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In Autodesk Inventor Professional 2024, I am failing to add a flange to a sheet metal cone (300° for now, eventually the tabs will be used to mount and close the funnel), that is created in a sheet metal part file by

  1. Sketching a line and an axis for a Contour Roll (Sheet Metal tab)
  2. Rotating a rectangle (3D Model tab)

open sheet metal funnel modeling attempt

For either there is no preview in the 3D view.
For 1. the flange dialog never offers OK or Apply, regardless of the settings.
For 2. if I adjust the settings provided by the Bend edit "glyph", the Dialog can be accepted but results in an error that has no further explanation.

It works straightaway when adding a flange to a plain Face.

What do I have to do to add flanges to this part?


Edit 1:

How can flanges be created so the cone is closed? The features (Thicken, Flange) intersect.
Rolling only 180 deg. and mirroring works in principle but also causes an intersection. Thickening inwards does not work.

enter image description here


Edit 2: Can't get Bend or Lofted Flange to work either.

create bend between contour roll and face

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1 Answer 1

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The reason for this seems to be the behavior of the top and bottom faces of the cone, they would make the ends of the flanges weird so that Inventor does not know what to do there. Creating the cone as a 3D model also seems to cause issues with the flange tool. You can solve it by forming the cone via sheet metal tools and adding a little straight extension, just long enough to accept the bending radius.

  1. Create the cone from a single tilted line with the proper measurements and by using the sheet tool "Contour roll". This lets you create the cone as sheet metal and enables the next steps. Setup for contour roll
  2. Create a work plane on the edge that you want to bend the flange around, perpendicular to the future flange.
  3. Add a little straight extension that is just wide enough to accept the desired bending radius with the standard sheet tool, this allows Inventor to create a well-defined flange and will vanish later in the bend.
  4. Add the flange on the end of the extension.
  5. Repeat on other side

Final result including the working planes:

Flange_Result

Concept of the flange extension:

Flange_Base

I hope the result turns out the way you imagined, let me know if some steps are unclear, then I add more screenshots.

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  • $\begingroup$ The Face "extension" built on the tangential workplane can be infinitely thin but seems to require the flange to use "face" as bend position, otherwise it ends up in offset-hell and everything intersects. $\endgroup$
    – handle
    Jan 2 at 16:17
  • $\begingroup$ The Thicken modifier can also be used (quicker than Workplane/Sketch/Face), as suggested in forums.autodesk.com/t5/inventor-forum/sheet-metal-cone-flange/… (distance twice the sheet thickness w/ default bend radius). $\endgroup$
    – handle
    Jan 3 at 8:47
  • $\begingroup$ Is there a way to close the funnel, i.e. Contour roll for 360 degrees (or rather 359,99..°) so that the flanges "touch"? The problem is that the "extensions" and flanges intersect with the cone and each other so the geometry is not generated. If the extensions are less than twice the thickness, Inventor does not properly remove the material used in the bend/flange. $\endgroup$
    – handle
    Jan 3 at 9:53
  • $\begingroup$ Clearly the edges at the open part of the funnel have to be parallel to be able to close it without intersection. Clamping it together will then cause the funnel to deviate from the shape of a perfect cone, that's the trade-off when clamping it. $\endgroup$ Jan 3 at 17:23

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