[PCB_FORUM] Re: extracting X-net lengths
- From: "Dennis Nagle" <den@xxxxxxxxxxx>
- To: <icu-pcb-forum@xxxxxxxxxxxxx>
- Date: Wed, 23 Mar 2005 12:11:36 -0500
CM is set up so it will only report Actuals for those Objects (pin
pairs, (X)nets) that are constrained - that's where that long list of
steps came from. There is, however, one worksheet in CM that will
populate with results without any constraints - Total Etch Length (TEL).
If you turn on the TEL DRC mode, and select Analyze for the design, you
will get Actuals reported for all Xnets. Downside here is that it will
only report a number for the entire Xnet. You can use the Etch Length by
Layer (or Pin Pair) reports to get the lengths of the subnets.
-Dennis Nagle
Cadence
________________________________
From: Andrew Noonan [mailto:andrew@xxxxxxxxxxx]
Sent: Wednesday, March 23, 2005 11:36 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: extracting X-net lengths
Good Lord, Cadence. All this just to get an Xnets length
report?????
I'm not normally a complainer but this is outrageous!!
-----Original Message-----
From: Reade, Sue [mailto:Sue.Reade@xxxxxxxxxxx]
Sent: Wednesday, March 23, 2005 6:40 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: extracting X-net lengths
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:
