Fusion Electronics
Working an electronics project and need help with the schematic, the PCB, or making your components? Join the discussion as our community of electronic design specialists and industry experts provide you their insight and best practices.
Showing results for 
Show  only  | Search instead for 
Did you mean: 

How to model a cutout at the edge of a PCB?

Message 1 of 5
130 Views, 4 Replies

How to model a cutout at the edge of a PCB?

I am new to Fusion Electronics and trying to design a pcb with some edge mounted components like switches (EVQ-P4). I want the switches to sit at the edge of the PCB so that the button part actually sticks a bit out. After some fumbling with the footprint I modelled a cutout which follows the spec. The cutout is modelled on layer "46 Milling". When I place the component somewhere on the PCB, the 3D model shows the cutout correctly. But when I place the component directly at the edge, the cutout is ignored.


Is there a way to get cutouts to work when they intersect the board edge?

As a workaround I can place the component a tiny bit off the edge. But that leaves a tiny wall of material. So this is not a good solution.





Component placed exactly at the edge of the board - no cutout

component placed exactly on the edge - no cutoutcomponent placed exactly on the edge - no cutout


Component placed somewhere on the board - cutout works

component placed somewhere on the board - cutout visiblecomponent placed somewhere on the board - cutout visible





Labels (1)
Message 2 of 5

I was able to reproduce this. It seems like a limitation of the system where the board shape interpreter gets confused because it can no longer find a continuous path with the milling shape on it's outline. Definitely something we can and should fix at some point.


As a workaround, you can move the shape in your component to the dimension layer (group select the lines & use the inspector to change the layer). You also will want to leave it 'open'. Then you can connect the board shape in your PCB to this open shape, the inferencing should make this relatively straightforward. Not ideal but it should get you there for now. The idea is really that there is one unambiguous path that defines the board shape. 


Screenshot 2024-02-11 at 1.28.19 PM.pngScreenshot 2024-02-11 at 1.00.39 PM.png

Pieter-Jan Van de Maele
Senior Engineering Manager, Fusion Electronics
Message 3 of 5

Thanks for your quick help! 


To test your workaround I made a simple component. Once initially placed it worked most of the time. But as soon as you move the component the whole system breaks. I am not able to connect the board outline to the component’s lines on layer 20 (Dimensions/BoardOutline). Even when the line overlap the shape inference doesn’t work.


In my original component I already had the cutout on layer 20 (Dimensions/BoardOutline). But since the component needs to be at a special coordinate the system doesn’t seem to be able to infer the board shape. I hope that this bug will be fixed very soon.

Message 4 of 5
in reply to: raywoSZTV2

Hi @raywoSZTV2,


I hope you're doing well.'s workaround is the currently accepted solution. The trick here is that no overlap is allowed. You have to draw the cutout on the dimension layer in the library. In the 2D PCB you have to connect the board outline exactly at the endpoints of the cutout, an overlap will not work. So leave the endpoints of the cutout in the library on a convenient grid.


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


Best Regards, 

Jorge Garcia
​Product Support Specialist for Fusion 360 and EAGLE

Kudos are much appreciated if the information I have shared is helpful to you and/or others.

Did this resolve your issue? Please accept it "As a Solution" so others may benefit from it.
Message 5 of 5
in reply to: jorge_garcia2

Hi @jorge_garcia2,


thanks for the follow up! Indeed it is most important to end the lines on a grid position or else the inference will fail. When doing so, the inference works. But I hope you realise that that is not possible every time and in every design. In my case I had to fiddle quite a bit to make it work. Even the slightest change in the design can break this as it is not very robust. That’s why I hope that this is seen as a bug and will be fixed soon. 


For now I know what to do and go on with designing my PCB. 🙂 

Thanks for your help!

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report