Creating a coil along a path

[JoelMckone]

I found a youtube video on how to create a coil along a path (for example - a telephone cord).  It was easy to create the part, however it took some experimenting to get a solid surface and turn of the inital sweep to remove the geometry required to create the actual coil.  The coil was inserted into an assembly (essentially a conduit for electrical wiring) without a problem.  However, when I put the assembly into a drawing file, the original geometry returns (yellow image in pdf) and the option to turn if off is greyed out.

Can this be fixed and if so how?

[SBix26]

Can you post the assembly, other components, and drawing files?  I can't replicate your results with the templates I have.

As always, it's important to let forum readers know what version of Inventor you're working with-- I found that your part file is 2024 format.

---

Sam B

Inventor Pro 2024.2 | Windows 10 Home 22H2

[johnsonshiue]

Hi! I guess the drawing view has "Associative" design view option turned on. Edit the drawing view -> uncheck the Associative. Then you should be able to make the surface bodies invisible in the shaded drawing view.

Many thanks!

[kacper.suchomski]

Are surface body views disabled in the model?
Is the visibility of surface bodies disabled in the drawing?

https://youtu.be/a7Y9wr_vfIw?feature=shared

[JoelMckone · Accepted solution]

Thanks for the tip - the 'Associative" design view was turned off, however I changed the Design View from 'default' to 'primary' which solved the problem.  It would probably been a while before I thought to check the drawing view settings as I was  focused on the making changes in the browser.

[rick_archerVPQCC]

Hi,

I have a similar thing I am trying to achieve but am struggling. I want to produce a helical sweep along the path below. This is a heater element coil. I found a Youtube that suggested creating a twisted surface and then use the edge of the surface as the path., but this was done on a circle. When I try to create the twisted surface using the below path, I get the error "the given sweep patch is not tangent continuous. To use the twist option, provide a smooth path". I have tried adding fillets between the straight lines but then get the error "The attempted operation did not produce a meaningful result". Any help would be greatly appreciated. I have added the file below. The coil size (for reference) is 6mm centre diameter and 1mm diameter wire. The pitch is not massively important, but I would like to get close to 2mm.

Thanks.

[kacper.suchomski]

Hi

I'm not at my computer, but the error seems reasonable. A 1 mm jump on such a strong fracture can create self-intersecting paths.

See what happens when you set the stroke to 5 or 10 mm.

[dan_inv09]

if the radius of your fillets is smaller than the radius of your coil (plus the radius of the wire if you get that far) then your coil can self intersect and Inventor won't do it.

I'm thinking that the straight bits run between some supports and the wire probably won't be coiled right there anyway. This picture is probably the opposite of what I'm trying to say but it's the closest picture I could find quickly:

maybe make just your straight segments coiled and then run little bit of straight wire between them

[johnsonshiue]

Hi Rick,

I believe this is a limitation in Twist Sweep. The path has to be tangent continuous. Also, as Kacper and Dan already pointed out, the rotation should not lead to self-intersection. Or the Sweep will fail to compute.

Many thanks!

[rick_archerVPQCC]

Thanks John. What does "tangent continuous" mean? Does it mean a closed path such as a circle?

[johnsonshiue]

Hi Rick,

It means the sharp corners need to be rounded.

Many thanks!