How do I add a fillet to a sweep?

[Will1337]

So I am learning different commands and tools in fusion 360 and I stumbled into a problem. I cannot seem to add a fillet to a sweep. The idea was to design a custom screw and nut, I have started out very basic but when I tried to smooth the edge of my "coil" I ran into trouble. I am not brand new to fusion, but I am definitely still learning.

If the problem is with my design or the way I am going about it please let me know.

I need to learn more about sketches and all the functions that that entails so maybe thats my problem? maybe a constraint in the sketch I am sweeping???

on another note: If there is a good tutorial or tutorial series on the sketch tool palette please let me know, I dont think I fully understand how to use it all

- Thanks

[MoshiurRashid · Accepted solution]

Hi

Thanks for posting. I've made your coil smooth by sketch filleting the profile. My suggestion is, if you can do it in sketch, don't bother to use any more feature for another operation.

Reason why it was not filleting the solid sweep: As you can see in the picture, the coil is divided in several pieces. Here, the faces are different. This happened because, your profile was too big than the pitch of the coil. Also can be more reasons in there. But, I suggest you to fillet it in the sketch and that makes life easy.

 

[Will1337]

Thanks, is there a way to add more sections uniformly? I mean without individually splitting each face with a construction plane or something similar. Would this allow me to fillet the edge? Now I'm just curious

[MoshiurRashid]

You're welcome.

Yes. If you get a continued face, it may let you filet the corner. But, also, it depends on the geometry.  

[MoshiurRashid · Accepted solution]

Here is a screencast for you which shows the difference between 1 face and many face impact.

https://autode.sk/2UjUR8h

Another thing, create the springs and coils by coil command. Don't use sweep for this case. I personally suggest this.

Why? It is in the screencast. 🙂 

[Will1337]

Thank you very much, I was wondering why there were so many faces. I had watched a tutorial about making custom threads this way, that's why I wasn't using the coil command, and instead using the sweep path and guide rail. your screen cast helps so much, thank you again.

[MoshiurRashid]

You're welcome. Feel free to post any issue you're facing. We are here to help. 🙂

[HughesTooling · Accepted solution]

Part of your problem is to create a nice clean sweep the sketch should be perpendicular to the path(Helix). Use plane along path then create the sketch on the plane like this.

Then create a line along the centre of the coil in another sketch to use as the path in the sweep. This will create a clean solid without all the segmentation.

Then you can fillet and end up with a lot nicer solid made from just 10 surfaces.

File's attached.

Mark

[HughesTooling]

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@MoshiurRashid wrote:

Hi

 My suggestion is, if you can do it in sketch, don't bother to use any more feature for another operation.

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This generally is not good advice, if at all possible keep sketches as simple as you can. Of course if you need a fillet in a sketch to aid construction or as a visual aid then use one but Fusion's sketch solver can get bogged down if you put too much info in a sketch.

Adding fillets to the solid will help overall performance and best advice is add fillets as late as possible in the design. Combines, Extrudes, etc. that join or cut a solid will work better on simple geometry, so add the fillets at the end of the design if you can.

Mark

[HughesTooling · Accepted solution]

Here is a problem you had in your design and also a problem you'll get with the coil feature. Because the section of the coil is created parallel to the helix axis the cross section is not 2mm.

If you measure between faces you get 1.942mm, this will get worse the steeper the helix angle.

Using the method where the sketch is perpendicular to the helix you get the correct cross section.

Mark

[MoshiurRashid]

I suggested this because, I thought the sketch profile of him was ment to be in that plane, in that size.

Thanks for elaborating the topic more and adding more resources.

[Will1337]

I always try to add any chamfer's or fillets at the end to sort of polish up the design, this is when i ran into the trouble. Thanks for all the help!