Is it possible to make V groove in sheet metal using flange command?

[Anonymous]

We have this cladding that 10mm thick. Using standard bend will result big radius, so we use v groove to minimize. How can we make this v groove using standard sheet metal commands like flange, etc... Please see the image below. Thank you.

[mcgyvr · Accepted solution]

You cannot accomplish that utilizing just the flange commands..

You can extrude that shape later but often times you will run into problems with the flat pattern command and getting accurate flat pattern dimensions.. So you have to decide whats important to you and what you can live with..

Quite a few have proposed workarounds from modeling the part in the as grooved material thickness to modeling it full material thickness and modifying the bend tables to get close to just including a note on the drawing about the grooving and not modeling anything to manually adding the vgroove to the flat pattern to more and more..

In general Autodesk Inventor does not really have a proven/reliable process for this somewhat uncommon practice.

A google search for "Autodesk Inventor V-grooving" will yield a bunch of posts/topics about it.. 

[johnsonshiue]

Hi! I have seen similar requests before. Inventor does not support such groove using sheet metal workflows. The bend zone needs to have consistent thickness. One thing you can try is this. You can model the sheet metal part at 10mm thickness without the V-groove. Then derive the part as another sheet metal part. Create the V-groove using Extrusion Cut. For flat pattern, go back to the original part and make the flat pattern. And, cut the V-groove in flat pattern accodingly.

Many thanks!

[IgorMir]

With a bit of a planning it is not a problem at all. Here is how. Please see attached file. IV2020 format.

Cheers,

Igor.

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@Anonymous wrote:

We have this cladding that 10mm thick. Using standard bend will result big radius, so we use v groove to minimize. How can we make this v groove using standard sheet metal commands like flange, etc... Please see the image below. Thank you.

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[Anonymous]

@IgorMir, can this be done without extruding the groove through the flat pattern?

[IgorMir]

Hi Randall,

It wouldn't make sense, I afraid. 
You will get a Flat Pattern, based on the thickness of the material. And if the material is 16mm Thk. - the outer radius of the bend (minimal one) will be 16.01, for example. And the overall size of the flat material won't be what's needed.
That's why you have to work out what the minimal outside radius you want to get first. And that, in turn - will control the minimal thickness of the sheet metal. I hope - it is understood.

Cheers,

Igor.

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@Anonymous wrote:

@IgorMir, can this be done without extruding the groove through the flat pattern?

[johnsonshiue]

Hi Folks,

I believe Model States may help this particular case without having to create two parts. You can create two Model States. One has the cladding but one does not have it (suppressed). In the Flat Pattern, create the cladding in the reverse order.

Many thanks!

[IgorMir]

Hi Johnson,

What two parts are you talking about? All the OP wanted was to get a smallest outside radiuses on a folded thick part.
It is fairly straight forward modeling, as far as I am concerned. And I had offered a sample part to the OP.

Cheers,

Igor.

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@johnsonshiue wrote:

Hi Folks,

I believe Model States may help this particular case without having to create two parts. You can create two Model States. One has the cladding but one does not have it (suppressed). In the Flat Pattern, create the cladding in the reverse order.

Many thanks!

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[officeCTLBL]

 genius mate, thanks

@officeCTLBL - this post has been edited due to Community Rules & Etiquette violation. 

[regonaymarygrace]

Hi Igor, I Have a related issue regarding acp. Since it is V groove, how can i edit the bend allowance value in the sheet metal rule. for example I have a 4mm thk acp. the alum is 1mm thk., inner radius is 0.5, but I want the outer radius to be 1mm

[IgorMir · Accepted solution]

With the plate 1mm thick the outer radius can be 1mm if inner (bend) radius is 0mm. But Inventor won't allow you to have zero Bend Radius. You could, however, make the Bend Radius extremely small. Say - 0.001mm. 
Here is a part in IV2020 format.

Cheers,

Igor.

[lauri_barnhart]

Hello, @regonaymarygrace,

Just checking in—did the responses shared by @IgorMir help clarify your question?

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Lauri | Community Manager