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How to unfold a section of a cone?

How to unfold a section of a cone?

How to unfold a section of a cone?

I'm trying to unfold a section of a cone.  The cone is split lengthwise and has uniformal thickness.  However, when I try to unfold it, I get an error.  At the same time, if I try to do the same thing for a 'cone' with square bases and rounded corners (edges), it unfolds it with no problem.  

RE: How to unfold a section of a cone?

It appears Inventor does not have this functionality inside. You should buy SPI or COPRA Metal Bender to do that(aproximately U$2000).
Maybe you have already seen that Inventor hasn't got another important function, the normal cut (that you use over the 3D model when you plan to have a sheet metal cut by a punching, plasma or laser machine before processing bends)

Project Engineer

RE: How to unfold a section of a cone?

I have had decent luck unfolding part of cones, but it doesn't always work for me....I'm sure it has something to do with the way that I generated the cone in the first place.

I am usually generating a template for fit-up to another cylinder or cone, so I am just interested in the "surface" flat pattern. (I can't verify the accuracy of a thicker material)

This is my process (probably not the best way, but it works for me): I start by making a solid model of the cone (usually extrude a circle at a set angle), I then subtract whatever bazaar geometry I need to remove for fit-up (usually I am intersecting a pipe at an angle), I then split the cone in half (we usually purchase them in halves anyway), I then shell the cone very thin (.0001" to reduce the k-factor error on the surface) and remove all the faces except for the face I am interested in, I then switch from modeling mode to sheetmetal mode, I then select the face I am interested in (turns cyan colored when selected) and hit the flat pattern button and it usually goes flat.

You can then make a 2D drawing of it. When placing the base view you must select "flat pattern" under the tab "sheet metal view" to get a flat (it defaults to folded model). You can place both a flat pattern and a folded view on the same sheet. I then normally output the geometry to autocad and ovelay the full size cone for the template (and verify the size).

If it doesn't work for you, post your e-mail address and I will send you an example. I'm using R7 SP1 ... I think there were some issues in SP0 that kept this from working but I can't remember for sure, and I can't remember if I did this same process back in 5.3 or not? Good luck

RE: How to unfold a section of a cone?

The key to generating flat patterns from cones or portions of cones is that Inventor along with many other similar modellers needs to a truly straight edge to get things started.

In the event that a cone has been sectioned or cut in some way it is critical that there exists an edge which was created by a cut plane that contains (exactly) the axis of revolution of the cone. At least that was the restriction in R7.0

There was also a further problem that if the portion of the cone to be flattened contained holes then it would not always unfold - again I have not tested this in R8.0 yet

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