Nets not connected between pages

Drawing Schematics, Hierarchical Design, BOM, Exporting net-lists, etc.
Post Reply
Message
Author
barrygrae
Posts: 3
Joined: 24 Jun 2010, 14:51

Nets not connected between pages

#1 Post by barrygrae » 24 Jun 2010, 14:58

Hello,

First I enjoy using the product...

But can someone tell me the best way to ensure that nets are connected in a multipage schematic?

I am using netports (VDD) from the Dsc_Sch and renaming them as needed (ie: OUT12). When I do this they are not connected automatically on the other pages. I have to select the net on each page and use net properties, name, connect by nets, connect by pins and apply to "net" to egt it to work in DIP PCB. There must be a better way.

Regards, Barry

Alex
Technical Support
Posts: 3131
Joined: 14 Jun 2010, 06:43

Re: Nets not connected between pages

#2 Post by Alex » 25 Jun 2010, 05:30

Make sure that netports have the same type.
Wires on different sheets are joined to single net if they connected to same type of netports.

1DOST
Posts: 3
Joined: 07 Jul 2010, 03:37

Re: Nets not connected between pages

#3 Post by 1DOST » 07 Jul 2010, 03:41

I want to connect only one net between different schematics. How can do this? I tried place page connector but it is for bus. Please more information about this situation.

Alex
Technical Support
Posts: 3131
Joined: 14 Jun 2010, 06:43

Re: Nets not connected between pages

#4 Post by Alex » 07 Jul 2010, 05:00

Use net ports or connect nets by name.
The easier way is assign the same name for nets on different sheets. "Connect nets by name" option in net properties should be activated.

rick.curl
Expert
Posts: 137
Joined: 14 Jun 2010, 16:46

Re: Nets not connected between pages

#5 Post by rick.curl » 08 Jul 2010, 08:03

I made a request a while back to add a feature like a page connector, but for a single net. For me, this would be TREMENDOUSLY helpful.

As coincidence would have it, I just got a batch of boards in yesterday where I had forgotten to rename one of the nets so it would connect between pages. Since there was no way to see it on the schematic (unless I went in an looked at each of the 75+ nets individually), this one slipped past me - so these boards will go in the trash.

-Rick

barrygrae
Posts: 3
Joined: 24 Jun 2010, 14:51

Re: Nets not connected between pages

#6 Post by barrygrae » 08 Oct 2010, 11:15

It is more complicated than described above. FYI, if netnames are used they will "jump" to a page-connector (made from a +12V in example) and then when that connector is copied to be used elswhere it will impose that netname on the new net. Not good.

ONLY SOLUTION FOR FOOLPROOF USE IS: Do not use netnames (for general use). Make your own page connector/per project, Copy +12V from discrete schematic, click on the lead and set pin properties (it will have power attributes when you copied it from +12V). Set as follows, type=none, electrical=undefined, name and number=1, properties and name font=single pin. Set component properties as such, value= ,type=A.

Then copy these as need in your schematic and rename (right-click) to your prefered name. If you right click for properties you will see type=A. If you right click to rename you will see "connector name"=A. Not sure which is which but I use the one at the top of the right-click list.

DO NOT mix netnames and off page connectors or you can end up with big problems that hopefully you will find before your boards arrive.

I hope this helps someone out there as it took a while to find a solution on my end.

Barry / GRAE LLC

-- 08 Oct 2010, 08:24 --

It is more complicated than described above. FYI, if netnames are used they will "jump" to a page-connector (made from a +12V in example) and then when that connector is copied to be used elswhere it will impose that netname on the new net. Not good.

ONLY SOLUTION FOR FOOLPROOF USE IS: Do not use netnames (for general use). Make your own page connector/per project, Copy +12V from discrete schematic, click on the lead and set pin properties (it will have power attributes when you copied it from +12V). Set as follows, type=none, electrical=undefined, name and number=1, properties and name font=single pin. Set component properties as such, value= ,type=A.

Then copy these as need in your schematic and rename (right-click) to your prefered name. If you right click for properties you will see type=A. If you right click to rename you will see "connector name"=A. Not sure which is which but I use the one at the top of the right-click list.

DO NOT mix netnames and off page connectors or you can end up with big problems that hopefully you will find before your boards arrive.

I hope this helps someone out there as it took a while to find a solution on my end.

Barry / GRAE LLC

-- 08 Oct 2010, 08:27 --

sorry for the double post.

novarm44
Technical Support
Posts: 312
Joined: 09 Jun 2010, 06:24
Contact:

Re: Nets not connected between pages

#7 Post by novarm44 » 09 Oct 2010, 04:03

I made a request a while back to add a feature like a page connector, but for a single net. For me, this would be TREMENDOUSLY helpful.
Use net-ports - it works in the same way as page connectors but for nets.
As coincidence would have it, I just got a batch of boards in yesterday where I had forgotten to rename one of the nets so it would connect between pages. Since there was no way to see it on the schematic (unless I went in an looked at each of the 75+ nets individually), this one slipped past me - so these boards will go in the trash.
You can check your nets via net-list or design manager or connection manager (what is preferred for you). Personally I do not recommend to use connection by names as sometime this cause problems, however many customers like this feature.

rick.curl
Expert
Posts: 137
Joined: 14 Jun 2010, 16:46

Re: Nets not connected between pages

#8 Post by rick.curl » 30 Nov 2010, 18:30

novarm44 wrote:Use net-ports - it works in the same way as page connectors but for nets.
Maybe I'm missing something here- In order to use Net ports I will have to create one in a library for each wire that I want to connect between pages-right? This seems to be very cumbersome, and I will end up with libraries cluttered with net ports that I will only use once or twice.
novarm44 wrote:You can check your nets via net-list or design manager or connection manager (what is preferred for you). Personally I do not recommend to use connection by names as sometime this cause problems, however many customers like this feature.
I know I can do it this way, but the way a page connector turns green when it is connected to another page is really neat! It makes it so quick and easy to tell at a glance what is connected and what is not while I am still looking at the schematic.

-Rick

Alex
Technical Support
Posts: 3131
Joined: 14 Jun 2010, 06:43

Re: Nets not connected between pages

#9 Post by Alex » 01 Dec 2010, 10:07

Nick,

you can create single net-port in library, then place net-pots on schematic and rename their types as you want. It is not necessary to create net-port for each net.

Post Reply