Can hierarchical sheets save layout time

Question

I have just read about multi-sheet design using the hierarchical approach.
This will be great for my project which involves driving 12 small dc motors with identical circuitry.

For those who are unfamiliar, basically I will have 2 a Sheet project:

One will be the schematic for 1 motor, with nice current limiting features etc.
The other will be the parent sheet, which will contain the power supply, MCU and 12 instances of the above motor sheet.

This saves me from drawing the same motor control schematic 12 times!

Not to mention, if I want to change something later on, I only have to do it once!

What I want to know is: can I push this timesaving feature into my layout design?

i.e. can I create a fully routed layout for 1 motor, and have CS automatically implement it 12 times?

I have looked through some of the documentation but so far have not seen a way of doing this.

awardautomation · Accepted Answer

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: Create the schematic using hierarchical sheets (it sounds hard but its incredibly simple) Add only 1 instance of the sub-sheet Update your pcb document and do the layout. Make it nice and tidy, right through to silk screen layout, check for errors etc. In the schematic: Add a second instance of the sub-sheet Use simple designators for the sheet instances like 1 and 2. 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" Delete the newly added components from instance 2 - not the ones you have already laid-out! 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" 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. 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 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

jimku · Answer

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

Can hierarchical sheets save layout time

Top Replies