[PEDA] NPT mounting holes

2002-03-25 Thread Gerald Gierach

Hi again, 
Do I need to have a pad size greater than zero for a NPT hole (mounting) or should I make it equal to zero.


Jerry Gierach

PCB Design Tech

Electro-Pro, Inc.

W66 N205 Commerce Court

P.O. Box 409

Cedarburg, Wi. 53012

Phone: 262-376-4574

Fax: 262-376-4575

[EMAIL PROTECTED]

[EMAIL PROTECTED]



Get your FREE download of MSN Explorer at http://explorer.msn.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] NPT mounting holes

2002-03-25 Thread Brad Velander

Jerry,
I don't know of any fabrication issue with the pad size if it is a NPT
pad, as long as the pad is reasonably smaller  or larger then the hole size.
Too close to the exact hole size and it can result in slivers of copper
which may endanger the integrity of the board if it breaks free and traps
somewhere that it shouldn't.
In P99SE there is a small bug in Print Preview that can account for
pads/holes not being printed under some conditions of pad size,layers and
plated/nonplated holes.

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 S8155 at NAB 2002 in Las Vegas April 8 - 11.


-Original Message-
From: Gerald Gierach [mailto:[EMAIL PROTECTED]]
Sent: Monday, March 25, 2002 9:29 AM
To: Protel EDA Forum
Subject: [PEDA] NPT mounting holes


Hi again, 
Do I need to have a pad size greater than zero for a NPT hole (mounting) or
should I make it equal to zero. 

Jerry Gierach
PCB Design Tech
Electro-Pro, Inc.
W66 N205 Commerce Court
P.O. Box 409
Cedarburg, Wi. 53012
Phone: 262-376-4574
Fax: 262-376-4575

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] NPT mounting holes

2002-03-25 Thread Gerald Gierach

Thanks Brad.


Jerry Gierach

PCB Design Tech

Electro-Pro, Inc.

W66 N205 Commerce Court

P.O. Box 409

Cedarburg, Wi. 53012

Phone: 262-376-4574

Fax: 262-376-4575

[EMAIL PROTECTED]

[EMAIL PROTECTED]






From: "Brad Velander" <[EMAIL PROTECTED]>
Reply-To: "Protel EDA Forum" <[EMAIL PROTECTED]>
To: "'Protel EDA Forum'" <[EMAIL PROTECTED]>
Subject: Re: [PEDA] NPT mounting holes 
Date: Mon, 25 Mar 2002 09:53:05 -0800 
 
Jerry, 
 I don't know of any fabrication issue with the pad size if it is a NPT 
pad, as long as the pad is reasonably smaller or larger then the hole size. 
Too close to the exact hole size and it can result in slivers of copper 
which may endanger the integrity of the board if it breaks free and traps 
somewhere that it shouldn't. 
 In P99SE there is a small bug in Print Preview that can account for 
pads/holes not being printed under some conditions of pad size,layers and 
plated/nonplated holes. 
 
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 S8155 at NAB 2002 in Las Vegas April 8 - 11. 
 
 
-Original Message- 
From: Gerald Gierach [mailto:[EMAIL PROTECTED]] 
Sent: Monday, March 25, 2002 9:29 AM 
To: Protel EDA Forum 
Subject: [PEDA] NPT mounting holes 
 
 
Hi again, 
Do I need to have a pad size greater than zero for a NPT hole (mounting) or 
should I make it equal to zero. 
 
Jerry Gierach 
PCB Design Tech 
Electro-Pro, Inc. 
W66 N205 Commerce Court 
P.O. Box 409 
Cedarburg, Wi. 53012 
Phone: 262-376-4574 
Fax: 262-376-4575 
 
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 
* 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 
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 
Chat with friends online, try MSN Messenger: Click Here

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] NPT mounting holes

2002-03-25 Thread Brian Sherer

It's useful to have a pad of finite size so that it'll be visible as a
reminder
in case you have (Show) Pad Holes turned off on the Design\Options
panel. Best to make an NPT pad up as a single-layer pad on the Drill 
Drawing Layer; this avoids creating objects on the Mask Layers during
Gerber generation, and eliminates error messages during DRC. I use 
10mil diameter pad for standard boards, with the hole size adjusted to suit.

