Can hierarchical sheets save layout time

I was given a live demo of the full version of Altium Designer a few years back and I remember them showing us the "Snippets" feature of Designer.  This allowed you to save small sections of schematics and layouts and I believe they could be somehow linked together to allow you to then place a schematic section and the appropriate layout for that into a new design.  But I do not believe this feature is included in Circuit Studio.  I agree this would be a big time saver!

I imagine someone on the forums here has found a workaround that probably isn't quite as easy as the Altium Designer method, but will probably do much the same as you are talking about.  Perhaps it is a matter of creating a small layout project and then copying from that open project into your new one???

Yes I think snippets were/are a way to do this in AD.  You can search for how to use them in the Altium Designer technical notes.  Also, in AD (as in the older Protel) you could cut and paste routing from one routed section and then easily change the net names to no name.  Then you could commit the free primitives to a new net name such as from the pads of parts.  I haven't tried this with CS yet.  What you are talking about is an advanced feature (IMHO); its just a guess, but I suspect CS has this crippled so as to get a distinction between full AD and CS.

You might make a test project and try copy/paste some routing from one block to another.  I'm thinking it would result in some rule violations due to net name mismatches.  If you are lucky it might allow these to be updated to take the new net names or perhaps you can do something like select all connected copper and then update the net names.

An easier option might be to make a component with a footprint that includes the layout and all the parts you want. Then just move it around and place it like you would an IC.

I have received feedback from CS development.

While the sheet entry is big time saver for schematics, there is no automatic way to propagate this through to the layout.
I did find a workaround:

1. Create the schematic using hierarchical sheets (it sounds hard but its incredibly simple)
2. Add only 1 instance of the sub-sheet
3. Update your pcb document and do the layout. Make it nice and tidy, right through to silk screen layout, check for errors etc.
4. In the schematic: Add a second instance of the sub-sheet
   • Use simple designators for the sheet instances like 1 and 2.
5. Update the PCB.
   • This will change the names of all the components in the completed layout by appending an underscore and the sheet symbol designator you used in the schematic. eg. "R7" -> "R7_1"
   • It will also add the components represented in the 2nd instance of the sub-sheet, (with the appropriate suffix) in a straight line, off the sheet as normal. eg. "R7_2"
6. Delete the newly added components from instance 2 - not the ones you have already laid-out!
7. Copy and paste the nicely laid-out 1st instance, include all components, nets, vias etc.
   • When the components are pasted, the names will automatically have "_1" appended. eg. the copy of "R7_1" will be named "R7_1_1"
8. Use the Component Links to link the unmatched schematic names to the new pcb names you copy and pasted. eg. "R7_2"  matches with "R7_1_1"
   • from PCB editor Ribbon -> Tools -> PCB Links -> Component Links
   • if you have only "designator" ticked at the bottom, they will automatically match based on the first letters. I was able to click click click them across to the matched column without changing anything.
9. Go back to the schematic and "Update PCB document" like normal.
   • This will change the names of the pasted components (and their nets) in the PCB to reflect the names used in the schematic
10. To add subsequent sheets, do them one at a time. You only need to repeat step 4, 7,8,9
    • Steps 5 and 6 are only necessary to force instance 1 to use the underscore-designator naming convention, so that when you come to step 8, you have only one set of components to match

It seems like a lot of steps but its actually easy, and saved me a lot of time!

When copy and pasting a selection of components:

• Drag a selection box around what you want to copy
• Hit ctrl-C,
• Click somewhere in the selection where you want the origin of the copy to be (like the centre of a terminal pad or header pin that needs to be in a specific place)
• Hit ctrl-V
• Click somewhere in black board space where the new origin should be. The new parts will be pasted with the origin where you clicked

This sounds very similar to multichannel layouts. You might be interested in a Youtube  video titled "CircuitStudio - Dealing with Multichannel Layouts" by harvie256.

Link:

https://youtu.be/1VOOqheRauU