How to combine Electronics Designs?

[bostonK74CU]

I am having a rough time trying to combine two Schematics/PCB's I have been working on at work. They were going to be separate boards but we have more space than expected and we decided to put it all on the same board, I just need to "copy/paste" them together with some minor edits. Panelizing them is not acceptable as they need traces going from one to another (which were previously terminal blocks and wires.) 

Copy/pasting the components from one schematic to another "works," but then I'll have to redo the layout of all those components on the PCB, which is obviously unideal. After some googling, I have tried creating a separate Electronics Design, create a new PCB, copy/paste the layouts from both into it, then link it to a schematic with their schematics on different sheets. This should work, expect I get the error "Schematic/PCB sync deactivated: Run ERC to find differences and resolve them." Clicking on this shows the "ERC Errors" window (attached), and clicking on Synchronizer, then Run, also yields no results, just removes half of the traces. 

Any help would be much appreciated. Thanks. 

[jesper8W75R]

My guess is that you could use Design Blocks to do this.
I haven't tried this feature, but it might solve your problem.
I think you could make one of the designs a design block, then pop it into the other design.

[jorge_garcia]

Hi @bostonK74CU ,

I hope you're doing well. In the latest release of Fusion 360 there is a feature called insert Schematic that is related to Designblocks. Make sure both your schematic and board are open and then try this feature to insert one design into the other.

Let me know if there's anything else I can do for you.

Best Regards,

[m.neujahr_at_moe]

Hello @bostonK74CU,

as you can see in the ERC-Dialog, al lot of parts are connected to the "wrong" net.

You can solve this by renaming the nets "GND1", "3.3V1" and so on to the desired net-name.

You can do this in schematic or in layout.
Try to identify net "GND1" and change its name to "GND". The next "ERC" schould show less errors.

Some earlier days, the "ERC" generated a text-file, where you found all ERC-errors, so someone would be able to solve the ERC-errors step by step with the text-file.

No fear, if you do this step by step, your problem can be solved in only a few minutes.

I think this way is much easier than generating design blocks.

[bostonK74CU]

@m.neujahr_at_moe 

I tried that, and it seems that the ERC is adding the "1" to the end of GND by itself. On both sheets the value for the GNDx symbols read "GND." However, in the ERC dialog box is shows GND for sheet 1 and GND1 for sheet 2. Very odd. 

[bostonK74CU]

@jesper8W75R, @jorge_garcia 

Yes, looks like that should work, except do you know how to save Design Blocks? I can see the "Insert Design Block" option on the Schematic and PCB tabs, but no way to create one. Everything I can find says that Design Blocks are not functional in Fusion yet, although most of that is from 2020. A bit frustrating how hard it is to find documentation about this. The Fusion 360 documentation lists the Design Block functionality in the Features, but I can find no info on how to implement it. 

Edit: Figured it out! Method is convoluted and poorly documented, but using Design Blocks works. Summary written below. 

[bostonK74CU]

@jorge_garcia 

Tried that. Has the same effect of copy/pasting the components from one schematic to another. Components are transferred to the schematic successfully, but the PCB layout is not. 

[bostonK74CU · Accepted solution]

Okay, I figured it out. Design Blocks work (they are functional in Fusion, despite what the forum thread says.) What you do is go to the schematic/PCB (either work) you want to import, write "write dbl" into the command line at the top of the screen. Save-as the design to a place locally (cloud is not an option.) Then go into the schematic you want to insert the original, then Design: Place: Insert Design Block: Select from my computer. Select the .dbl file you saved locally. Place the block of components. The PCB layout will be preserved. Just move them where you'd like, then delete the old border. 

[peter]

Thank you Boston. I have been trying to work out how to create a design block.

I had no idea it was a command line to save.

[giladk]

This doesn't work (might have working in the past)

You can open the dialog by writing "write dbl" but no files are being actually saved.

[jorge_garcia]

Hi @giladk,

As reported on the other thread, the recommend solution no is to use the Insert Electronic design command. Both the schematic and layout come in. Please let me know if you are not seeing the layout come in. In order for the layout to come in, there needs to be a 2D PCB open together with the schematic.

Let me know if there's anything else I can do for you.

Best Regards,

[giladk]

Hi Jorge.

This works but this is copy-paste.

When I change the original it does not propagate down.

This feature is just half baked, more like 25% baked...

Gilad

[jorge_garcia]

Hi @giladk,

Designblocks didn't propagate either, so we have parity. I agree that it would be very useful if these circuit blocks could be treated just as components and have them update and propagate changes, but we've never had that. This would be net new functionality. I'll pass your comments along to our team to include that in the sub-circuits work that's being done.

Let me know if there's anything else I can do for you.

Best Regards,

[mjstn2011]

Adding my inputs to better clarify the Insert Electronic Design workflow which I am using with success.  I hope this helps people new to this need.

Lets call the full design desired to be inserted into other designs  'SrcDesign'.  This is a full schematic and even complex pcb layout to be used more than once.

Lets call the larger design 'TargetDesign' as it needs 1 or more of the full SrcDesigns in it that were formed in Fusion 360 Electroncs.  

This flow is needed because as of Jan 2025 design blocks cannot be created in Fusion 360 and only can form in Eagle (Im not discussing design blocks here).

Im going to keep my SrcDesign so it fits on one schematic sheet as I don't know what 'evils' happen for inserting a multi-sheet SrcDesign.

• Open  SrcDesign and open TargetDesign so there are tabs for them open on top.
• Select TargetDesign schematic.   In sheet view use 'New' to create a new Sheet that has nothing at all in the sheet yet but is open now (blank)
• In Design mode in the TargetDesign use  Place then 'Insert Electronic Design'.  Window comes up showing SrcDesign so highlight that and use Select button
• A window will come up with all nets in SrcDesign in the 'Old name' column and the New Names to be used.  Here you will want to change nets in the New name column that must be unique to this new inserted block of schematic/pcb layout.  So maybe you had PWR_OUT well not for New Name click name and say PWR2_OUT for example.   This is important or you can have a royal mess separating nets after you hit OK in this window.
• After OK the new schematic sheet may need to be positioned in this new home for this schematic sheet. If a frame, put the frame at origin perhaps.
• Now use  Switch - Switch to PCB Document.  The ENTIRE board with edge cuts and mounting holes and everything will be in lower left.   So in my case I removed the edge cuts and mounting holes I had in SrcDesign and main silkscreen for name of circuit.  Then use a Move:Group to move the entire new layout section where it needs to be on TargetDesign.

I hope this is helpful even though it is more wordy.  I had to play around to figure this workflow out from the earlier very brief blanket terms used.