Brian
Foothill Services LLC


* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] NPT mounting holes

2002-03-25 Thread Steve Baldwin


 I don't know of any fabrication issue with the pad size if it is a
 NPT
 pad, as long as the pad is reasonably smaller  or larger then the hole
 size. 

Something that I've been caught by a couple of times is having a 
pad on NPTH holes that are the same size as my fiducials. It 
seems that the CAM operator would see that all my NPTH holes 
had a particular size pad, select them based on that, then delete 
them all. It had me scratching my head for a while, thinking What 
is wrong with my Gerbers ?. It's clearly an error on the part of the 
board house, but now that I know, I've changed my library parts to 
stop the situation arising.

Steve.

==
Steve BaldwinElectronic Product Design
TLA Microsystems Ltd Microcontroller Specialists
PO Box 15-680, New Lynn  http://www.tla.co.nz
Auckland, New Zealandph  +64 9 820-2221
email: [EMAIL PROTECTED]  fax +64 9 820-1929
==

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] NPT mounting holes

2002-03-25 Thread DUTTON Phil




Re: [PEDA] NPT mounting holes

2002-03-25 Thread Igor Gmitrovic

Jerry,

I make the pad and the hole size the same and tick off the Plated box in
the Pad-Advanced menu. It works fine with the Print Preview and my PCB
manufacturer doesn't complain.

Igor

-Original Message-
From: Brad Velander [mailto:[EMAIL PROTECTED]]
Sent: Tuesday, 26 March 2002 4:53 AM
To: 'Protel EDA Forum'
Subject: Re: [PEDA] NPT mounting holes


Jerry,
I don't know of any fabrication issue with the pad size if it is a NPT
pad, as long as the pad is reasonably smaller  or larger then the hole size.
Too close to the exact hole size and it can result in slivers of copper
which may endanger the integrity of the board if it breaks free and traps
somewhere that it shouldn't.
In P99SE there is a small bug in Print Preview that can account for
pads/holes not being printed under some conditions of pad size,layers and
plated/nonplated holes.

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 S8155 at NAB 2002 in Las Vegas April 8 - 11.


-Original Message-
From: Gerald Gierach [mailto:[EMAIL PROTECTED]]
Sent: Monday, March 25, 2002 9:29 AM
To: Protel EDA Forum
Subject: [PEDA] NPT mounting holes


Hi again, 
Do I need to have a pad size greater than zero for a NPT hole (mounting) or
should I make it equal to zero. 

Jerry Gierach
PCB Design Tech
Electro-Pro, Inc.
W66 N205 Commerce Court
P.O. Box 409
Cedarburg, Wi. 53012
Phone: 262-376-4574
Fax: 262-376-4575

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] NPT mounting holes

2002-03-25 Thread Geoff Harland

 It's useful to have a pad of finite size so that it'll be visible as a
 reminder in case you have (Show) Pad Holes turned off on
 the Design\Options panel. Best to make an NPT pad up as a
 single-layer pad on the Drill Drawing Layer; this avoids creating
 objects on the Mask Layers during Gerber generation, and
 eliminates error messages during DRC. I use 10mil diameter
 pad for standard boards, with the hole size adjusted to suit.

 Brian

While I appreciate that using pads on the Drill Drawing Layer avoids
creating images on the Solder Mask layers, printouts of the Drill Drawing
layer are problematic for such pads; only those pads which are located on
the MultiLayer layer, and external copper layers (I think), have their
associated hole diameters depicted, and counted, in printouts of the Drill
Drawing layer. (However, these holes *are* listed and counted in the NC
Drill files.)

As such, I confine all pads having an associated hole to the MultiLayer
layer (see below for more details).

 I make the pad and the hole size the same and tick off the Plated box in
 the Pad-Advanced menu. It works fine with the Print Preview and my PCB
 manufacturer doesn't complain.

 Igor

  Do I need to have a pad size greater than zero for a NPT hole (mounting)
  or should I make it equal to zero.
 
  Jerry Gierach

Personal preference to some extent, but I set each such pad's pad diameter
equal to its hole diameter when saving the PCB file, and when generating
printouts. And when I want to generate Gerber files, I set the pad diameter
of all such pads equal to zero.

I have created a process within my PcbAddon server which facilitates either
zeroing all such pad diameters (for pads having unplated holes) or setting
the pad diameter of each such pad equal to its hole diameter.

