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.
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How to unfold a section of a cone? 2
- Thread starter ArtSmart
- Start date
drvitorino
Mechanical
- Sep 16, 2003
- 6
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
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
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1
- #3
DesignerMike
Mechanical
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
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
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1
- #4
Hi
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
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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