Re: [PEDA] URGENT HELP REQUIRED: Paste Mask

2002-02-19 Thread Jason Morgan

Yes and No.

Yes I designed the board and No the Vias are not free pads.

There is no holes in the solder paste layers on the origional protel
drawing, only on the gerber import.

The gerber import is just photoplot commands, therefore if there is a shape
there then there will be a hole.

J.


-Original Message-
From: Brad Velander [mailto:[EMAIL PROTECTED]]
Sent: 18 February 2002 19:31
To: 'Protel EDA Forum'
Subject: Re: [PEDA] URGENT HELP REQUIRED: Paste Mask


Jason,
did you actually design this board? Because I have a feeling that
what you're describing means that your vias are actually free pads. Is that
a possibility? Normally vias don't show on a solderpaste layer. Other
possiblity is that you have loaded a padmaster back in as a pastemask.

I have assumed that in your original message you were trying to say
...tented vias have solder paste on them from the paste mask layer.

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

See us at Booth 323 at Satellite 2002 in Washington, DC March 6-8.



-Original Message-
From: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED]]
Sent: Monday, February 18, 2002 10:58 AM
To: Protel EDA Forum
Subject: Re: [PEDA] URGENT HELP REQUIRED: Paste Mask


In a message dated 2/18/2002 1:42:56 PM Eastern Standard Time, 
[EMAIL PROTECTED] writes:


 As normal we load the gerbers back into protel to check they look right,
 I've noticed that
 the tented vias have solder on them on the paste mask.  Why, and how do I
 get rid of it?
 
 I've never noticed this before but can't say it hasn't happened.
 
 We're just about to spin the boards and want to know if this will affect 
 the
 mask manufacture.
 

If so, I'd consider that a bug in Protel. But you may have been covered (so 
to speak) by the board house in the past. The board houses I've dealt with 
routinely mask the silkscreen with the soldermask layer, so you don't get
ink 
on the exposed pads. The assembly house may well do the same thing between 
the soldermask and the paste mask, to avoid getting past on top of the 
soldermask. If so, that would explain why you haven't seen a problem in the 
past.

Steve Hendrix

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] URGENT HELP REQUIRED: Paste Mask

2002-02-19 Thread Jason Morgan

Entirely probable..

We sent the gerbers anyway. And then tried a different gerber viewer this
morning.

PANIC OVER, call off the dogs.

Leon was right. Protels' importer saw the vias as through
hole pads, so placed a free pad at its location on multi layer.

The free pads have a paste mask so protel created one in addition to
the paste mask that was in the gerber.

Not sure if that is actually a bug, probably not, but something to be
aware of.


Many thanks,
Jason

-Original Message-
From: ICT Mail [mailto:[EMAIL PROTECTED]]
Sent: 18 February 2002 23:43
To: Protel EDA Forum
Subject: Re: [PEDA] URGENT HELP REQUIRED: Paste Mask


Jason, just a thought here
When you load gerbers back into a blank PCB file, you must remember that for
a given layer, all the lands that represent vias and pads etc will be
imported as free pads and will take on the design rules specified in your
PCB file. Vias are just a D-code for a given artwork layer.

I suspect that if you tented these vias when looking at them in Protel after
importing the gerbers, they would actually have a Solder Mask assigned which
would be the default for a free pad or general rule in the viewing PCB
file.

I would recommend using a Gerber viewer / editor for viewing Gerber files.

Leon Fonstin


-Original Message-
From: Jason Morgan [mailto:[EMAIL PROTECTED]]
Sent: Tuesday, 19 February 2002 5:36 AM
To: Protel EDA Forum (E-mail)
Subject: [PEDA] URGENT HELP REQUIRED: Paste Mask
Importance: High


Hi,

As normal we load the gerbers back into protel to check they look right,
I've noticed that
the tented vias have solder on them on the paste mask.  Why, and how do I
get rid of it?

I've never noticed this before but can't say it hasn't happened.

We're just about to spin the boards and want to know if this will affect the
mask manufacture.

Many thanks,

Jason.

