Re: [PEDA] Microstrip footprints

2002-07-24 Thread Tony Karavidas

Jami, you need to learn the definition of a bug I guess. Bitch all you want
about Protel, I don't care. Just be accurate. You're a professional, not
some high school hack. You should be able to refer to a problem as either a
bug or a poor implementation, a lack of implementation, or something you
just don't like. There is a difference between all four.


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.

YES!!!


Tony






 -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

Re: [PEDA] Microstrip footprints

2002-07-24 Thread Brad Velander

Daniel, Ian,
there is a further possible design corruption problem when using the
Assign Net to Connected Copper function during an update. If you have
updated a footprint to a new footprint at the same time that you are
updating with the connected copper checked. You can really screw up your
database if the new footprint touches some copper that the old part did not,
or the new part is in a different rotation and touches some copper
(typically GND) that it shouldn't have. The part may be updated, make the
illegal connection, then the update copper from connected pads updates the
illegally connected copper to the wrong net (usually changing it from GND in
my designs). I prefer to run the update, check all existing components in
the existing layout (typically only those already placed and routed) to see
that they don't make a short to something they shouldn't, then I will run
the Netlist Manager, Update Free Primitives From Component Pads function.

Sincerely,
Brad Velander.

Lead PCB Designer
Norsat International Inc.
Microwave Products
Tel   (604) 292-9089 (direct line)
Fax  (604) 292-9010
email: [EMAIL PROTECTED]
http://www.norsat.com


-Original Message-
From: Ian Wilson [mailto:[EMAIL PROTECTED]]
Sent: Tuesday, July 23, 2002 4:06 PM
To: Protel EDA Forum
Subject: Re: [PEDA] Microstrip footprints


SNIP

When you synchronise from a Sch to the PCB using Tools/Update PCB you can 
check the Assign Net to Connected Copper check box but I found this made 
the synch slower than otherwise and by more than the time taken to manually 
run the Update Free Primitives from Component Pads process - I did not do a 
careful check though.

Ian Wilson



* Tracking #: 1AAC93682FBEEE4D8614CDD9E9026534892FEC04
*


* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *



Re: [PEDA] Microstrip footprints

2002-07-24 Thread Daniel Webster


 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

Re: [PEDA] Microstrip footprints

2002-07-23 Thread Daniel Webster


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
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *



Re: [PEDA] Microstrip footprints

2002-07-23 Thread JaMi Smith

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
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *



Re: [PEDA] Microstrip footprints

2002-07-23 Thread Ian Wilson

On 10:31 AM 23/07/2002 -0700, Daniel Webster said:

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

Protel does not support complex pads as such.  You can achieve what you 
want with combinations of pads and fills as you are doing.  To remove the 
DRC errors you can use the Update Free Primitives from Component Pads 
command.  This command says free primitives but it will actually update 
fills and tracks that are part of a footprint.

This command is somewhat hidden:
Design/Netlist Manager... Click on the Menu button and select Update Free 
Primitives from Component Pads.

When you synchronise from a Sch to the PCB using Tools/Update PCB you can 
check the Assign Net to Connected Copper check box but I found this made 
the synch slower than otherwise and by more than the time taken to manually 
run the Update Free Primitives from Component Pads process - I did not do a 
careful check though.

Ian Wilson



* Tracking #: E15F96AD78499A488F1F631A9C6D0D87C69599AD
*


* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *