Can't add fillet

[Vetier.david]

Hey guys, 

New at Fusion but really loving it for 3D printing parts!

I am currently trying to design a new trim lever for my jetski. The part is pretty much finished... but I am trying to get a smooth curve on the lever so its nicer on myhands. My workflow is a bit of a mess as I am still working out how to draw more complex parts. Sometimes if something goes wrong that I don't understand, I'll use another command to fix the problem - rather than fixing it at its source - so I apologise for that.

I have been trying to add the fillet function to the edges of the lever body - but it will not accept this. I have done something wrong....

Any advice would be greatly appreciated! 

Thanks 

Dave

[HughesTooling]

The problem area is here. You can get to around 0.5mm but the the radius on the part stops you going any farther, can you make this area less pointy?

[Vetier.david]

Thankyou!!

That was so quick!

I just made it less sharp and it allowed me 2mm. If i was to try and add a round face for this, which tool would you use? As it seems like fillet can only do so much....

Thanks again

[HughesTooling]

A few quick pointers and advice.

First. Your first sketch should not be a single spline. You could probably do this all with arcs and lines, definitely everything to the right of the red line should be lines and arcs.

I don't have time to go all through the timeline, actually the timeline for this part should only be maybe 5-10 features at most. I don't think you've grasped the idea of the timeline and going back and editing features\sketch and also reusing sketches.

Up to this point you could have used just one sketch and 4-5 extrudes. You should have edited the first extrusion to change the thickness not use 2 more extrudes like this for example. First 3 sketches are pretty much the same and could have been a single sketch. Extrude lets you set the start height so the sketches don't need to be at different levels.

[HughesTooling]

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@Vetier.david wrote:

Thankyou!!

If i was to try and add a round face for this, which tool would you use? As it seems like fillet can only do so much....

Thanks again

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Fillet can do a full round but you are limited by the radii of the part you're adding the fillet too. Here's a quick example where the smallest rad is 5mm on a 10mm thick part and I can add a 5mm fillet. If the part was 11mm thick you would not be able to add a 5.5mm fillet because the 5mm rad on the part is the limit.

[HughesTooling]

Thinking a bit more about what you want, you could use sweep to create a part with a rounded profile but that could be difficult to setup.

I came up with a bit of a hack that might be a bit easier. Basically you add a 2 sided draft to the part then 2 sets of fillets to get something like this.

Screencast shows the workflow.

Mark