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] URGENT HELP REQUIRED: Paste Mask

2002-02-19 Thread Brad Velander

Jason,
if you haven't caught on to your problem yet, I think that one of
the other posters hit the nail on the head. There may be nothing wrong with
your original Gerber files, the problem may have arose when you imported
them back into Protel.
Importing Gerber back into Protel is something that I do not do, I
want independent confirmation that the Gerbers are correctly generated. So
if I don't do this explanation justice, bear with me and try to understand
the concept I am pointing out.
I believe that when you import Gerbers back into Protel then most of
the imported pads are treated as free-pads upon importation. This new
free-pad is not a via any longer (if it was a via pad to start with), now it
is interpreted as a free pad and as such it will show a solderpaste mask
opening in the database which you have imported it into. Remember that your
imported Gerber is now a new Protel primitive and thus it may behave like
any other primitive and may not truly represent the former Gerber element
that you thought you imported.

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

See us at Booth 323 at Satellite 2002 in Washington, DC March 6-8.



-Original Message-
From: Jason Morgan [mailto:[EMAIL PROTECTED]]
Sent: Tuesday, February 19, 2002 1:08 AM
To: 'Protel EDA Forum'
Subject: Re: [PEDA] URGENT HELP REQUIRED: Paste Mask


Yes and No.

Yes I designed the board and No the Vias are not free pads.

There is no holes in the solder paste layers on the origional protel
drawing, only on the gerber import.

The gerber import is just photoplot commands, therefore if there is a shape
there then there will be a hole.

J.

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] URGENT HELP REQUIRED: Paste Mask

2002-02-19 Thread Bob Wolfe

Jason,
I did not follow this one from the very beginning but,
I would also 100% agree that bringing a gerber file back into your
CAD system for any reason other than to use it to reproduce
a board you have no CAD data for, or copy sections into an
existing board etc. is not good. I would NOT recommend it as a means of
verifying gerber data for fabrication. Way back Cadnetix offered
gerber import as the only means of checking gerbers too, but this was really
not an accurate way to do this you really need to view them in another
piece of sofware, which we did. Cadnetix also offered a smart gerber input
for just the purpose of bringing a gerber only design into the CAD system.
In all the cases I have seen like here with Protel bringing the gerber file
into the CAD system usually relies on settings or pad data inherent from the
CAD system. In the case of Cadnetix you were merely importing the pads
from your own library to view up the gerber, an dbeliev me that is not
checking any gerber data, it merely means you had a pad in the library
with the proper name. In this case it seems its a problem with the way the
CAD system handles vias. In any case use a separate viewer or CAM software
to do this function.
Bob
Robert M. Wolfe, C.I.D.
[EMAIL PROTECTED]


* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] URGENT HELP REQUIRED: Paste Mask

2002-02-18 Thread HxEngr




Re: [PEDA] URGENT HELP REQUIRED: Paste Mask

2002-02-18 Thread Brad Velander

Jason,
did you actually design this board? Because I have a feeling that
what you're describing means that your vias are actually free pads. Is that
a possibility? Normally vias don't show on a solderpaste layer. Other
possiblity is that you have loaded a padmaster back in as a pastemask.

I have assumed that in your original message you were trying to say
...tented vias have solder paste on them from the paste mask layer.

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

See us at Booth 323 at Satellite 2002 in Washington, DC March 6-8.



-Original Message-
From: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED]]
Sent: Monday, February 18, 2002 10:58 AM
To: Protel EDA Forum
Subject: Re: [PEDA] URGENT HELP REQUIRED: Paste Mask


In a message dated 2/18/2002 1:42:56 PM Eastern Standard Time, 
[EMAIL PROTECTED] writes:


 As normal we load the gerbers back into protel to check they look right,
 I've noticed that
 the tented vias have solder on them on the paste mask.  Why, and how do I
 get rid of it?
 
 I've never noticed this before but can't say it hasn't happened.
 
 We're just about to spin the boards and want to know if this will affect 
 the
 mask manufacture.
 

If so, I'd consider that a bug in Protel. But you may have been covered (so 
to speak) by the board house in the past. The board houses I've dealt with 
routinely mask the silkscreen with the soldermask layer, so you don't get
ink 
on the exposed pads. The assembly house may well do the same thing between 
the soldermask and the paste mask, to avoid getting past on top of the 
soldermask. If so, that would explain why you haven't seen a problem in the 
past.

Steve Hendrix

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] URGENT HELP REQUIRED: Paste Mask

2002-02-18 Thread Abd ul-Rahman Lomax

At 06:36 PM 2/18/2002 +, you wrote:
As normal we load the gerbers back into protel to check they look right,
I've noticed that
the tented vias have solder on them on the paste mask.  Why, and how do I
get rid of it?

(1) are you sure that they are vias and not free pads?
(2) what are the paste mask rule settings?

We're just about to spin the boards and want to know if this will affect the
mask manufacture.

Paste mask is typically the last operation which might or might not give 
you a little extra time. It might even be applied by the assembler as 
distinct from the board fabricator

[EMAIL PROTECTED]
Abdulrahman Lomax
Easthampton, Massachusetts USA

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] URGENT HELP REQUIRED: Paste Mask

2002-02-18 Thread ICT Mail

Jason, just a thought here
When you load gerbers back into a blank PCB file, you must remember that for
a given layer, all the lands that represent vias and pads etc will be
imported as free pads and will take on the design rules specified in your
PCB file. Vias are just a D-code for a given artwork layer.

I suspect that if you tented these vias when looking at them in Protel after
importing the gerbers, they would actually have a Solder Mask assigned which
would be the default for a free pad or general rule in the viewing PCB
file.

I would recommend using a Gerber viewer / editor for viewing Gerber files.

Leon Fonstin


-Original Message-
From: Jason Morgan [mailto:[EMAIL PROTECTED]]
Sent: Tuesday, 19 February 2002 5:36 AM
To: Protel EDA Forum (E-mail)
Subject: [PEDA] URGENT HELP REQUIRED: Paste Mask
Importance: High


Hi,

As normal we load the gerbers back into protel to check they look right,
I've noticed that
the tented vias have solder on them on the paste mask.  Why, and how do I
get rid of it?

I've never noticed this before but can't say it hasn't happened.

We're just about to spin the boards and want to know if this will affect the
mask manufacture.

Many thanks,

Jason.

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] URGENT!!!

2001-12-12 Thread Anthony Whitesell


No source or seed for the polygon to attach to.  The polygon is isolated
from its net.  Try placing a via in the region of the polygon and then
double click the polygon and press return in order to get the polygon to
rebuild.  I have been dealing with this over the past few days.

Anthony Whitesell
Sunrise Labs


-Original Message-
From: Sean James [mailto:[EMAIL PROTECTED]]
Sent: Wednesday, December 12, 2001 3:28 PM
To: Protel EDA Forum
Subject: [PEDA] URGENT!!!


What would keep a polygon pour from not forming if
A. There are no keepouts.
B. There are no areas present to create dead copper pours.
C. I am pouring over the same net.

Sean James
PCB Designer
Telecast Fiber Systems, Inc.
102 Grove Street
Worcester, MA 01605
(TEL) 508.754.4858 x33
(FAX) 413.541.6170



* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] URGENT!!!

2001-12-12 Thread Ted Tontis

make sure that remove dead copper is not selected.

Ted

-Original Message-
From: Sean James [mailto:[EMAIL PROTECTED]]
Sent: Wednesday, December 12, 2001 2:28 PM
To: Protel EDA Forum
Subject: [PEDA] URGENT!!!


What would keep a polygon pour from not forming if 
A. There are no keepouts.
B. There are no areas present to create dead copper pours.
C. I am pouring over the same net.

Sean James
PCB Designer
Telecast Fiber Systems, Inc.
102 Grove Street
Worcester, MA 01605
(TEL) 508.754.4858 x33
(FAX) 413.541.6170



* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] URGENT!!!

2001-12-12 Thread Narinder Kumar

May be there is nothing to connect No pad ) on that net in that area.

Narinder
- Original Message - 
From: Sean James [EMAIL PROTECTED]
To: Protel EDA Forum [EMAIL PROTECTED]
Sent: Wednesday, December 12, 2001 3:28 PM
Subject: [PEDA] URGENT!!!


What would keep a polygon pour from not forming if 
A. There are no keepouts.
B. There are no areas present to create dead copper pours.
C. I am pouring over the same net.

Sean James
PCB Designer
Telecast Fiber Systems, Inc.
102 Grove Street
Worcester, MA 01605
(TEL) 508.754.4858 x33
(FAX) 413.541.6170



* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] URGENT!!!

2001-12-12 Thread Darryl

Perhaps the polygons have been turned off, this has caught me out when I
have not had enough coffee.

Tools/ Preferences/ Show/Hide -polygons 'hidden'

Cheers,
Darryl Harrison

-Original Message-
From: Sean James [mailto:[EMAIL PROTECTED]]
Sent: Thursday, December 13, 2001 9:28 AM
To: Protel EDA Forum
Subject: [PEDA] URGENT!!!


