[PCB_FORUM] Re: How do I preserve REFDESs when packing in Allegro Design Entry HDL...
- From: Jerry Grzenia <geraldg@xxxxxxxxxxx>
- To: "icu-pcb-forum@xxxxxxxxxxxxx" <icu-pcb-forum@xxxxxxxxxxxxx>
- Date: Tue, 19 Apr 2011 07:46:19 -0700
Hi Austin,
There are only a couple causes for the ref des values to change and parts
getting ripped up in Allegro -
1. You've deleted the package folder files.
2. You don't select the preserve option in Export Physical.
3. Several part names/properties in DEHDL have changed.
Short of these, ref des values should be maintained.
This is why I've asked for a testcase - so we can examine the issue as it
indeed is very odd.
Jerry
-----Original Message-----
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of
allegrolist@xxxxxxxxxxxx
Sent: Tuesday, April 19, 2011 9:08 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: How do I preserve REFDESs when packing in Allegro
Design Entry HDL...
Hi Mark,
THANK YOU! That worked great. It was only 8 pages, so only 5 minutes to
do. All the components that shouldn't have been ripped up, now aren't!
Back on my merry way again ;-)
The question really, for Cadence that is, is why on earth does it redo the
REFDESs in the first place? And, even when it redoes them, why does it
rip-up components that are still in the design, and had no change except
the REFDES...and it doesn't do that to all of them, only some of them.
Best Regards,
Austin
Original Message:
-----------------
From: Mark Salberg msalberg@xxxxxxxxxxxx
Date: Tue, 19 Apr 2011 06:40:20 -0400
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: How do I preserve REFDESs when packing in Allegro
Design Entry HDL...
Austin,
We usually replace $LOCATION with LOCATION for every ref des if this
happens.
It hard locates all ref des instead of $LOCATION (Soft location)
Unfortunately, you have to do find / replace on each page.
1. Start the Project Manager and open your project.
2. Start Design Entry
3. In the Concept Console Window type: find $location Note:
find $LOCATION can be copied, then Ctrl V to paste in each
page. Paste does not work?
A group will be created and the number of occurrences found
on that page, will be
listed in the Console Window along with the group name. See
example below:
4. Either Type: change "group name" Enter appropriate group
name. (i.e.) change A in cmmand window
(OR) *Select Group / Text Change [A]* pull-down menu
Note: All members of the group should be temporarily hilited.
Note: If group selections are "grayed out", then select the
correct group in the group tool bar.
(below the schematic)
5. Next, Rt Click and select Editor (see below) or typeCtrl+E.
The window seen below will appear.
*Note:* This will start theText Editor tool and display a
listing of ALL group members...
6. From the pull-downs, select Edit / Replace. A window will
appear.
7. On the Find line enter $LOCATION (This is case sensitive.)
On the Replace line enter LOCATION
Select Replace All.
*Note:*When complete select File->Savein the text editor.
You may then close the Text Editor.
8. In Concept select File->Save to write the schematic page.
9. Repeat for all schematic pages
Regards,
Mark
On 4/18/2011 11:25 PM, allegrolist@xxxxxxxxxxxx wrote:
> Hi Jerry,
>
> Thanks for the help. I don't have a small test case. I could try making
> one...and perhaps in the morning, I may try that. This is pretty
> frustrating. I know it worked correctly at one time, as an older BOM has
> the correct REFDESs, but every new BOM/netlist I generate has the REDESs
> redone. I really wouldn't care if they were redon if when I read it in to
> the layout, it didn't unpace components that shouldn't be unplaced...and
> therefore get their traces ripped up.
>
> So, I'll figure out what to try next in the morning. It's been a very
> frustrating afternoon/evenin/night trying to figure out what's going on
> here.
>
> Best Regards,
>
> Austin
>
>
> Original Message:
> -----------------
> From: Jerry Grzenia geraldg@xxxxxxxxxxx
> Date: Mon, 18 Apr 2011 18:23:17 -0700
> To: icu-pcb-forum@xxxxxxxxxxxxx, icu-pcb-forum@xxxxxxxxxxxxx
> Subject: [PCB_FORUM] Re: How do I preserve REFDESs when packing in Allegro
> Design Entry HDL...
