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Curved Flat Metal Panel & Flanges

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Message 1 of 5
adam.couch.uae
3558 Views, 4 Replies

Curved Flat Metal Panel & Flanges

Please see the attached phtographs fo the actual fabricated panels. These show to reverse the information in the flat sheet drawings is no correct - the v cuts are neededflange we need to make V-Cuts in the flange to allow this to be bent in the reverse direction and folded. My question is can Inventor undertake this?

 

We have had sisues where the fabricators are undertaking the final fabricated aluminium panels incorrect in accoerdance witht he required geometry and they are struggling to create the drawings. We have therfore, only this week, looked at Inventor as a source to assist in this - we can model the panels but the flat sheet is not correct and does not show the required V-Cuts to create a reversed flange - like the images. Any ideas??

 

IN addition I also need to add flanges to the straight section of aluminium panel however the contour flange created will not permit this - see pdf for where I need to add returns. File attached. Any assistance wold be greatly appreciated.

 

Kind regards,

 

Adam.

4 REPLIES 4
Message 2 of 5

Hi Adam,

It can be done, but there are certain workflows that need to be followed. For instance, on the Contour Roll; you cannot apply a flange to the edge of the rolled/curved portion of part. In order to apply the flange, you need to use the Unfold command. This will make either a portion, or the whole part, unfold into a flattened piece. Do not confuse this with the Flat Pattern command. Once you unfold the rolled portion, the part should look like a two-sided pan, or a c-channel. You can now apply the flanges to each end. This unfolded form will also allow for you to create a Sketch on the face of one of the flanges (or on a plane parallel to the face) and make your V-cuts to allow the material to bend properly. Once you're done editing the unfolded part, use the Refold command to fold the part back to it's final shape. Be sure to choose the exact same points that you chose when using the Unfold command, otherwise the part will re-orient itself within the model space and other funky things.

As far as the part not being accurate, I've noticed that you made the center line of the cylinder not on the center line of the model itself (x, y, or z axis). I believe, but am no 100% certain, this is the reason the flat pattern stretch out is about 10mm short (if you were to do a full 360° revolution). I made a test model in which the center line of the cylinder falls on the Z axis and the stretch out is 100% correct with a K-factor of 0.5. Also, in your model, if you double click the Contour Roll, it gives you 4 different options for the Unroll Method. This could be because the center line does not fall on an axis, but I haven't tested that out. On the test model I made, the Unroll Method is greyed out and can't be changed, but is set to "kFactor".

I'll work on re-creating your model a little later with the center line of the cylinder lying on an axis and see if that fixes the discrepancy. I've attached a pictured and your modified part file.

_______________________________________
Eddie

Product Design Suite 2017 x64
Windows 10 (Build 1511) Professional x64
Message 3 of 5
erazorzedge
in reply to: erazorzedge

To follow up, I learned that the Contour Roll command does different things based on what you give it as a profile to revolve. If you choose just a single straight line, it will default to using a simple K-factor based roll. If you choose a profile other than a single straight line, it provides you 4 different options to choose from. See below for descriptions of each method (from the programs web-help).

 

Unfolding  & Unrolling
Specifies the method to unroll the Contour Roll feature. These methods all derive a Developed Length by multiplying the Rolled Angle by a Neutral Radius. They differ by the type of input provided:

Unroll Method
Centroid Cylinder An axis parallel to the revolute axis passes through the evaluated Centroid location providing input to define a neutral cylindrical surface. Default method.
Custom Cylinder Specifies a sketched line that defines the surface of the cylindrical neutral surface.
Developed Length Specifies the value that drives the developed length of the flattened rolled segment.
Neutral Radius Parametrically determines a value for the neutral radius (when multi-segment profiles are considered).
KFactor Method used for single-segment linear profiles.

 

In the attached images you'll see the differences in the Unfolded Length in the dialog box and also the position of the red line in the model. You'll see that choosing Neutral Radius for this part will work as intended. If you use the formula I have shown in the dialog box, you will get the correct stretch-out for a roll-formed piece. Change the "500mm" to whatever radius you're actually working with for each specific part.

 

I hope this helps.

_______________________________________
Eddie

Product Design Suite 2017 x64
Windows 10 (Build 1511) Professional x64
Message 4 of 5

Another option without using Unfold/Refold is to create linear extension based on the side face. It should be long enough to accommodate bend. Then simply create a flange based on the linear edge.

Thanks!

 



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 5 of 5

Many thanks for all the effort and information on my question - highly appreciated as being so new to Inventor (3 days of basic training) I am finding the learning curve massive. I will review all of your suggestins and input but just wish to thank you for the time taken.

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