What would keep a polygon pour from not forming if
A. There are no keepouts.
B. There are no areas present to create dead copper pours.
C. I am pouring over the same net.

Sean James
PCB Designer
Telecast Fiber Systems, Inc.
102 Grove Street
Worcester, MA 01605
(TEL) 508.754.4858 x33
(FAX) 413.541.6170


---
Incoming mail is certified Virus Free.
Checked by AVG anti-virus system (http://www.grisoft.com).
Version: 6.0.237 / Virus Database: 115 - Release Date: 3/7/01

---
Outgoing mail is certified Virus Free.
Checked by AVG anti-virus system (http://www.grisoft.com).
Version: 6.0.237 / Virus Database: 115 - Release Date: 3/7/01


* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] URGENT!!!

2001-12-12 Thread Brendon Slade

Has it successfully poured before now?

Is it just pouring outlines? - do you have No hatching selected?
Do you have minimum primitive size set to something outrageous?

Just some real quick thought.

HTH
Brendon.

- Original Message - 
From: Sean James [EMAIL PROTECTED]
To: Protel EDA Forum [EMAIL PROTECTED]
Sent: Thursday, December 13, 2001 9:28 AM
Subject: [PEDA] URGENT!!!


What would keep a polygon pour from not forming if 
A. There are no keepouts.
B. There are no areas present to create dead copper pours.
C. I am pouring over the same net.

Sean James
PCB Designer
Telecast Fiber Systems, Inc.
102 Grove Street
Worcester, MA 01605
(TEL) 508.754.4858 x33
(FAX) 413.541.6170




* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] URGENT!!!

2001-12-12 Thread Patrick Adair

Insure that polygons are not hidden under the show/hide options of the
display.

Patrick

-Original Message-
From: Narinder Kumar [mailto:[EMAIL PROTECTED]]
Sent: Wednesday, December 12, 2001 2:45 PM
To: Protel EDA Forum
Subject: Re: [PEDA] URGENT!!!


May be there is nothing to connect No pad ) on that net in that area.

Narinder
- Original Message -
From: Sean James [EMAIL PROTECTED]
To: Protel EDA Forum [EMAIL PROTECTED]
Sent: Wednesday, December 12, 2001 3:28 PM
Subject: [PEDA] URGENT!!!


What would keep a polygon pour from not forming if
A. There are no keepouts.
B. There are no areas present to create dead copper pours.
C. I am pouring over the same net.

Sean James
PCB Designer
Telecast Fiber Systems, Inc.
102 Grove Street
Worcester, MA 01605
(TEL) 508.754.4858 x33
(FAX) 413.541.6170



* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] URGENT!!!

2001-12-12 Thread Sean James

Never mind. It was a stupid rule.
Sean James
PCB Designer
Telecast Fiber Systems, Inc.
102 Grove Street
Worcester, MA 01605
(TEL) 508.754.4858 x33
(FAX) 413.541.6170

- Original Message - 
From: Brendon Slade [EMAIL PROTECTED]
To: Protel EDA Forum [EMAIL PROTECTED]
Sent: Wednesday, December 12, 2001 3:51 PM
Subject: Re: [PEDA] URGENT!!!


 Has it successfully poured before now?
 
 Is it just pouring outlines? - do you have No hatching selected?
 Do you have minimum primitive size set to something outrageous?
 
 Just some real quick thought.
 
 HTH
 Brendon.
 
 - Original Message - 
 From: Sean James [EMAIL PROTECTED]
 To: Protel EDA Forum [EMAIL PROTECTED]
 Sent: Thursday, December 13, 2001 9:28 AM
 Subject: [PEDA] URGENT!!!
 
 
 What would keep a polygon pour from not forming if 
 A. There are no keepouts.
 B. There are no areas present to create dead copper pours.
 C. I am pouring over the same net.
 
 Sean James
 PCB Designer
 Telecast Fiber Systems, Inc.
 102 Grove Street
 Worcester, MA 01605
 (TEL) 508.754.4858 x33
 (FAX) 413.541.6170
 
 
 
 

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] URGENT!!!

2001-12-12 Thread Abd ul-Rahman Lomax

At 03:28 PM 12/12/01 -0500, Sean James wrote:
What would keep a polygon pour from not forming if
A. There are no keepouts.
B. There are no areas present to create dead copper pours.
C. I am pouring over the same net.

