Why can't I apply a flange to this sheetmetal component

[ngowans]

A little background first, I am making a series sheetmetal flashings(several hundred variants) where the length is variable and the mitred angle of the ends of the flashings in plan is variable. I want to be able to feed inventor the width between centres at a datum use a number called "angle controller" which will adjust the angle of each side from 35 to 90 degrees,. my ipt file will receive a number from -55 to +55 and will apply a left hand mitre to anything under 0 and a right hand mitre to anything over 0. 

So far all is working well, and 2 of the 3 flashing types in this arrangement are working without fault. 

For some reason though the final flashing arrangement as show below will not seem to let me apply a flange. 

 Actually that's not accurate, the face highlighted will allow me to apply a flange, but only when the flashing mitre angle is not at 90

As soon as I try to apply the flashing to the 90 degree end, I get this error. 

I have been through my geometry and as best as I can tell, all of the cuts to generate this part are coplanar and perpendicular to the face of the material which was a bit of a pain to actually set up since nothing wanted to stay constrained to the projected geometry of the workplanes. I have been through measured any dimension, it tells me the thickness is exactly 3mm regardless of where I measure. 

I have added a form to change the angles and attached the file for people to have a look at. Any advise most appreciated. 

[JDMather]

Is something like this what you are after?

[ngowans]

Yes but I need the flange applied to both sides of the profile regardless of angle. As soon as the angle changes to 90 degrees (more accurately as soon as the "AngleController" parameter changes to anything more than 0 in your example) , it removed the flange and gives me an error. 

[WHolzwarth]

I didn't understand all of your concerns, but I noticed non-rectangular cuts in the flatpattern.

Placing a checkmark for Cut Normal in Cut8 looked better.

[ngowans · Accepted solution]

I managed to resolve the issue, 

The problem was that the cut plane "Top Cutouts" was developed separately from the cutbacks on the top and bottom, 

The cuts shown on the above in blue are a different feature from the purple highlighted cutout. This means that a flange can be added to the purple element when the overall cut of the profile is not 90 degrees, essentially the edge highlighted below allows it to function. 

However, when the cut is 90 degrees, the two separate features become coplanar, and as far as inventor is concerned, this is the same face at the end of the profile, if this was the end of a single contour flange, or a square "cut" on the end of said flange then inventor would be able to handle it and would flange as normal as it would be formed from a single feature. Unfortunately, when creating the flange in my case, inventor sees this as a single piece of geometry as shown below but since it's being formed from two totally different features, it seems to get confused. 

The solution was to add a small step to the top cutouts, This forces inventor to see this as two separate pieces of geometry and will allow the flange to be added. 

This could be considered a bug in the way inventor sees profile end faces which are created from two separate features. 

Intended geometry as below. 

[johnsonshiue]

Hi Folks,

The reason why Flanges cannot be created on those edges is because the side faces are not consistently perpendicular to the sheet metal faces. It creates inconsistent body thickness. The easiest way is to check either "Cut Across Bend" or "Cut Normal."

Another handy technique is to normalize the side faces by using Thicken command. Go to 3D Model -> Thicken -> uncheck Auto-Blend -> Intersect -> pick the inner faces -> distance = Thickness. Repeat the process from outside. Sometimes you may need to do it in reverse order. After that, the side faces will all be perpendicular to the sheet metal faces. And, the Flange can be created.

Many thanks!