Autodesk Fusion - modelling a Brake lever?

[Lacathedrale]

I am building up a model of an SR Dia. 1427 van for use in G1 - it's going pretty well, but the one thing which is flummoxing me is the brake lever handle. I know how it needs to look in plan and in profile, but I can't seem to figure out the order of operations to have it follow both - the following image shows the problem - it needs to joggle around the axleboxes by about 9mm:

 

 

At this stage I'm considering just printing it in the flat and then bending it to shape with hot water - but I've seen lots of other brake gear designs which model the shoes, hangers, rods, lever, ratchet block all as a single insert that pops in behind the solebar and I would really like to mimick that if I can.

 

I would normally consider using Loft, but the multiple profiles (and joggle) is in one axis while the path is in another, and the route between them seems anything but straightforward!

[Skinnylinny]

Personally, what I do in that situation is create two sketches - one from above and one from the side. I then extrude the side view overlength (over-thickness? So that it extends beyond the furthest in and furthest out points of the lever) as one body.

Next, I extrude the top view downwards through the previous body (again as a new body). I split the first body, using the second body as the splitting tool. Remove un-needed bodies, and you should have a brake lever that bends in multiple directions at once!

[TM2201A]

Brake levers are quite a challenge as they can't usually be drawn using the basic 3 planes that the CAD system initially presents you with and you've got the fun of forcing the Loft/Sweep/Variable Section sweep system to create solid parts reliably (oh the fun we had with Ideas and ProEngineer).

 

I'd start off getting solid bodies on to known planes ( in this case vertical) so that's the drive boss at the v hanger end and the handle end of the lever. Then create further reference planes (constrained by centre lines or dimensions from the solid bodies) into which centre lines for thin features or sweep/loft paths and profiles can be drawn. Once the basic 3D bent bar has been created then go through and do cutting operations to get any tapered profile, Morton cam details, etc. Finally add rounds/fillets, chamfers and any drafting required to make the part look cosmetically correct/improve printability.

[Quarryscapes]

2 options: 1) do as suggested above, create a top view of the lever with the bends, and a side view, extrude one then the other as a boolean intersect and job done. 

2) create the lever as sheet metal and develop that way. A lot more convoluted for a printed lever, but if you ever wanted to do an etched one this would be the way to go. 

[Lacathedrale]

Thank you all, I'll have to look up the intersect tool!

 

[Arun Sharma]

The other way is to forget about additive manufacture and 3D CAD sculpt it from a drawn solid block

[Quarryscapes]

Sorry I'm at work without a screen recorder, but this should make it clear enough the intersect method:

 

Start with the side profile:

 

Then add a top view:

 

Extrude one of the profiles:

Then the other using the intersect option from the operation drop down:

 

et voila

 

[12A Models]

On 23/04/2024 at 10:16, Skinnylinny said:

Personally, what I do in that situation is create two sketches - one from above and one from the side. I then extrude the side view overlength (over-thickness? So that it extends beyond the furthest in and furthest out points of the lever) as one body.

Next, I extrude the top view downwards through the previous body (again as a new body). I split the first body, using the second body as the splitting tool. Remove un-needed bodies, and you should have a brake lever that bends in multiple directions at once!

 

Exactly how I would tackle it too!