Try turning off remove dead copper, see what you get. Dead copper is any 
polygon copper that has not connected to already-existing primitives, say a 
pad or via, assigned to the polygon net. If no such primitives exist, dead 
copper will be removed for the entire polygon, it is all dead.

While areas of isolation can create dead copper, dead copper is the 
default condition if there are no places for the polygon to pick up its net.

There may be other possible causes, such as a very high setting for grid 
and/or fill track width. Normally, grid should be set to 0. Contrary to 
what one might guess, zero grid means that grid is ignored and track is 
spaced with maximum efficiency for total fill.

If you turn off remove dead copper in the polygon dialog and your polygon 
appears, then the problem is the lack of a seed primitive. If this does not 
fix the problem, it is from another source.




[EMAIL PROTECTED]
Abdulrahman Lomax
Easthampton, Massachusetts USA

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] URGENT!!!

2001-12-12 Thread Bagotronix Tech Support

Hey, Abdul:

If any ATS dollars are to be paid, they should be paid to you!  You are
better tech support for Protel than any corporate Protel tech support I've
seen.

In the EE dictionary, under Altium Total Support, it says see Lomax, Abd
ul-Rahman.  ;-)

Best regards,
Ivan Baggett
Bagotronix Inc.
website:  www.bagotronix.com


- Original Message -
From: Abd ul-Rahman Lomax [EMAIL PROTECTED]
To: Protel EDA Forum [EMAIL PROTECTED]
Sent: Wednesday, December 12, 2001 4:56 PM
Subject: Re: [PEDA] URGENT!!!



* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] URGENT!!!

2001-12-12 Thread Brad Velander

Ivan,
you missed definitions 2  3 which stated, see Wilson, Ian and
see Harland, Geoff respectively.

Overall we have a great bunch of people on this forum and everyone
deserves acknowledgement for their contributions because it definitely is
much better then any technical support that I have received from numerous
CAD vendors. Let's keep it up through the Holidays and right through
whatever the new year brings from Protel/Altimatium.

Sincerely,
Brad Velander.

Lead PCB Designer
Norsat International Inc.
#300 - 4401 Still Creek Drive,
Burnaby, B.C., Canada, V5C 6G9.
Tel   (604) 292-9089 (direct line)
Fax  (604) 292-9010
Website: www.norsat.com


-Original Message-
From: Bagotronix Tech Support [mailto:[EMAIL PROTECTED]]
Sent: Wednesday, December 12, 2001 2:24 PM
To: Protel EDA Forum
Subject: Re: [PEDA] URGENT!!!


Hey, Abdul:

If any ATS dollars are to be paid, they should be paid to you!  You are
better tech support for Protel than any corporate Protel tech support I've
seen.

In the EE dictionary, under Altium Total Support, it says see Lomax, Abd
ul-Rahman.  ;-)

Best regards,
Ivan Baggett
Bagotronix Inc.
website:  www.bagotronix.com

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] URGENT!!!

2001-12-12 Thread Don Ingram

Ditto

Cheers
Don
- Original Message -
From: Bagotronix Tech Support [EMAIL PROTECTED]
To: Protel EDA Forum [EMAIL PROTECTED]
Sent: Thursday, December 13, 2001 8:24 AM
Subject: Re: [PEDA] URGENT!!!


 Hey, Abdul:

 If any ATS dollars are to be paid, they should be paid to you!  You are
 better tech support for Protel than any corporate Protel tech support I've
 seen.

 In the EE dictionary, under Altium Total Support, it says see Lomax, Abd
 ul-Rahman.  ;-)

 Best regards,
 Ivan Baggett
 Bagotronix Inc.
 website:  www.bagotronix.com


 - Original Message -
 From: Abd ul-Rahman Lomax [EMAIL PROTECTED]
 To: Protel EDA Forum [EMAIL PROTECTED]
 Sent: Wednesday, December 12, 2001 4:56 PM
 Subject: Re: [PEDA] URGENT!!!





* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] URGENT!!!

2001-12-12 Thread Brian Guralnick

If you have the option -remove dead copper- on  there is no access to the specified
pour over same net in the area where you wish to build this polygon.  This would in
fact start and seem to finish building the polygon, except it disappears right at the
end.

Also make sure your trace clearance gap rule is small enough so that a polygon can
actually be built.


