I did not know about the ability to included unconnected copper. Thanks,
that may prove quite useful. As far as the problem of shorts, I have come up
with my own solution to this. I place matching netlabels on either ends of
the microstrip symbol, so that I maintain a netlist connection. I do not
want these netlabels to appear on the schematic when printed so I change
their color to white and print in color to the monochrone laser printer. I
use a non-white background while working on the netlabels so that they are
visible to me, but change the background back to white before printing. This
has worked well for me, and removes DRC errors even when the pads used to
make the microstrip sections are overlapping each other. My only difficult
is with making the odd shapes with fills, etc., and eliminating the DRCs
created for the non-pad copper in the footprint. I think if I use the
"Update Free Primitives from Component Pads" command which Ian mentioned,
being careful not to create shorts that I do not intend, this will solve my
problems temporarily. I appreciate the help on this issue, and hope that
Protel will consider adding better utilities for handling microstrip design.
Perhaps someone will get ambitious and write a server which creates the
microstrip pattern from the information embedded into the schematic symbol.
Wouldn't that be slick !

Daniel

-----Original Message-----
From: JaMi Smith [mailto:[EMAIL PROTECTED]]
Sent: Tuesday, July 23, 2002 3:23 PM
To: Protel EDA Forum
Cc: JaMi Smith
Subject: Re: [PEDA] Microstrip footprints


Protel understands nothing of microstrip mitered corners or microstrip
components such as inductors.

There are two parts to the problem, one concerning "unconnected" copper, and
the other with "shorts".

The first, unconnected copper, is similar to a question raised here in this
forum a while back regarding "dual footprints" for a crystal, where a
"library component" needs to contain more "copper" than just a "pad" or
"hole", and in that particular instance, a "pad" and a "hole" connected
together with copper.

This is a problem in Protel, and the current Official "soultion" is to make
whatever copper "shapes" that you need in your "library component", and then
"check" the box that says "include copper" when you are doing an "update"
(syncronizing) from the Schematic to PCB.

You can also do a form of this in the "Netlist Manager" menu, where you can
also include the connected copper.

This will solve most Netlist problems and DRC errors (except the short, for
which see below), but the problem is that you have to remember to do this
every time you "update", and I hate to use the "Netlist Manager" functions
because they "scare" me, having on occasion had it short nets together and
lose others completely, forcing me to go back to do another "update".

The real problem is that you should be able to design copper areas within a
"library component" and have those copper areas remain permanently
"attached", electrically (or netlist) speaking, to whatever electical "pad"
of "land" it is connected to, but Protel simply isn't smart enough to do
that in it's current incarnation.

We can only hope it will show up in DXP Service Pack 3 or 4.

If I were to call this a "bug" here in this form,  I would instantly be
trashed with reasons why it should not be so.

So I will be content to state that it is simply a GLARING DESIGN OMISSION.

A secondary issue that you will find when you do this is the "short". This
has been discussed at length here in this forum, and there really is no
acceptable way aroud the "DRC" error problem here (although you can search
the archives for the "Lomax Short", which some claim to be at least a
partial solution to the problem).

Here again, the real problem is that you should be able to design copper
areas within a "library component" and have those copper areas remain
permanently "attached", even if it constitutes a short, but once again
Protel simply isn't smart enough to do that in it's current incarnation.

Again, calling this a "bug" here in this form would simply instantly invoke
responses.

So here I will be content to simply to state that it is a SUPER GIANT
ENORMOUSY GLARING DESIGN OMISSION OF UNPRECIDENTED MAGNITUDE AND
PROPORTIONS.

In answer to your current problem, I would simply design a "library
component" for both PCB and Schematic for your "miter", and simply add it to
your schematics and also your pcb's and "live" with the DRC error.

I think that you will find that this is what you will have to do with
virtually any "RF" parts such as these miters in transmission lines or
certain types of inductors that would constitute a short at "DC".

Respecting resistors, capacitors and transmission lines, you might find it
useful to note that a 20 mil wide pad on an 0402 surface mount R or C mates
perfectly with a 20 mil wide 50 ohm line derived with 12 mil of FR4 over a
ground plane (assuming you can tolerate FR4 in your design).

JaMi Smith
[EMAIL PROTECTED]

* * * * * * * * * *

----- Original Message -----
From: "Daniel Webster" <[EMAIL PROTECTED]>
To: "'Protel EDA Forum'" <[EMAIL PROTECTED]>
Sent: Tuesday, July 23, 2002 10:31 AM
Subject: Re: [PEDA] Microstrip footprints


>
> Has anyone developed footprints for microstrip sections ? I have been
trying
> to do this with pads set to certain length and widths. Mitered corners are
> particularly challenging to make as a library footprint. I have used two
> pads placed side by side at a 45 degree angle with the desired
measurements.
> If I add fills to this footprint to complete the desired pattern then I
will
> get DRC errors on my board once I load a netlist. It would be nice for
this
> situation to have various pad shapes available (user defined), triangular,
> trapazoidal, etc. If anyone has found a solution, or knows where I can
find
> microstrip footprints, please let me know.
>
> Thanks,
> Daniel
>
>
>
>
> ************************************************************************
> * Tracking #: 302C7AEC4E668747A3931191787D4A780F50FC92
> *
> ************************************************************************


* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Forum Guidelines Rules:
* http://www.techservinc.com/protelusers/forumrules.html
*
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to