6
\$\begingroup\$

I´m new to Altium Designer. It seems like AD can´t use Off Sheet Connectors for hierarchical design, so I want to change all Off Sheet Connectors to Ports.

Is there an easy way to do this? Btw: There are a lot of Off Sheet Connectors in the design.

How can I use NetLabels in the hierarchical design? Somehow only Ports appear as Sheet Entries.

Thank you.

\$\endgroup\$

3 Answers 3

11
\$\begingroup\$

I would beg to differ with the answers posted here, but Altium absolutely has the ability to do what you're trying to do.

Because people sometimes use different names than others for the same thing, I'm just going to show a basic example, not necessarily tailored to your question, but you should be able to modify this easily to suit your needs.

The key to the solution is the Smart Paste tool.

Lets say I have a bunch of ports and I'd like to paste them onto nets of the same name. Simply select and Copy.

enter image description here

Click Edit -> Smart Paste

Here I chose paste as net labels and wires:

enter image description here

The final result:

enter image description here

As you can see from the second image, you can paste as Ports, Net Labels, even as Sheet entries where you can paste them onto a hierarchy.

This is very useful for connecting say a connector block up to a new hierarchy with a large number of nets. For example, from the same original Copied material, I pasted this onto a sheet symbol.

enter image description here

I trust you can modify this to suit your original question.

\$\endgroup\$
7
  • \$\begingroup\$ Hmm, I'm going to have to try this out tomorrow! I wish I'd known this a few months ago, it would have saved me a lot of time and effort! \$\endgroup\$
    – DerStrom8
    Commented Feb 9, 2017 at 2:31
  • \$\begingroup\$ I just tried your method on off-sheet connectors and it works very well! Thank you for sharing! \$\endgroup\$
    – Douwe66
    Commented Feb 9, 2017 at 6:58
  • \$\begingroup\$ Exactly what I was looking for, thanks Joel! Saved me a lot of time. \$\endgroup\$
    – GM18
    Commented Feb 9, 2017 at 7:58
  • \$\begingroup\$ Thumbs up from me! Works like a charm. Thanks for bringing this to my attention. I've used Altium for over two years and I still didn't even know that this "smart paste" even existed! \$\endgroup\$
    – DerStrom8
    Commented Feb 9, 2017 at 20:39
  • \$\begingroup\$ @Derstrom Sure thing. Altium seems to have everything but the kitchen sink in it. \$\endgroup\$ Commented Feb 10, 2017 at 1:53
2
\$\begingroup\$

In Altium Designer ports are used to create sheet entries. Net labels are used to connect wires and buses inside a sheet only.

The power supply symbols (GND, VDD etc) are common over multiple sheets, so you don't need to make ports for them (although you can if you want it for clarity).

I don't think you can easily change the off-sheet connectors into a port, so you need to place a new port and give it the right name.

Altium documentation states the use of off-sheet symbols only for a specific reason:

Multiple sub-sheets may be referenced by a single sheet symbol. Separate each filename by a semi-colon in the Filename field. With the effective use of off-sheet connectors placed on the sub-sheets, you can effectively spread a section of your design over multiple sheets, treated as though they were one giant (flat) sheet. Note however, that use of off-sheet connectors is only possible for sheets referenced by the same sheet symbol.

\$\endgroup\$
2
  • \$\begingroup\$ Thank you Douwe66. When I set the NetLabels for Hierarchical Design (Project-> Project Options-> Options-> NetIdentifier Scope) I still can´t use Netlabels as sheet entries. Am I missing something? Or isn´t this possible at all? \$\endgroup\$
    – GM18
    Commented Feb 8, 2017 at 12:34
  • 1
    \$\begingroup\$ If their scope is set to global, net labels do not act as ports (sheet entries) but instead simply connect all nets of the matching name across all schematics in the project. If you want a hierarchical design, however, you really should use ports, which then you place on sheet symbols. \$\endgroup\$
    – DerStrom8
    Commented Feb 8, 2017 at 14:31
0
\$\begingroup\$

If my memory serves, off-sheet connectors were really only included in Altium Designer for backwards-compatibility with older versions of the software (Protel). I generally use global net names instead.

As for changing off-sheet connectors to ports, I don't believe Altium currently has a good way to do that. I think you'd have to go through them one-by-one to replace them with ports. I ran into this a few months ago at work -- an old design used off-sheet symbols but we needed to change them to ports for use in a hierarchical schematic. We ended up having to go through and replacing them manually. It would be nice if Altium would allow the "Object Kind" to be changed in the Schematic Inspector.

EDIT: I tested Joel's answer and it works beautifully. Please disregard this answer.

\$\endgroup\$
1
  • 1
    \$\begingroup\$ @DerStrom8 See my answer above, might save you some time in the future. I had to do this once with a 440-pin ComExpress footprint and Smart Paste saved the day. :-) \$\endgroup\$ Commented Feb 8, 2017 at 23:08

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.