Brian Guralnick


- Original Message -
From: Patrick Adair [EMAIL PROTECTED]
To: Protel EDA Forum [EMAIL PROTECTED]
Sent: Wednesday, December 12, 2001 4:02 PM
Subject: Re: [PEDA] URGENT!!!


| Insure that polygons are not hidden under the show/hide options of the
| display.
|
| Patrick
|
| -Original Message-
| From: Narinder Kumar [mailto:[EMAIL PROTECTED]]
| Sent: Wednesday, December 12, 2001 2:45 PM
| To: Protel EDA Forum
| Subject: Re: [PEDA] URGENT!!!
|
|
| May be there is nothing to connect No pad ) on that net in that area.
|
| Narinder
| - Original Message -
| From: Sean James [EMAIL PROTECTED]
| To: Protel EDA Forum [EMAIL PROTECTED]
| Sent: Wednesday, December 12, 2001 3:28 PM
| Subject: [PEDA] URGENT!!!
|
|
| What would keep a polygon pour from not forming if
| A. There are no keepouts.
| B. There are no areas present to create dead copper pours.
| C. I am pouring over the same net.
|
| Sean James
| PCB Designer
| Telecast Fiber Systems, Inc.
| 102 Grove Street
| Worcester, MA 01605
| (TEL) 508.754.4858 x33
| (FAX) 413.541.6170
|
|
|
|


* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] Urgent help needed

2001-10-25 Thread John M. Cardone

All,
Do you find these components (in the negative quadrant) in the gerber or
pick and place outputs?
jmc


Ian Wilson wrote:
 
 At 10:09 AM 25/10/01 +1000, you wrote:
 Ian, it's actually pretty easy to loose parts.
 We recently have had a situation where a group of components have been
 unknowingly moved into the negative region of the database as part of a
 move selection process early in the placement stage. It turns out that the
 syncroniser matches the parts and the pins for the netstherefore no
 missing components.The netlist exists in the database but the physical
 ratsnest does not (I assume the physical ratsnest is only valid for the
 database extents). The DRC was 100% ok. It would appear that the DRC makes
 the assumption that if there is a valid net but no ratsnest then the net
 must be connected. (ie no broken net) (also no clearance errors either)
 
 I would be interested if anyone else has had this problem.
 We use SP6, W98
 
 We only found it by noticing an associated text string on the left hand edge
 of the database area when zoomed right out.
 
 I too have seen the moving components (not for a long time though), for me
 at least, they have always existed in the netlist and the component
 report.  I had not noticed what happens to the ratsnest when a component is
 off in ga-ga land but it still exists in the database, the netlist, the
 component report, the ASCII PCB version and even component browser. I have
 not checked if they exist in an exported spreadsheet.
 
 Thanks for the info on the ratsnets not showing for the gone-ape
 components (technical term),
 Ian Wilson

-- 

John M. Cardone   Electro-Mechanical Dsgn. Engr. Grp.
M/S 278-100   Mechanical Engineering Section, 352
4800 Oak Grove Dr.NASA / Jet Propulsion Laboratory
Pasadena, Ca 91109 
Tel: 818.354.5407 MailTo:[EMAIL PROTECTED]
Fax: 818.393.4860


* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] Urgent help needed

2001-10-25 Thread rlamoreaux



I have had a library update cause a part to go haywire when the origin of
the library part was way off from the center of the part. This was due to
the library being imported from another package if I remember correctly.

I have had a component move off the viewable area, and found a way to fix
it relatively quickly.

First I output a pick and place the assembly.
Next I find the part in question in the pick and place and I change it's
x,y location to a good location
Now I go back to the PCB and I select Tools Autoplacer Place from file and
I use the changed PIK file to place the part in a good location.

Rob


* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] Urgent help needed

2001-10-25 Thread M. Wahab

I actually made a J C, but was never able to locate it.
However, With the help I got I was able to fix the problem
thanks to all who took the time to respond.



M. Wahab

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] Urgent help needed

2001-10-24 Thread Abd ul-Rahman Lomax

At 07:52 AM 10/24/01 +0200, Emanuel Zimmermann wrote:
Maybe that the reference point for the .lib part moved for whatever reason.
This can cause the component to be placed out of the working area after update
PCB operation.

Good thinking.

