Replacing component in pcb layout

Making PCB Layouts, Manual routing, Auto-routing, Copper pouring, Updating from Schematic, Manufacturing Output
Post Reply
Message
Author
roaibrain
Posts: 8
Joined: 16 Feb 2023, 10:11

Replacing component in pcb layout

#1 Post by roaibrain » 16 Feb 2023, 10:19

I need to replace the micro usb with a usb c port in an existing pcb layout (it's 2 sided). Apart from the long way around - editing the schematic with the new component and routing the board all over again are there any more efficient methods?

Another way I tried:
- Replace component in schematic
- From pcb layout editor -> "Update layout from schematic" - "From refDes/component" (I don't get the difference and both do the same thing) => this removes the micro usb pattern from the layout and adds in the usb C pattern
- Manually route the tracks.

Is that the only way to go about it?

Thanks

Tomg
Expert
Posts: 2028
Joined: 20 Jun 2015, 07:39

Re: Replacing component in pcb layout

#2 Post by Tomg » 17 Feb 2023, 05:38

Schematic Editor
1) Replace the component, make sure all connections are where they should be and run the "ERC" verification test. If it passes, resave the schematic.

PCB Layout editor
1) Right-click on the old component and select "Unroute Traces" in the context menu. I like to do this as a precaution to help prevent the possible unrouting of non-related traces.
2) In the main menu choose File > Update Layout from Schematic > By Components... (If this brings up the "Open" dialog window, select/highlight the related schematic file and click on its [Open] button.) If the "3D Model Differences" dialog window appears, click on its [Use Schematic Models] button. Finally, if a "Warning" dialog window appears, click on its [No] button.
3) Reposition the new component as needed, rearrange any conflicting components to accommodate the new component and update the existing copper pour(s).
4) Press softkey [F12] to optimize the ratlines.
5) Finish routing to the new component. If you want to try letting DipTrace do it for you, right-click on the new component and select "Route Traces" in the context menu.
6) Clean up any other slop and update the existing copper pour(s) again.
7) Run the "DRC", "Check Net Connectivity" and "Compare to Schematic" verification tests. If they all pass, resave the PCB.

From the tutorial
"1) By components means using the hidden IDs to determine component-to-pattern links – this mode works only if the circuit was created in DipTrace Schematic. Renewing by components doesn't depend on Reference Designators, therefore, they can differ in the schematic and on the PCB."

"2) ByRefDes means that component-to-pattern links are determined only by Reference Designators. Components must have the same reference designators on the circuit board and in the schematic."
Tom

Post Reply