Sheet metal bends in Inventor / Fusion

[sako243]

I suspect a very specific / niche problem but there must be a solution somewhere as it is manufacturable. I was pleasantly surprised that some quotes from Fractory for it to be laser cut and CNC bent were not that far off the online prices for the sheet of aluminium so it's quite appealing to just farm out the cutting and bending - thus I'd like to make it as accurately as possible so minimise the amount of weldng / cutting / trimming etc., that needs to be done afterwards.

The first issue is on the bend up the side - I've got it this close by choosing "Linear Weld" in the corner options of the bend but it's still a 3mm gap - it will be TIG welded and quite a gap to fill. I'd have thought there'd be a way to close up the gap a bit to allow for a tighter fit-up.

The second problem area is the top corner - ideally I'd like to extend this up to meet or extend past the top of the main panel - if it extends up past it then I can apply a cut across the top to trim off any of the excess (I've tried this in the top-left corner in the image below and it applies the cut to the flat pattern so that would work).

Any thoughts? I should say that I'm currently doing this in an old copy of Inventor Professional 2012 that I have and would prefer it to be done in that if possible.

 

[daedalusminos]

I would think you can tweak those gaps by rotating the face - the same is probably true for the second issue. Take a look at this foled bracket (in Fusion):

Base plate with ends folded up

Two edge flanges added (nothing extraordinary yet):

Face rotation:

Another face rotation:

Flanges:

 

[daedalusminos]

For your first problem, you need to tweak the bend rule as it needs a relief notch on the first fold

 

[daedalusminos]

I should also add that rotating the face tends to put a twist in the cut edge....but obviously the laser cuts square.

 

[daedalusminos]

Here's that first bend with some relief 1.5mm sheet 0.5mm bend radii, 1.5mm relief circle:

 

[sako243]

I figured out the rules I needed to tweak in the end. It will be welded up but if the gap could be closed it makes it a lot easier.

 

[Misterg]

I figured out the rules I needed to tweak in the end. It will be welded up but if the gap could be closed it makes it a lot easier.

In Fusion, you need to edit the sheet metal rule to change the 'Minimum Gap' setting (default is the material thickness):

I would have expected this would be something that one could override for each bend/flange, but this doesn't seem to be an option.

 

[sako243]

I would have expected this would be something that one could override for each bend/flange, but this doesn't seem to be an option.

It is in my ancient copy of inventor

I think I'll need to have a play with the settings a bit to add a cut out at the corner because I suspect it'll tear or crinkle if it's actually made but I have got the gaps a lot closer now.

 

[Misterg]

It is in my ancient copy of inventor

Those look similar to the available overrides in the F360 'Flange' tool, but 'Minimum Gap' isn't there (AFAICT):

A quick google says that the same settings exist in at least some versions of Inventor under 'Sheet Metal Defaults' (Mitre/Rip/Seam Gap):

(from here)

You can set the gap independently of the bend relief, so you can have close fitting flanges but still have a relief cut at the base of the bend to avoid distortion when folding.