Suggestions for flattening coil ends

[CruftMeister]

Folks,

Has anyone come across a good way to "flatten" the ends of a coil in Fusion?  I'm looking to make the equivalent of a ground spring where the ends are planar normal to the axis of the spring.  I started with a coil made with the "coil" command and made an offset plane along the Z axis as my sketching surface, with the idea of creating a cut along the Z axis as well.

I was looking for the equivalent of the Solidworks Convert Entities command, or even Offset Entities command, but could not seem to get any of the commands in the F360 sketcher to emulate those tools.

I was able to use one of the intersection commands in the F360 sketcher to capture the spring geometry intersection with my sketch plane, but  I don't think I'm using the tool correctly as the intersection yields a purple line that isn't really a sketch entity - you can't make any geometry with it.  I was able to subsequently use the circle command to sketch on top of the outer purple intersection entity, but I would have thought the intersection tool would do that by itself. Am I missing something?

Also, I'm able to make the cut, but it leaves a little artifact of the very edge of the spring - see attached image.

Does anyone know a technically correct method to make these cuts in Fusion?  I'd like the end result to have not be fragile in case I change the coil down the road - i.e. diameter or wire size, etc.

Thanks,

Art

[I_Forge_KC]

Hey Art,

Check out this screencast.

Basically, I use a huge shape that "eats" all the geometry. It's technically bad form to leave the rectangle unconstrained, so feel free to size it as you see fit. So long as your shape (could be a circle or any shape really) is larger than your spring, you won't end up with any funky artifacts.

[TheCADWhisperer · Accepted solution]

I made a user Parameter named Height.

Try experimenting with the variable (do not make too short such that the coil self-intersects - it shouldn't fail increasing the value).

My circle is tied to the geometry.

V2 might be a bit easier for you to exercise.  (I took out the User Parameter for Height - simply edit the Coil feature parameters.)

BTW - Hot key P while in sketch is the same as Convert Entities in SolidWorks. 

I would do this part the same way in SolidWorks.

Another option is to Revolve a Rectangle for the Cylindrical intersection rather than Extrude.

I assumed you want to "grind" flats on both ends from your description.

Now, if you want a transition of the helix to a angle of torus at the ends.... 

[CruftMeister]

Hi CADWhisperer,

Wow, that was awesome - I didn't even know you could do that - I need to do some googling on the F360 intersect operation.

On question, on the sketch, which particular sketch command did you use to get your sketch? I assume it was one of the Project/Include commands?  I'm intrigued by the "p" hotkey, I will google this as well.  I like the fallback of the revolve, that is a nice alternative, and yes, I did want to grind both ends, but assumed I had to do it in 2 operations, had never seen this intersect operation you used.

Thanks for your help,

Art

[michallach81 · Accepted solution]

Hi Art, I have another way to get coil in a fast way. It's also worth watching because I use some trick with timeline that may not be obvious.

A bit of back in to the future

With my method you should be able to use Parameters:

[HughesTooling · Accepted solution]

Here's another way using boundary fill. One advantage to using planes for the cut is you can change the diameter of the coil and the trim still works.

Mark

[CruftMeister]

Hi Michal,

Thanks, that is a very interesting approach to tackling the problem.  I would  not have thought of trying that,I will definitely keep that trick in my toolbox for future use.

Art

[CruftMeister]

Hi Mark,

Hey, thanks for putting this together.  As with a lot of the other methods posted here, I've had my eyes opened to tools and approaches with which I am not familiar.  Its funny, this is closest to what I started with, two offset planes, but I never got to the second cut after the artifact showed up.  I like this method as the boundary approach takes care of both cuts in one fell swoop and as you mention, allows for non-brittle results to future changes to the coil.  Thanks.

Art

[michallach81 · Accepted solution]

Hi guys, I don't know why you think my method may not be parametric or would failed while recovering.

My method have only 3 featuers: Cylinder, OffsetFaces and Coil. The whole trick is to add OffsetFaces after Coli was made by "moving in time". In my first video I've made only one offset. I was hopping that you will understand whole idea, and know how to add UserPrameters. Of course to get siezes as you like best would be to offset both faces for half of section diameter, if so then initial Cylinder need to be size plus section diameter. We can also find proportions for right number of Revolutions. We need first to know what mean 1 Revolution when coil is cut. 1 Revolution is when bottom starts, the top would end. To check it, you can copy your coil and move it by it height. If everything is fine ends should match.

Because it would take a lot of time to explain proportion between coil heigt, section diameter and number of revolution, I've made file with all set to work. I have also short screencast. As you will see I use Pattern instead of copying, cause Pattern is parametric and Move is not. All the time both ends matches if I have full revolution.

I will also attach my file.

[CruftMeister]

Hi Michal,

Actually I'm not savvy enough to make judgments about being parametric or not, I think your method is great as well.  This one thread has shown me so many tools available in F360 that I didn't know about.  The extra explanation and file added below are very helpful as I now realize I didn't get what you did on the timeline 100% the first time through - a very clever trick with the timeline.  Thanks also for sending the file, I will upload and play.

Art