Sheet Metal Corner Gap????

Could anyone help please, I'm using Inventor 2008 Pro in the sheet metal format, and having a slight problem with corners!! The guys in the workshop are telling me that when they bend up an enclosure the edges of the flanges are always corner to corner. I've been trying to achieve this by creating a face and four flanges and then using the corner seam tool to bring the edges together corner to corner. But it has to have a gap size, i have tried putting in "0", but it will not recognise this. which means i always have to have a gap. I have tried selecting the corner rip tab, but this will not then allow me to select an edge. Any help would be much appreciated.

Thanks.

I could kind of recreate this, but it requires a bend radius of ~0 (actually, like .0001 since it won't accept zero). This causes it to run painfully slow since I think it tries to rationalize it in some way and this is only a marginally realistic bend radius.

On that same note, there was one corner that this kept crashing on (well, erroring out, not crashing the program).

All of this leads me to believe that there HAS to be a better more programmatic way to go about this, but I'm still too green to see it. That said, here's at least one way to make it look like that.

After setting your BendRadius to almost zero to make your flange:

Finish making your flange (or four of them rather) and then, open Expand the flange you created in the browser, right-click on Corner# > Edit Corners. I think you have to do them all individually, but select one of the corner icons, hit the first checkbox and from the dropdown select "No Seam" (has a big red X on it).

This should give the effect your looking for.

Zip and attach what you have so far.

Thanks for the detailed response. But i am still struggling with it. I've followed the steps that you listed above but i don't seem to have the same options as you when i right click on the corner tab in the browser. I have tried to include a screen shot of the options that i have(Not very experienced with forums). Maybe i'm going about this the wrong way. At the moment i am just creating test parts, to find a way to acheive this corner to corner before i can start on a real project!!

Corner seam.pdf

It could be because I'm using 2009, and if that's the case I'm sorry for misleading you. As I said, I'm still brand spanking new to the program and am probably doing (more than) half of it wrong.

Good luck, hopefully somebody else will have more luck pointing you in the right direction (and I have to admit, I'm quite curious now).

Need help,

I guarantee that, despite their best intentions, your shop people are lying to you whether they know it or not. A gap of zero between two edges would require them to be welded together. Inventor is a computer program and as such is very literal in what you tell it to do. Try putting in a very small number for your gap.

There must be a gap of some value or the program sees an interference. 2009 has some better tools as Hoozin has shown you but 2008 should be able to do what you want. Perhaps you could post a file like JD suggested, that way we can see what you have already done and point you in the right direction. It may be that you need to model things a little differently to get the result you want.

I have uploaded a zipped part file, this is a test part file that i am using to try and acheice the corner to corner seam. If it opens up properly, you will see that i have had to put small gaps in the corner seams. But as i mentioned before, i need no gap at all. Again any help would be much appreciated!!

Mike

Test Unfold.zip

Yoiur first sketch is unconstrained, I would start with this document -

http://home.pct.edu/~jmather/AU2007/MA105-1L%20Mather.pdf

I would have used a single Contoured Flange rather than 4 Flanges. Also in the manufacturing process you cannot make the flanges to exact sizes - there is always a +/- tolerance. A gap (might be very very small) is generally built into the design to account for Maximum Material Condition. Otherwise hand fitting will be required. Your shop floor people are probably doing a bit of artistic hand fitting.

I've taken a look through the pdf, and there are some good tips in there!! Not being a sheet metal gut myself, i havn't used(avoided) using the sheet metal format much. I am starting to understand the reason why a gap is needed in the corners. I am a little baffled about using the contour flange command for creating the sides of the box. Having not used this command before i am assuming that the outcome would be a solid four sided box. I am trying to use this format for unfolding the model for a CNC punch layout. Maybe i should have mentioned this before. What the guys in the shop are telling me is that the flange width/length should be exactly equal to the width/length of the box minus 2 x thickness of material???

Check your bending styles option. Change to Linear weld, and gap to 0.1mm. This should automatically set your corners 0.1mm without doing corner seam, since physical bending will not easily achieve a 100% angle precision, 0.1mm is acceptable. As for the radius, it shoud be around 15 - 20% of thickness, as this is the final physical result. Setting a small radius will cause a deform or bulge to the 3 corner bend. I don't have the program at this pc, so i can't give a detailed explanation to where to find those buttons.