>
>
> Hi Austin,
>
> If you have a small testcase, please send it to Customer Support, we'll
> take a look at it for you.
>
>
>
> Regards,
>
> Jerry Grzenia
>
> -----Original Message-----
> From: allegrolist@xxxxxxxxxxxx [mailto:allegrolist@xxxxxxxxxxxx]
> Sent: Monday, April 18, 2011 04:25 PM Pacific Standard Time
> To: icu-pcb-forum@xxxxxxxxxxxxx
> Subject: [PCB_FORUM] Re: How do I preserve REFDESs when packing in
> Allegro
> Design Entry HDL...
>
> Hi Jerry,
>
> I do exactly both of those, and it still redoes the REFDESs. It makes
them
> sequential, and fills in the gaps. I'm obviously missing something, and
> it's very frustrating. I've tried quite a few things, just not hit on the
> right one yet.
>
> Thanks!
>
> Austin
>
> Original Message:
> -----------------
> From: Jerry Grzenia geraldg@xxxxxxxxxxx
> Date: Mon, 18 Apr 2011 14:01:05 -0700
> To: icu-pcb-forum@xxxxxxxxxxxxx
> Subject: [PCB_FORUM] Re: How do I preserve REFDESs when packing in Allegro
> Design Entry HDL...
>
>
> Hi Austin,
>
>
>
> First, don't "repackage". In the Export Physical form, make sure you have
> "Preserve" checked:
>
> [cid:image001.png@01CBFDE1.D26367B0]
>
>
>
> Click on the Advanced button (upper right above), select the Layout tab.
>
> Make sure the option for "Reuse Ref Des numbers" is NOT checked:
>
> [cid:image002.png@01CBFDE1.D26367B0]
>
>
>
> Jerry
>
>
>
> -----Original Message-----
> From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
> [mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of
> allegrolist@xxxxxxxxxxxx
> Sent: Monday, April 18, 2011 3:31 PM
> To: icu-pcb-forum@xxxxxxxxxxxxx
> Subject: [PCB_FORUM] How do I preserve REFDESs when packing in Allegro
> Design Entry HDL...
>
>
>
> Hi,
>
>
>
> Every time I repackage (Design Entry HDL, 15.7), it reassigns the REFDESs.
>
> I want to keep the existing REFDESs (and their gaps). How can I specify
>
> this?
>
>
>
> Thanks,
>
>
>
> Austin
>
>
>
>
>
> --------------------------------------------------------------------
>
> mail2web.com - Microsoft(r) Exchange solutions from a leading provider -
>
> http://link.mail2web.com/Business/Exchange
>
>
>
>
>
> -----------------------------------------------------------
>
> 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
>
> -----------------------------------------------------------
>
>
> --------------------------------------------------------------------
> mail2web - Check your email from the web at
> http://link.mail2web.com/mail2web
>
>
> -----------------------------------------------------------
> 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
> -----------------------------------------------------------
>
N<.nÇ+0/00·¿º{.nÇ+0/00·'zwZ^(TM)ë,j
¢'.¥Æߢ»¦ê®zË_ç¥S(Ël¢¸0S(ØZ²æãyËh~Ë>±
Êâmê+º{.nÇ+0/00
>
·"¢øz(ÂØ^j·!S(÷¬¡ûaS(Éb²Ø(¶^m¶Y"ÿÃ
ç¥S(Ël¢¸?j·!S(÷¬þ'.¥Æߢ»¦üúènW¦²S(йë-S
(0/00ìIéÝjw
> ¦j)m¢'.¥Æߢ»¦iÙ¢z(Çëyéb²Û(®ã
>
> --------------------------------------------------------------------
> mail2web - Check your email from the web at
> http://link.mail2web.com/mail2web
>
>
> -----------------------------------------------------------
> 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
> -----------------------------------------------------------
--------------------------------------------------------------------
myhosting.com - Premium Microsoft® Windows® and Linux web and application
hosting - http://link.myhosting.com/myhosting
-----------------------------------------------------------
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
-----------------------------------------------------------
-----------------------------------------------------------
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
-----------------------------------------------------------
Other related posts:
