Sheet Metal Self Intersecting Flanges Error

[pinco pallino]

I need to bend flanges at 100 deg. See pic. The corner has to be trimmed and welded. Is there a command for mating the joint or they have to be extrude cut one by one?

Thanks in advance.

[JD Mather]

It doesn't look like you modeled the part correctly. Why didn't you attach the file here?

[linnmaster]

Try modelling both the flanges in one feature by selecting the two edges .... it should automatically mitre. There are options in the flange dialogue box that allows seam ... where you can adjust overlap or clearances between each flange, even hole shape and setting for the corner relief hole.

[JD Mather]

Try modelling both the flanges in one feature by selecting the two edges ....

 

The way I read it one flange is angled 10° while the other is perpendicular - so I don't think your method will work. Can you post an example with your method?

 

That is why I always always always suggest posting the file or an example that exhibits the same behavior to check the design intent. I "think" I can get it to work, but without the file....

[linnmaster]

Hmm. I need to know how to do that also so will watch keep close eye on this.

[kencaz]

You need to add a couple corner seams after your have created the 100 deg flange.

 

Here is a 3 sided flange at 90 and a single at 100 with two corner seams added to correct the flange.

 

 

Hope that's what your looking for...

 

KC

[JD Mather]

Looks like KC has it figured out.

 

If you want tighter corners set the bend to tear or linear weld and one side to overlap. Might decrease the gap as well.

[linnmaster]

Hmm .... I get an error.

 

If you do the 100 deg and the 90 deg flange in such a way where the flanges do not you intesect each other, the corner seam can be applied and works as above confimed by KC.

 

If I construct the flanges in such a way where they intersect, ie, 100 deg flange, and 100 deg flange, or 90 deg then 100 deg, I find that you get an intersection error (number 1) and (number 2) error when you apply the corner seam.

[pinco pallino]

Thanks for your input.

I think I’ve got it.

Innmaster, the way you suggested didn’t work with IV 10. (not 2010)

 

 

JD here both flanges are at 100 deg.

 

 

The trick as I found, is to offset the flanges sufficiently to avoid intersecting on creation. Use then the corner seam tool to bring them together.

I also found that to achieve symmetry in the flat pattern is hallways best to create the flanges with an offset equal or bigger to the outer radius of the fold. Join them together if needed with the corner seam tool.

[shift1313]

Pinco one thing you can do if you have some funny intersection points is to create a new face. I have had to do this when i had edges meet at multiple angles or arcs. Inventor doesnt allow it but other software allows you to change the sketch of the bend during creation, but with inventor you need to draw it before hand. If you need it at something other than 90degrees just create a new plane that intersects the line you wish to start the bend from. Here is an example. Of course this example would be extremely hard to make but the point is you can create funny shapes. I simply made an offset of my first flange in the sketch.

[kencaz]

Pretty cool Shift!

 

couple questions though.

 

1. Can you show me the intersecting plane your referring too.

 

2. Can this be then flattened or not..?

 

Thanks

 

KC

[shift1313]

1. I select the edge you would select to create a flange, then the side face of the part and create a work plane at an angle. In my images it was at 30degrees.

 

2. Yes it can be flattened. After i created the 30degree work plane i started a 3d sketch and got an intersection curve between the solid and the work plane. Then i start a 2d sketch on my 30 degree work plane, project the edge i want from the 3d sketch and offset it whatever i want my gap to be. Finish sketching the face then in the face dialog box, select the sketch face to use, then select the edge you want for your bend.

 

If you want your sketched face doesnt need to intersect the rest of the body. You can create a blend between the two.

[kencaz]

Thanks, Matt,

 

I'll have to give it a try.

 

KC

[pinco pallino]

Thanks, Matt,

 

I'll have to give it a try.

 

KC

 

Me too.

Shift, that's impressive.

Did you use the contour flange tool for the first flange?

And why using 3 D sketch intersection? Haw about project cut edges?

[pinco pallino]

As for the project cut edges as I asked previously, I found the answer my self.

You right Shift, mast be a 3D intersection.

Here I'm trying to reproduce your work every thing went smooth but got in trouble with the Corner Seam tool.

It only allows to select one edge at a time, see result in pic.

How did you trim it?

Thanks again to all of you.

[shift1313]

Hey pinco, yeah once you try to project the edge you find out its not where you want it:)

 

I created the images above using only the flange tool and face tool. I created a flange at 120degrees 1inch long, then another at 30degrees 1/4inch long. Then created the plane, 3d sketch for the intersection of the plane and the flange. Then the face. And finally i created a sketch to Cut the edge of the first flange so it was 30degree off(matching the newly created face). Hope that made sense.

 

I could have used the contour flange tool for the first flange. The results would still be the same:)

 

 

If you want a more in depth step by step let me know.