in a big heap in the middle of the PCB
file. Zoom way in and drag them all until nothing is on top of anything
anymore. Now you want to look at each part carefully.
There may still be errors in the netlist. Check that all the pins
on each part that should be connected to something have a green line connecting
them to the right place. For example, if you have a resistor with
only one side connected, something may be wrong. To fix problems
like this, click on the suspicious component to find outs its name.
Then go back into the schematic, look carefully at the component, and try
to fix the problem. After you fix the problem, just repeat step 3
again.
