SHEET METAL CORNER

[AnthonyHarris90842]

Hi Guys
Although I have worked with inventor for a very long time I have never used sheet metal so I really need some help here.
I attached my files so you can see how I went about achieving my desired design.
I took a normal IPT which was adaptive in another assembly and I got it to be the shape I want.
As it is a part for sheet metal work and I now need a flat pattern I decided to derive it into a sheet metal part and then sort of model over the derived part and in so doing if I change the original part my sheet metal part should also update.
Ok is this a good way to work with sheet metal parts which I think makes them sort of adaptive?

Secondly I have two images below. The first one is how I am currently getting my corner from the method I am using but I would like my corner to be the same as the second pic.

Thank you very much

[Anonymous]

I would prefer to avoid derive.
It works fine if you move a hole, but it becomes an issue if you add or remove holes, or make other drastic changes to the geometry.

If I absolutely *had* to use the workflow you used, I would derive it as a surface. That way you don't have to derive it once more just to create the flat pattern.

In regards to your corners, inventor sometimes renders it in a weird way, even if the flat pattern does it correctly. You cannot always rely on what it shows in the corner of the folded part.

However, you can change your corners by changing options in the "corner" tab on your corner seams.

[Anonymous]

I just did a remodel in the way I would go about creating this.

I believe you can always add a weldment in the assembly environment, although I have no experience with weldments.

[AnthonyHarris90842]

Hi YE
Will look at your file and come back to you.
Thank you so much for your help

[SBix26]

No need to derive-- simply use the Convert button to change the file to a sheet metal part (then make sure to set thickness, bend radius, etc.)

---

Sam B
Inventor Pro 2021.2.1 | Windows 10 Home 2004
LinkedIn

[johnsonshiue]

Hi! The two images actually show two types of corner relief. The top one is a three-bend corner, and the bottom one shows a two-bend corner. The "Tear" relief shape is only available in two-bend corner, not in three-bend corner.

I suspect you may want to change the three-bend corner to "Intersection" type. But, in folded model, the shape will look the same as what you have now.

Many thanks!

[AnthonyHarris90842]

HI SBix26
Yes I know you can just convert it but then will it still be adaptive as with my work flow where if the derived part changes then my sheet metal part will change to suit.
Also I read somewhere that you have to show Inventor where the rip lines are and post processing with the bends

[AnthonyHarris90842]

Hi Johnson
Yes I tried that and it stays the same.
What I am basically trying to achieve is an adaptive sheet metal part that changes to fit my derived model, hence my work flow in the Sheet metal sizer IPT.
Maybe you can suggest a better way to do this then

[Anonymous]

Hello @AnthonyHarris90842 

If your aim is to change with the width of a wheel of some kind, you can project a line showing the width.
Then dimension it, and set the length of the contour flange in my example to be that Driven Dimension.

You can also project the circle and and dimension the profile tangentially to that.

[AnthonyHarris90842]

Also now I cant remember how I got the bend to look like the second pic in the original post

[SharkDesign]

Corners and tears are specified when making the flange, you can also change them by double clicking to edit the flange and clicking on the icon that hovers over the corner. 

As for your other question, based on other posts I've seen you make, you are very keen on adaptivity. Inventor doesn't work well with adaptivity and I'd advise not to use it. However, you can do it your way by not doing a derive. Convert to sheet metal as someone else said here and make sure your material thickness and all rads are correct. Inventor will treat this as a normal sheet metal part and allow you to create flat patterns. 

[AnthonyHarris90842]

Hi James
Yeah I know I use adaptivity quite a bit and the reason is we design and build custom high tech automation machinery and there are constant changes to so many parts during the design stage that we need adaptivity to save time and also some times you forget to change all the parts that are effected or even interfere.
Will try and convert the part and see what happens.
Thank you so much for your help

[AnthonyHarris90842]

Hi James
I converted the part to sheet metal as you suggested but Inventor wont give me the flat pattern.
I attached the converted file.

[Anonymous]

You need to rip some welded corners for it to unfold.

See attached where I only added some rips to your part.

[AnthonyHarris90842]

Hi YE

Thank you so much for your help.
I checked out the part and I have a question for you.
Once I have converted the part and done the rips would the part still be adaptive and change as it did originally?

[Anonymous · Accepted solution]

Yes. Nothing of what I did should break any adaptivity.

I would, however, always start with a sheet metal part, and use sheet metal functions such as face and flange. They will ensure in most cases that you can get a proper unfold.

As I stated earlier, you would be able to draw the part as I did originally by referencing the thickness and diameter of the wheel, and then drawing your initial sketch and contour flange with reference to those.


Edit: With sheet metal functions such as face and flange, you will also automatically get corner seams and bends without the need to do any cutting or fillets.

[SharkDesign]

Yes because it is parametric. All the features above the rips would update.
However this doesn't mean that you won't create errors if the sheet metal
rules are no longer being followed. Also, your flat pattern will probably
error and require being regenerated.