For my final year project im designing a piece of consumer electronics and the casing will predominantly be made up from numerous injection mouldings.
So that each component locates with other components correctly is it best to model the whole thing (casing) in pretty much in one go then split it using the ‘split’ feature in Solidworks.
Im presuming this is the way its done in industry but as i have no real world experience with such a product im not sure. Usually i start with my main component then model everything else off that in an assembly becuase that is how i was taught on my internship but that was POP/retail which hardly has the same issues.
Can anyone shed any light on designing injection moulded assesmblies using Solidworks?
You’ve got it right. build your main form then break it up into different parts using the split feature or the same cut on two parts named differently, ie case_top, case_bottom, etc. Then just go from there.
You might also want to leave a gap in the partline. We usually leave 1mm, but these are large plastic parts, consumer eectronics would probably have a more refined part line, maybe .25mm or .5mm
I generally have a surface master in a Plastic assembly file, with all of the surface information (including part ling surfaces. But I do not thicken, shell or add fillets to this part. In the same assembly I have a blank part for each injection molded part. Then I offset the main shape knit and the needed Partline surfaces for that specific part. I use the Partline surface to offset a trim surface (in my case with a 1mm gap, I offset the P/L surface at .5mm), and trim away the shape with that new offset, then trim again and thicken, shell, and detail that part.
hope that makes sense.
Then repeat on the other parts, offsetting the P/L surface the opposite direction obviously.
sorry…I can’t do a demo, I’m really busy right now.
are you constructing in solids or surfaces?
if you are constructing in solids you can disreguard most of what I explained and you’re on the right track for now.
if you are constructung in Surfaces, here’s a simpler explanation:
(imagine the final product is a 2 part assembly, top part and bottom part)
your solidworks plastic assembly would actually be 3 parts
-Surface master
this has all of the construction information but is not a solid plastic part. This part is only for your construction. -top part
this starts as a Main surface knit offset from the surface master, and is trimmed back by another surface offset, the part line surface, tehn you trim the part line surface and knit an enclosed surface volume. then this volume is thickened, shelled and detailed (bosses, fillets, bolt holes, ribs) -Bottom part
same as top part but part line offset trims back opposite (revealing your bottom surfaces. Repeat above process
You’re right… it’s very difficult to explain in words