Setting the pad diameter equal to hole diameter when producing printouts
means that the associated hole gets to be depicted in the printouts; OTOH,
there is no merit in flashing such pads within Gerber files (because any
copper within the associated hole's boundary does not end up within the
final PCB). While it arguably doesn't hurt to have such pads flashed (as
long as the diameter of the flash is less than the diameter of the pad's
hole), eliminating a flash all together results in smaller Gerber files.

Regards,
Geoff Harland.
-
E-Mail Disclaimer
The Information in this e-mail is confidential and may be legally
privileged. It is intended solely for the addressee. Access to this
e-mail by anyone else is unauthorised. If you are not the intended
recipient, any disclosure, copying, distribution or any action taken
or omitted to be taken in reliance on it, is prohibited and may be
unlawful. Any opinions or advice contained in this e-mail are
confidential and not for public display.


* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] NPT mounting holes

2002-03-25 Thread Bob Wolfe

Also I believe there is an extra process step involved when you have pad
area on a NPT hole. Most vendors I have delt with asked if they could plate
the hole
in some cases we said yes in others we said no and they delt with it.
In most of the cases they were just mounting holes (not tooling) and the pad
was only there to provide a keepout for routing and parts, and we either
just let the vendor plate those or actually when processing gerbers did not
add these pads to output or output a smaller pad than hole.
It was very easy back with 274D to set up standard aperture lists to handle
it
automatically.
Seems there are a few ways in Protel and your own preferences to handle this
but if your board
house is needing extra steps to do something you could prevent in your
output process he is probably charging you for them.
So talk to your house also.

Robert M. Wolfe, C.I.D.
[EMAIL PROTECTED]
- Original Message -
From: Steve Baldwin [EMAIL PROTECTED]
To: Protel EDA Forum [EMAIL PROTECTED]
Sent: Monday, March 25, 2002 3:22 PM
Subject: Re: [PEDA] NPT mounting holes



  I don't know of any fabrication issue with the pad size if it is a
  NPT
  pad, as long as the pad is reasonably smaller  or larger then the hole
  size.

 Something that I've been caught by a couple of times is having a
 pad on NPTH holes that are the same size as my fiducials. It
 seems that the CAM operator would see that all my NPTH holes
 had a particular size pad, select them based on that, then delete
 them all. It had me scratching my head for a while, thinking What
 is wrong with my Gerbers ?. It's clearly an error on the part of the
 board house, but now that I know, I've changed my library parts to
 stop the situation arising.

 Steve.

 ==
 Steve BaldwinElectronic Product Design
 TLA Microsystems Ltd Microcontroller Specialists
 PO Box 15-680, New Lynn  http://www.tla.co.nz
 Auckland, New Zealandph  +64 9 820-2221
 email: [EMAIL PROTECTED]  fax +64 9 820-1929
 ==


* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] NPT mounting holes

2002-03-25 Thread Steve Baldwin

 Also I believe there is an extra process step involved when you have
 pad area on a NPT hole. 

I've talked to a couple of vendors about the implications of 
PTH/NPTH holes. Their requirements are essentially that they want 
copper of the minimum annular ring outside of the hole for PTH and 
that amount of clearance inside the hole for NPTH due to drilling 
tolerance. That assumes a hole that is small enough to be masked 
by the etch resist and those holes will be drilled prior to plating (no 
cost penalty). The allowable size of the hole seems to vary quite a 
bit and isn't usually published (that I've noticed).
If the hole is bigger than that threshold, it will be done on the 
routing machine near the end of the process. Probing a bit further 
with one vendor, I found out that although the NPTH drill and the 
outline routing run on the same machine, they are two separate 
programs so the boards go through it twice. (This particular place 
was rather 'low-end' so I don't know how applicable that it to other 
fab shops).
In the case of the vanishing fiducials, the board house was getting 
so many boards with pads the same size as the holes for NPTH 
holes, they have got into the habit of removing all pads from NPTH 
drill sites. That's quite reasonable except that the CAM operator 
decided to select based on pad size and that caused my fiducials 
to fall off.

Regards,

Steve.

==
Steve BaldwinElectronic Product Design
TLA Microsystems Ltd Microcontroller Specialists
PO Box 15-680, New Lynn  http://www.tla.co.nz
Auckland, New Zealandph  +64 9 820-2221
email: [EMAIL PROTECTED]  fax +64 9 820-1929
==

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