How to roll a flat Sheetmetal part

[SMillsYS3X2]

I'm trying to add a roll to a flat Sheetmetal part. Searching ways to do this keep leading me to videos that start with a rolled part THEN unfolding it, adding cuts and holes and other features, then refolding it. Is there a way to start with a flat part, add the features you want THEN 'fold' it into a rolled part?

Basically start with this;

and change it to this;

[steveh5]

SMills...

Assuming you are already converted this to sheet metal and set your thickness.

1) Yes...you can start as a flat profile and then bend up using the "FOLD".

2) You can then "UNFOLD" the part after you formed it. You can do all the bends or just a couple. Add some features and then "REFOLD" it.

3) Then "REFOLD" it back up

HTH,

Steve H.

[SMillsYS3X2]

Your mis-understanding. I need to ROLL the entire part from a flat, not bend one or more flanges. 

[CGBenner]

@SMillsYS3X2 

Hi, from what I can see in IV2026 (I'm not experiences with Sheet Metal), it looks like you need to use Contour Roll to create the basic shape, Unfold it and add the Holes/Cutouts, and then Refold it.

[SMillsYS3X2]

Hence my question about starting from a flat. Trying to get accurate overall measurements from flat, THEN worry about it's shape.

[steveh5]

Does this example help you out? This part is rolling from a flat.

[SMillsYS3X2]

I can't accept DLs from this forum, so I can't see it. 😞

[johnsonshiue]

Hi! Steve is right. This can be done using Fold command. You need to set the bend radius very large so that the entire piece is bent. Inventor Contour Roll is meant to create the elbow that has two linear extensions on both ends. Unfold (unroll) ensures the two linear extensions go back to straight state.

Many thanks!

[steveh5]

Message me directly and I will send via email?

[kacper.suchomski · Accepted solution]

Hi

Look at this:

[dan_inv09]

(This seems like a wall of text but trust me)

Did you create it in the sheet metal environment?

Say you have a model that you just created and you do not know about "environments".

I've never used sheet metal for anything I've made for work so all I know is just from playing around a little bit here and there. (Actually, I think I did have a 1/2 inch thick piece of steel that was about a quarter of a circle that I used in a big welded housing - it didn't come in matching the print and from then on we used three or more flat pieces for whatever would have looked nicer as a curved piece.)

Find the environments tab - probably just to the right of view, and on it there is "convert to sheet metal"

Now way towards the right find sheet metal defaults, click the pencil next to sheet metal rule and the style and standard editor pops up where you have to create a new sheet metal style - pick your material (the default may be fine for now) and change the thickness to what the thickness of your part is (how far you extruded your profile - you might even be able to put the parameter name in there)

Then you put a sketch on the face of your part and add a "bend line", for some reason it only wants to work  if the line runs from one edge of the part to the other if it's too short or too long it does not like to let you select it

Pick "fold", select your bend line and put in your bend radius and you can hit okay - you are going to be using a big radius - the default is for a pretty sharp corner, your curve is along the whole part.

and you get a funky bent part - heck one of the radiuses that I just tried the bent part was off the screen.

I get a more likable part by putting the bend line in the middle of the part and selecting the middle "fold location"  - the first I assume is supposed to put your line in the middle of the bend which doesn't seem so useful in our case (and I have no idea what purpose the third has with the line at the end of the bend).

So, I use what I call "the start of the bend" option - but that only bends half of the part, so we have to go and share the sketch and fold again but this time hit the first button in "flip controls" and that does the fold on the other side, do not forget to pick the "fold location", I'm pretty sure it will always go back to the first choice every time you start a new fold and that is going to give you funky results.

Now, someone who actually knows what they are doing - please explain to us what I just did, why nothing else seems to work in a way we would like, and if there is some way to do it better! Thanks.,

[SMillsYS3X2]

Still starting with a 'contour' part. And I would like to do it that way, but one of the headaches with this part is that it's ends are angled. So the refold fails after I angle the ends. 😞

Here is a picture of the flat, the angled ends don't show up too well in the isometric pictures above.

[SMillsYS3X2]

This looks like the best solution so far. Have a problem with the part moving away from origin when in the formed view. Adding work planes and points as needed so I can place it in the assembly as intended.
Picture of the formed view with the origin and plane the flat is on highlighted.

[kacper.suchomski · Accepted solution]

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@SMillsYS3X2 wrote:

Still starting with a 'contour' part. And I would like to do it that way, but one of the headaches with this part is that it's ends are angled. So the refold fails after I angle the ends. 😞

Here is a picture of the flat, the angled ends don't show up too well in the isometric pictures above.

---

This is not an obstacle.

[SMillsYS3X2]

Oh, I see! That could work!

[NigelHay]

Trying to do something similar but I need the roll up to be helical. I've tried several methods but none quite work. Whatever way I create it, I need to be able to unfold it into a flat pattern.

Ideally, I would start with this:-

...and end up with this:-

I've created this by using the coil command to make a 1 turn rectangular helix, then adding the end folds but those end pieces are a real bodge. I've just extruded the end profile. This will not let me create a flat pattern & the unfold command will not unfold the ends as they were not bent.

[dan_inv09]

Holy Mackerel!!

I do not think that Inventor is capable of doing what you need.

This nastiness is the closest that I could come up with. (note the little flat bit on the end of the coil that allows the flange to exist)

[NigelHay]

Dan,

Did you start with the flat form then use the bend command with a large radius? I tried that but could only get it to bend half of the flat form. Could you share your model?