Yes, that would do it, and it is not a terribly uncommon error. Move 
Component, clicked onto an empty space, will pull up a list of components, 
which will allow picking the component up. One will be able to tell 
immediately what its extents are when it is being moved. Editing it from 
the panel is another possibility, just change the XY coordinates by adding 
or subtracting appropriate values (remember, Protel will think that the 
component is at the reference position, which in this case will *not* be 
where the primitives are located.

Modifying the library part to put the reference on pin 1 or on the centroid 
and then running update component should also do it, probably the easiest 
and best solution. I'd look at the library part first and see where the 
reference is living



[EMAIL PROTECTED]
Abdulrahman Lomax
Easthampton, Massachusetts USA

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] Urgent help needed

2001-10-24 Thread Ian Wilson

On 03:07 PM 24/10/2001 -0700, Abd ul-Rahman Lomax said:
At 07:52 AM 10/24/01 +0200, Emanuel Zimmermann wrote:
Maybe that the reference point for the .lib part moved for whatever reason.
This can cause the component to be placed out of the working area after 
update
PCB operation.

Good thinking.

Yes, that would do it, and it is not a terribly uncommon error. Move 
Component, clicked onto an empty space, will pull up a list of components, 
which will allow picking the component up. One will be able to tell 
immediately what its extents are when it is being moved. Editing it from 
the panel is another possibility, just change the XY coordinates by adding 
or subtracting appropriate values (remember, Protel will think that the 
component is at the reference position, which in this case will *not* be 
where the primitives are located.


This is exactly why I suggested that the netlist or component report should 
be checked or even just use J-C to see if the component is still around 
somewhere.  Though I suspect that this is not happening in this case as it 
would be pretty hard to loose a large BGA package due to a shift - you 
would think you would notice it sitting around somewhere.  The ratsnest 
would certainly show something interesting.

Ian Wilson


* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] Urgent help needed

2001-10-24 Thread ICT Mail

Ian, it's actually pretty easy to loose parts.
We recently have had a situation where a group of components have been
unknowingly moved into the negative region of the database as part of a
move selection process early in the placement stage. It turns out that the
syncroniser matches the parts and the pins for the netstherefore no
missing components.The netlist exists in the database but the physical
ratsnest does not (I assume the physical ratsnest is only valid for the
database extents). The DRC was 100% ok. It would appear that the DRC makes
the assumption that if there is a valid net but no ratsnest then the net
must be connected. (ie no broken net) (also no clearance errors either)

I would be interested if anyone else has had this problem.
We use SP6, W98

We only found it by noticing an associated text string on the left hand edge
of the database area when zoomed right out.


-Original Message-
From: Ian Wilson [mailto:[EMAIL PROTECTED]]
Sent: Thursday, 25 October 2001 8:36 AM
To: Protel EDA Forum
Subject: Re: [PEDA] Urgent help needed


On 03:07 PM 24/10/2001 -0700, Abd ul-Rahman Lomax said:
At 07:52 AM 10/24/01 +0200, Emanuel Zimmermann wrote:
Maybe that the reference point for the .lib part moved for whatever
reason.
This can cause the component to be placed out of the working area after
update
PCB operation.

Good thinking.

Yes, that would do it, and it is not a terribly uncommon error. Move
Component, clicked onto an empty space, will pull up a list of components,
which will allow picking the component up. One will be able to tell
immediately what its extents are when it is being moved. Editing it from
the panel is another possibility, just change the XY coordinates by adding
or subtracting appropriate values (remember, Protel will think that the
component is at the reference position, which in this case will *not* be
where the primitives are located.


This is exactly why I suggested that the netlist or component report should
be checked or even just use J-C to see if the component is still around
somewhere.  Though I suspect that this is not happening in this case as it
would be pretty hard to loose a large BGA package due to a shift - you
would think you would notice it sitting around somewhere.  The ratsnest
would certainly show something interesting.

Ian Wilson


* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] Urgent help needed

2001-10-24 Thread Ian Wilson

At 10:09 AM 25/10/01 +1000, you wrote:
Ian, it's actually pretty easy to loose parts.
We recently have had a situation where a group of components have been
unknowingly moved into the negative region of the database as part of a
move selection process early in the placement stage. It turns out that the
syncroniser matches the parts and the pins for the netstherefore no
missing components.The netlist exists in the database but the physical
ratsnest does not (I assume the physical ratsnest is only valid for the
database extents). The DRC was 100% ok. It would appear that the DRC makes
the assumption that if there is a valid net but no ratsnest then the net
must be connected. (ie no broken net) (also no clearance errors either)

I would be interested if anyone else has had this problem.
We use SP6, W98

We only found it by noticing an associated text string on the left hand edge
of the database area when zoomed right out.


