2
\$\begingroup\$

I don't understand why we need to define some sheet entries and sheet symbols in Altium with multi sheet design ?! Indeed, nets are already connected to each other by their ID from sheet to sheets as I understand or via Port. Why do we need to add on the top of this to describe Altium about sheet entries and sheet symbol architure ?

\$\endgroup\$
2
  • \$\begingroup\$ Can you be more clear what are you trying to learn that wasn't answered as part of your previous question? \$\endgroup\$ – The Photon May 14 '16 at 16:37
  • \$\begingroup\$ In the previous question I understood the different type of connector, in the current question I am asking why do we use sheets... \$\endgroup\$ – chris May 14 '16 at 17:21
3
\$\begingroup\$

Indeed, nets are already connected to each other by their ID from sheet to sheets as I understand or via Port.

This depends on the Net Identifier Scope you choose for your project.

  1. Global (Net labels and ports global)

This is the scope you refer to. Ports and net labels connect across all sheets throughout the design. This is similar to what you may know from "Eagle" layout editor and other "simple" design tools. It is not suited for a clean modular design.

  1. Flat (Only ports global) – ports connect globally across all sheets throughout the design.

This gives better control of the sheet inter-connections since you have to specify ports for signals that should go "off-sheet".

  1. Hierarchical (Sheet entry <-> port connections, power ports global)

This requires manual inter-sheet connection and usually uses a "top sheet" with only sheet symbols on it as a base. Note that power ports (12V, GND etc) are global for convenience.

  1. Strict Hierarchical (Sheet entry <-> port connections, power ports local)

This one requires you to also connect power ports between sheets. There may be two different 5V voltages in one design for example, which could be connected by accident when using the normal hierarchical design. "Strict" has the advantage that you would manually check every single connection.

\$\endgroup\$
1
2
\$\begingroup\$

To Support Reuse

...to support multi-channel design -- the reuse of sections -- either by having multiple copies of the block in one design or reusing it across multiple designs.

Global nets are generally a problem as they can lead to forgotten/unexpected connections when moving across designs or when multiple engineers work on the same design -- especially when the design is very large.

Ports objects by themselves, do not create a reusable block. They are just half of the solution. The ports manifest as ports in sheet symbols to allow you to attach nets to them.

\$\endgroup\$
0
\$\begingroup\$

Don't assume that a net label on one sheet is connected to the same net label on another sheet. Its an option in the project settings which I think is off by default. The pcb layout has no problem creating 2 distinct nets with the same name. (I speak from bitter experience)

Sheet symbols with sheet entries allow you to place functional blocks in a sheet and then show how the blocks are connected together on the top sheet which serves as a nice block diagram. It also allows channel based designs, with repeated sheet symbols which have separate inputs and outputs but the same circuitry

\$\endgroup\$
1
  • \$\begingroup\$ so you recommend to use port between sheet ? \$\endgroup\$ – chris May 18 '16 at 16:00

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