[PCB_FORUM] Re: extracting X-net lengths
- From: "Reade, Sue" <Sue.Reade@xxxxxxxxxxx>
- To: <icu-pcb-forum@xxxxxxxxxxxxx>
- Date: Wed, 23 Mar 2005 08:40:12 -0600
Our input is 3rd party netlist. I was going through the same sort of
thing with Xnets. This is what Cadence sent me this instruction. I have
not yet tried this on the board I'm working on. If this works correctly,
your board lengths should show up in the constraint spreadsheet.
One way to accomplish this using Allegro Expert is to create a single
pin pair
in the Constraint Manager Spreadsheet, create a Topology file in
SigXplorer and
update the topology in the Constraint Manager Spreadsheet with the new
Electrical
CSet. Then select all other nets in the Spreadsheet and add these nets
to the
new Electrical CSet.
It is recommended to start with a clean database that does not have any
properties
or Electrical CSets assigned to nets and follow the detailed steps
below?
Open Constraint Manager and select the Relative Propagation Delay
Constraint
>- Select Setup > Electrical Constraint Spreadsheet?
>- Select Net > Routing > Relative Propagation Delay
Create a Pin Pair on ONE net
>- Select the net under the Objects column
>- Select the Right Mouse Button (RMB) > Create > Pin Pair?
>- Select the appropriate pin pair from each column to apply the
constraint to,
Apply > OK. The pin pair information should be displayed under the
netname in
the Spreadsheet
Create a Topology with SigXp from the Constraint Manager Spreadsheet
>- Select Tools > SigXplorer... > Topology Editor... > OK (or select
net, then
RMB > SigXplorer)
>- Set > Constraints...
>- Rel Prop Delay (tab)
>- Select the same pin pair (reference designator.pin number) in the
lower left
corner that was defined previously. Notice the From/To in the "Rule
Editing"
section is populated with these selections.
>- Scope = Global
>- Delta Type = Length
>- Delta = 0
>- Tol Type = Length
>- Tolerance = 25 (half of your requirement, +/-)
>- Fill in the "Rule Name" (Match Group name) near the top of the "Rule
Editing"
section
>- Select the "Add" button to the right of this list. Notice the rule
gets added
in the "Existing Rules" section.
>- Select the "Apply", "OK" buttons
>- Select File > Update
>- Select File > Exit
>- Answer YES to 'Do you wish Net "xyz" to reference ElectricalCset
"xyz"?'
>- Close the 'topology.log' window
Notice the pin pair information is listed twice in the Constraint
Manager
Spreadsheet, once under the Match Group name and once under the net
name. The
net name will show the Referenced Electrical CSet assigned to the net
too. You
will probably have to widen the column to the right of the "Objects"
column to
see this info.
Select the rest of the nets that you wish to assign the same pin pair
constraint to
>- Select the cell of the net just below the cell that shows the pin
pair of the
net
>- Hold down the Left Mouse Button and drag the mouse down to select
other nets
>- Right Mouse Button, Electrical CSet References...
>- Select the CSet Reference from the Pull Down; select the "OK button,
then the
"Close" button
>- You should notice the pin pairs will show up under the Match Group
name near
the top of the Spreadsheet form. The individual nets will also show the
pin pair
information along with the Referenced Electrical CSet.
________________________________
From: sathish kumar [mailto:sathish6in@xxxxxxxxxxx]
Sent: Tuesday, March 22, 2005 9:11 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] extracting X-net lengths
Hi,
Can anyone update me how to extract lengths for series terminations nets
including both before and after termination nets in electrical
constraints spreadsheet. Right now we are ahceiving it by extracting
both the before and after terminating net lengths and working with excel
worksheets to attain the total length.
I beleive there is an X-net concept in electrical constraints sheet to
acheive this easily inside the tool itself.. Let me knowif any using
this option.
Thanks in Advance...
With Sincere,
Sathish.
GDA Technologies Inc
</TB
----------------------------------------------------------- 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 please login at
//www.freelists.org. Our list name is icu-pcb-forum or go to
//www.freelists.org/archives/icu-pcb-forum/ Problems or Questions:
Send an email to icu-pcb-forum-admins@xxxxxxxxxxxxx Want to post a job
listing ? DON'T DO IT HERE! Better yet, join our jobs listing forum.
SUBSCRIBE: icu-jobs-forum-subscribe@xxxxxxxxxx POST:
icu-jobs-forum@xxxxxxxxxx
-----------------------------------------------------------
Other related posts:
