Inventor part unfold view

[ss13953642009]

How to create an unfolded view of a circular part in Inventor, using a cylindrical body with a pipe opening as an example: unfold the cylindrical body (from 0° to 360°) so that it becomes a rectangle, with the pipe opening displayed at the corresponding angle.

[WCrihfield · Accepted solution]

Hi @ss13953642009.  Are you talking about a complete cylinder, with no seam in it?  If so, then you would have to create a seam in it first, one way or another, before it will let you flatten it out.  One way to do that is with the 'Rip' feature, which is only found in sheet metal parts, on the Sheet Metal tab, on the Modify panel.  So, first the part would need to be a sheet metal part.  If it is not already a sheet metal part, then you may be able to convert it into one.  Next, you may have to create some work features (WorkPlanes, WorkAxes, WorkPoints) on the model, because that feature will ask you where you want to place that feature, and a cylinder has no straight edges or vertices around its inner or outer cylindrical faces to choose from.  In a quick example, I first created a WorkAxis at the cylinder's center, then a WorkPlane that is 'Tangent to Surface and Parallel to Plane', using one of the 'origin' planes as a reference for the parallel angle, and the outer cylindrical face as the other.  Then created an axis on that outer plane, that is on that outer cylindrical face.  Then created 2 points along that outer axis, one at the top edge/face of the cylinder, and the other at the bottom edge/face of the cylinder.  Then, when I used the Rip feature, I chose the 'Point to Point option, chose the cylinder's outer face, and chose those two points, then specified the 'rip gap' as a minimal value, like 0.001".  Once that was done, I could create the FlatPattern as usual.