Wrapping a drawing around a cylinder/surface

[Anonymous]

I'm working on a complicated design. The lower half has a curve to it (see that shows the profile)

The drawing however has slots that need to be cut into that curve, but not straight through, basically properly wrapped. Is there an easy way to do this?  right now I'm considering creating a temporary cylinder, figuring where they should go, creating a tangent construction face, and then redrawing them on that (first the one row, then the other. But there must be something easier.

Anyone can help would be much appreciated.

[TrippyLighting]

"Properly wrapped" equates to "in direction of the surface normal".

You should be able to put a tangent construction plane directly onto that curved surface without the need for an additional cylinder.

[Bertho_Boman]

My question "How to model a circular cam with a perpendicular edge" is closely related to your request so hopefully someone will describe the wrapping procedure.

[ahreum.ryu]

noHi @Bertho_Boman, 

Thank you for posting! 

I think it would be possible if we use "Sheet metal". unfortunately Fusion 360 is not supporting yet (it will be launched soon).

As of now, we would use workarounds. 

1. As saying @TrippyLighting "You should be able to put a tangent construction plane directly onto that curved surface without the need for an additional cylinder. " 

2. Split surface along with your sketch and use press pull function. but I'm not sure this way is easy... I'm sharing my idea if I missed something please let me know. 

Many thanks

[halfmoonmods]

So this was a great thread.   Learned a couple of things for sure.  However, what if one wanted to model a slot wrapped around a cylinder?  This method works on the small scale but if you wanted it to go say 3/4 of the way around a cylinder then this method falls apart real quick. 

Does anyone have a solution to this?

[Bertho_Boman]

My question: "How to model a circular cam with a perpendicular edge" is basically the same problem as yours.

Look at the replies there.

Basically the feature will be in "Sheet Metal" which is not released yet.

Bertho

[TrippyLighting]

@halfmoonmods

Please create your own thread, share your design and maybe make a screencast where you encounter the problem.

[Anonymous]

I went into sketch mode and used the Project/Include 3D Geometry function and selected the edges of the face that you can see the straight blue lines attached to.

I then used the break link command and turned the two straight edges and the radius edge into independent curves.

Once that was done I moved the radius curve into a position along the face and copied that curve twice and the copies into new positions, I then used the Pattern on a Path to pattern the shapes.

I have left the last pattern in the screen shot so you can see how it works out.

[Anonymous]

I'm not sure I understand this solution. Could you post a screencast? (I know it's a hassle. Sorry)

[Anonymous]

I did try this... but getting them the correct distance was difficult, to say the least. Yes, it does equate to 'in the direction of surface normal'. 🙂

Thanks

[Anonymous]

I don't think I'll get the proper slot shape this way. Since they're equally spaced (and clearly so in the final product) I'm a little concerned about that.

Please, when "sheet metal" comes out, I hope you call it "wrapping a sketch to a shape" and it goes under Project. This is hardly limited to sheet metal. 🙂

[Anonymous]

You can maintain whatever spacing you like in both directions.

When copying and moving the radius curve you have control over the length along the face spacing and when copying the object along the radius curve you have control over the vertical spacing

[TrippyLighting]

Very nice solution!

[Anonymous]

Solution I ended up using.

So, what I ended up doing was

- Creating a single plane that was target to the first of the bottom two rows of vents

- creating a drawing on that plain

- projected in the two points for the center of the slot circles

- using the slot that semi overlapped the curve (only a small amount was off) and then extruded it so it stuck out from the shape each as a new body

- I then created a circle that was the same as the curve I needed to follow on an offset plane that represented the center of the circle of the slot.

- cut wouldn't work as there was the overlap with the non curved section for for I simple extruded it 2mm and created a new body

- Once I had one extruded out, I was able to using Create-Pattern following Path to have the two rows on the curve follow the curve exactly with the distance specified so that it matched the ones on the flat surface.

- I offset the one row which needed to be,- extruded all the new bodies through the curve.

The slots seem to be the right angles. The slots are the correct distance from each other.

I've a screencast (although not sure how helpful it'll be)

[ahreum.ryu]

Hi @Anonymous, 

Thank you for your solution! 

Regarding Sheet metal, I searched this webpage and it posted that sheet metal will be released in early December. (but I'm not sure whether to be delay )

here is detail information for sheet metal 

Hopefully it will be released soon! 

Many thanks!