[PCB_FORUM] Re: squares on same clines intersections
- From: rjbzxr@xxxxxxxxxxxx
- To: icu-pcb-forum@xxxxxxxxxxxxx
- Date: Fri, 02 Jun 2006 12:30:14 -0400
Q1. What is this diamond mark?
This diamond mark is referred to as a "connect point" or "cpoint". The
displayed
size of this connect point is controlled by the "Connect point size" field
in the Drawing Options >Display Tab
Q2. Do any of these marks influence a design?
There is no "influence" of the design other than marking where a FIXED cline
segment joins a cline segment that does not have the FIXED property.
Q3. Is this a "feature" for the fixed segment?
This is a feature of the fixed segment which lets the user know where clines
join that have differing FIXED property values.
This is explained in the documentation titled:
"Allegro/APD Design Guide: Routing -- 2. Interactive Routing"
in the section labeled:
Connection Behavior in Groups
If the user would like to remove these connect points they can perform the
following:
1. Remove the FIXED property from the clines
2. Use Edit >Move and select all of the clines
3. In the command area type:
ix 0
This will merge the clines into one segment as can be seen by performing a "Show
Element on the clines before and after the above steps are performed. Please
have
only CLINES selected in the FIND filter.
-----Original Message-----
From: george.h.patrick@xxxxxxxxxxxxxx
To: icu-pcb-forum@xxxxxxxxxxxxx
Sent: Fri, 2 Jun 2006 08:41:36 -0700
Subject: [PCB_FORUM] Re: squares on same clines intersections
The diamond denotes a Tee point or a cline coming from a module. I have also
seen them occasionally when a line runs across a constraint areas (usually
shows up when you slide such a line). I have only seen them not able to be
deleted when something associated with the cline is fixed. If the cline is
part of a module you may need to unfix the module.
If none of that helps you should try running dbdoctor on the database.
Good luck!
--
George Patrick
Tektronix, Inc.
Central Engineering, Engineering Design Services
P.O. Box 500, M/S 39-512
Beaverton, OR 97077-0001
Å 503-627-5272 (voice) Æ 503-627-5587 (fax)
http://www.tektronix.com http://www.pcb-designer.com
"Off-Grid and Proud of it!"
-----Original Message-----
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of William Billereau
Sent: Friday, June 02, 2006 01:02
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: squares on same clines intersections
Hello Chris (Vince?)
Here is a screenshot.
The rhombus is inside the red ellipse.
Delete clines only selects the clines on the right of the rhombus (the
temporary highlighted on) but not the left part of the cline (I redraw it with
a thin blue line)
A derive connectivity does not correct the probleme.
William.
=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=
| Billereau William | PCB Designer |
| | Tel: (+4122) 76 73403 |
| CERN TS/DEM | william.billereau@xxxxxxx |
| 1211 Geneve 23 Switzerland | Société: AMEC-SPIE/Electrotech |
=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=-=
-----Original Message-----
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of vince fornier
Sent: 01 June, 2006 11:50 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: squares on same clines intersections
> On some jobs, we re-route traces and then we got rhombuses (rotated
> squares) on same clines intersections. It is the same net, connection
> is done but it causes that delete clines (not clines segs) deletes
> only part before or after these squares.
>
> What and where to change to remove these squares and make complete
> clines?
Some screenshots would be helpful. But I think I understand your issue: one or
more of the sides of the rhombus is not a cline but rather a collection of
clines that look to the eye as one continuous trace - so instead of doing
"delete clines" once you must do it mulitple times to clear up all the little
stubs?
If such is the case, you could delete one such short cline which would
implicitly make the others part of a dangline cline(s). Do this for all the
rhombuses , then you could scrub all the affected nets with SKILL routine
find_dlines
HTH,
Chris Walters
local Cadence guru
(Apple)
_______________________________________________
Join Excite! - http://www.excite.com
The most personalized portal on the Web!
-----------------------------------------------------------
To subscribe/unsubscribe:
Send a message to icu-pcb-forum-request@xxxxxxxxxxxxx
with a subject of subscribe or unsubscribe
To view the archives of this list go to
//www.freelists.org/archives/icu-pcb-forum/
Problems or Questions:
Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx
-----------------------------------------------------------
___________________________________________________
Try the New Netscape Mail Today!
Virtually Spam-Free | More Storage | Import Your Contact List
http://mail.netscape.com
Other related posts:
