[PCB_FORUM] Re: XNet dilemma
- From: "Macindoe, Gary" <Gary.Macindoe@xxxxxxxxxxxx>
- To: <icu-pcb-forum@xxxxxxxxxxxxx>
- Date: Wed, 6 Oct 2010 18:43:34 -0400
Thanks for the help Chris. It works by putting the voltage property on
the net either with CM or Edit -> Properties (as per Dave's suggestion).
Regards,
Gary MacIndoe
Senior PCB Layout Designer
Contract - Kelly Services
Covidien
EbD R&D
5920 Longbow Drive
Boulder, CO 80301
303.476.7458
www.covidien.com
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Shaw,
Christopher
Sent: Wednesday, October 06, 2010 4:09 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: XNet dilemma
P3V3VDC needs to have a voltage property added to it (ie value 3.3) in
the constraints manager (in the Properties->General Properties
worksheet). This will automatically exclude it from any xnet without
removing the part models.
However this should be done BEFORE any models are assigned. If the
models ARE already assigned then you need to un-assign them first, and
the voltage property, then you can add all the models again. So it's
perhaps easier just to un-assign them now, but remember for the next
design.
Chris
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Macindoe, Gary
Sent: Wednesday, October 06, 2010 4:45 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: XNet dilemma
Well, the net "P3V3VDC" is a member of the XNet "EEPROM_WP" for one
example (3.3V & EEPROM write protect?).
I don't think there is a reason to have xnets setup at all.
I like to put the property Ratsnest_Schedule = Power_And_Ground on my
power and gnd nets so that the rats look like this:
Instead of the rats going all over the place (yeah, I don't like filled
pads either!).
Regards,
Gary MacIndoe
Senior PCB Layout Designer
Contract - Kelly Services
Covidien
EbD R&D
5920 Longbow Drive
Boulder, CO 80301
303.476.7458
www.covidien.com
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Shaw,
Christopher
Sent: Wednesday, October 06, 2010 3:28 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: XNet dilemma
But what do you mean exactly by 'should not be there'?
Chris
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Dave Seymour
Sent: Wednesday, October 06, 2010 4:25 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: XNet dilemma
Edit> Properties (find filter set to Comps) > No_Xnet_Connection
Or
Specifically, remove the model from the component.
Analyze > Model Assignment > Select the part and clear the model. ( this
will come back if you reassign all models or auto assign)
Hope this helps.
Dave
Dave Seymour
Ixia
www.ixiacom.com
919.267.4840
________________________________
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Macindoe, Gary
Sent: Wednesday, October 06, 2010 5:17 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] XNet dilemma
Hey guys,
I have some XNets in my design that should not be there.
I asked the DE and he said that he didn't add them in the schematic (he
doesn't even know about them).
Does anyone know if there is a way to remove them in Allegro?
Thanks for any help.
Regards,
Gary MacIndoe
Senior PCB Layout Designer
Contract - Kelly Services
Covidien
EbD R&D
5920 Longbow Drive
Boulder, CO 80301
303.476.7458
www.covidien.com
Other related posts:
