Workflow suggestions for inserting PCBs in design

[eu-accounts]

Hi everyone!

I am working on a production and testing jig for an electronics project. The main idea is that there is a top board in which PCBs slot into. To get a general idea of what I am talking about, look at an image of the design at the bottom of the post. The thing I can't wrap my head around is what kind of workflow to use to design such a thing, so that it can be easily modified without messing up the whole design. There are two ways which come to mind: insert a 3D model of the PCB, try and align it manually roughly where I would want it, project the outline of the PCB in a sketch, add an offset for the outline to include some tolerance and then cut out the outline from the mounting block. This seems like a rather messy approach, plus it means I have to do a lot of eyeballing in terms of alignment. Modifying the PCB design usually breaks a lot of the design as well.
The second approach I see is to generate a dxf file from the PCB CAD, insert that as a sketch, use it to make my cuts and then use a rigid joint to insert the PCB in the cutout. This seems to be a bit better but it also means I have to fully constrain the PCB outline in a sketch in order to constrain its location without messing up its outline because as far as I can tell, fusion 360 has no sketch blocks. For more complicated outlines this makes the sketch a total mess and is therefore also undesirable. Ideally I would just have a dxf import behave as a single entity in a sketch that is fully constrained against itself but its absolute location can be set using constraints.

I've used both workflows in my designs previously it wasn't very fun to say the least, so I'm thinking there has got to be a better way to get this done.

I'd appreciate any input from you folks on the best approach for this so that I can stop tearing my hair out any time I have to modify either the PCB or the jig design.

[chrisplyler · Accepted solution]

I'm gonna say...uh...maybe...

...Whatever Component requires the cutout...make a new Component nested inside of that Component...rename that new, nested Component something like "PCB Cutout" and create the sketch w/ outline and offset inside that new, nested component. Don't create any Bodies in there, just use that Component as a "container" for the sketch.

Now you can make copies of that Component (including the sketch inside of it of course), either linked copies that will always be the same no matter what changes you make to the original OR an UN-linked copy which you can edit to create different offset values or whatever. You will be able to Joint these empty (except for the sketch) Component(s) wherever you like, and then use those sketches to extrude/cut into other Components.

[eu-accounts]

Getting a little closer to where I would want this to lead to, but there was one thing I was unable to do with this approach: align components. Say I have a connector on PCB1 and that same connector on PCB2 and I want those PCB be aligned in a way in which the connectors are facing each other. If the outlines were both just a blocks in a single sketch, then I could just draw a line between the centers of the connectors and and apply the Parallel/Horizontal constraint and be done with it. Is it only possible to use the move command with your approach or is there a way in which to use constraints to align such sketch components?

[chrisplyler]

Use the Joint system in F350 to position two Components (including the sketches they contain) relative to each other as desired.

[etfrench]

You can also create joint origins if there aren't any suitable existing.  In your example, create joint origins at the center of each connector, then create a rigid joint between them.  Set the appropriate offset distances.

[chrisplyler]

---

@etfrench wrote:

You can also create joint origins if there aren't any suitable existing.  In your example, create joint origins at the center of each connector, then create a rigid joint between them.  Set the appropriate offset distances.

---

I'm sure you could pick an inside corner of the front face of the female side, and an outside corner of the front face of the male side, and then give a Z offset representing how far you want the ends pushed into each other. Joint Origins are valuable, but don't make things more complicated if you don't have to.