I too have seen the moving components (not for a long time though), for me 
at least, they have always existed in the netlist and the component 
report.  I had not noticed what happens to the ratsnest when a component is 
off in ga-ga land but it still exists in the database, the netlist, the 
component report, the ASCII PCB version and even component browser. I have 
not checked if they exist in an exported spreadsheet.

Thanks for the info on the ratsnets not showing for the gone-ape 
components (technical term),
Ian Wilson


* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] Urgent help needed

2001-10-23 Thread Daniel Webster

Wahab:

If you check in your Protel backup directory on your harddisk, you will
likely find a backup of the library where your BGA footprint existed. Rename
the backup file to a .LIB name and open in Protel to see if your old
footprint is there.

Daniel

-Original Message-
From: M. Wahab [mailto:[EMAIL PROTECTED]]
Sent: Tuesday, October 23, 2001 11:06 AM
To: Protel EDA Forum
Subject: [PEDA] Urgent help needed


Hi,

I was updating from a pcb library a footprint of
a BGA component, however, the component disappeared 
completely.
What went wrong? is there anyway to recover? It doesn't accept
undo, and it's very difficult to position a new BGA footprint
in place of the disappeared one. Back up is affected as well.

Help is grately appreciated.

Thanks
M. Wahab

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] Urgent help needed

2001-10-23 Thread Ian Wilson

On 02:06 PM 23/10/2001 -0400, M. Wahab said:
Hi,

 I was updating from a pcb library a footprint of
a BGA component, however, the component disappeared
completely.

This sounds odd.  Was there anything unusual about the footprint?  How did 
you do the update, by pressing Update PCB from within the PCBLIb editor?

If you produce a netlist or a component report is the component designator 
still listed?  Can you jump to the component designator (with J-C)?

What went wrong? is there anyway to recover? It doesn't accept
undo, and it's very difficult to position a new BGA footprint
in place of the disappeared one. Back up is affected as well.

If your backups are affected then I assume you are not using the auto-save 
server to regularly save open files?  What about the backed up DDB (*.DBK 
is it)?  here are at least three forms of backups produced by Protel 
(including the auto-saved files) - have you checked all of these?

Older versions of the file? Your regular back-ups?

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] Urgent help needed

2001-10-23 Thread Abd ul-Rahman Lomax

At 02:06 PM 10/23/01 -0400, M. Wahab wrote:
 I was updating from a pcb library a footprint of
a BGA component, however, the component disappeared
completely.
What went wrong? is there anyway to recover? It doesn't accept
undo, and it's very difficult to position a new BGA footprint
in place of the disappeared one. Back up is affected as well.

(1) I don't know what happened.

(2) You should have backups for all the files involved (your library and 
your PCB), and there are normally, assuming you have autoback enabled -- 
ask if you do not know how to do that, two different backups, one in the 
backup directory for autobackups, plus two (Backup of ... and Previous 
Backup of ...) in the directory where the ddb lives. You'll need to import 
the latter.

Note that autoback can fail to operate if one constantly keeps the program 
in a state where there is a pending operation. Protel allows pending 
operations to be stacked, so occasionally one should back up through the 
stack with the Escape key.

But the other backups are created whenever you overwrite a file in the 
.ddb, if this is an option, I haven't noticed. Some users don't like them, 
but they are easy to generically delete because of the really distinctive 
names.

(3) To replace a routed component accurately, select the component, use 
Move Block, and pick up the component at a pad center that corresponds to a 
now-hanging track end. The current layer should be set to that track's 
layer. Snap will now place the component *exactly* as it was when the track 
was completed, assuming it was on grid. (Good practice leaves track ends 
coincident with pad centers.)


[EMAIL PROTECTED]
Abdulrahman Lomax
Easthampton, Massachusetts USA


* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] Urgent help needed

2001-10-23 Thread Emanuel Zimmermann



Abd ul-Rahman Lomax wrote:


 (1) I don't know what happened.

Maybe that the reference point for the .lib part moved for whatever reason.
This can cause the component to be placed out of the working area after update
PCB operation.


 (3)  (Good practice leaves track ends
 coincident with pad centers.)

Really good advise!


Regards,

Emanuel

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