Sheet metal part with flanges over a curved surface

[Anonymous]

I am still new to inventor (yes only 3 weeks experience ), but with some advice from some folks here I am making headway.  I'm still having problems with a few concepts though.  After watching a dozen or so videos and reading even more write-ups, I still can't seem to get the proper way to create flanges over curved sheetmetal surfaces.  So, after seemingly trying every possible permutation of possible ways to go about this, I decided to see if one of you can help me figure this out.  

Part of the issue may be the general way I am having to go about this, so if you'll indulge me, I would like to breifly explain a bit about what I am doing.  I am creating an entirely new dash assembly for a 69 Camaro project, and given that I have no 3D model of the firewall, floorpans or anything else inside the car, I started with foam/cardboard templates that were made in the car itself.  I've then digitized those and imported them into Inventor as the basis for creating the rest of the components that can be however I like.  I say this may be the problem just because it seems like the workflows in Inventor are designed to start from a drawing and create 3D shapes rather than start with a 3D shape and create the drawings that then recreate the 3D parts. I have redrawn the digitzed parts following JD Mathers' advice to create better native geometry, but I am still having to create parts derived from other parts as needed to connect the left and right sides while taking in measurements from how everything fits in the car once I've made some of the items.  Maybe it's just me, but this seems to be counterintuitive in Inventor from the normal sense of designing something from scratch where you design all the parts to work together from the start.  I've attached an image export of where I am so far to give some perspective (still a long way to go I know).  

Anyway, the attached files include 3 of the many attempts for creating the sheetmetal "skin" that will make up the passenger side of the dash board.  The basis for the overall arc of the skin is determined by a part I created from one of the foamboard templates that I designed at the outset (maybe I should attach that too).  The first attempt was to make a sketch off of that first part (the one from the foamboard template) and paste it into a new part.  I then extruded it, unfolded it, cut it as needed and refolded it.  All is fine, except that I also need to add a flange at the outer edge along the arc and I can't get it to work.  To add this flange, I drew a line on a new sketch of the unfolded part where I want it, use the Fold command and all looks good.  Then when I go to refold it, I get a preview that looks perfect (see attached screenshot) but then the computer goes off into la-la land for a really long time and never returns.  I have to end task and restart the program.

After some input here on another part, I decided that the way I should be doing it instead would be to instead derive the skin from the mounting flange I created to join the parts together.  So, I made another version by using the Derive command in a newly created part and importing the previously created flange part as the base solid.  That was much faster, but I still can't get the sheetmetal flange to work on the opposite side of the part for the same reason as above.

Lastly, I started similar to the previous attempt, but used a surface extrusion and the Thicken command to create the skin thinking there may be something wrong with the thickness/uniformity of the part in the other methods causing the program to hang up.  Unfortunately, I had the same issue as the others.  

I also tried several variations using the contour roll, but couldn't get anything that resembled what I wanted (something about the axis thing that has me confused), the standard flange tool (both in folded and unfolded form) but that wouldn't let me select any edges, and the contour flange but I have no way (that I can figure) to combine the outer arc with the 90 degree flange on the other end.  I just know I'm probably missing something very simple.  Most of the rest of this project has been pretty easy to figure out.

Any input would be greatly appreciated.  

[CCarreiras]

Hi!

Sorry, i have not read all you testament 🙂

Is this what you had tried to achieve?

[CCarreiras]

Also... when you post a derived part, you have to post also the main part...

[Anonymous]

Hi Carlos,

Thanks for the reply.  That's what I have already (on one of the attempts) that has a designed flange along the top edge.  The only thing I see different in the pic is that it is mirrored.  What I need is the green preview entity Inventor showed me in the screenshot (posted here again).  After showing me the preview, I click apply and the program locks up.  I'm guessing I have some geometry that it doesn't like or I am going about the process all wrong.

Good point about the derived part.  I have added that to the attached zip file, which reminded me of another issue.  In doing all these different tests, one thing I ran across in doing the derived part was that I had to remove all the fillets from the sharp edges at the middle zigzag in the part otherwise I got an error when trying to project geometry to make the arc for the skin.  Could be a fluke, but I'm wondering because I eventually would like to put the fillets in there.  If I do, is that going to cause issues given that all of the parts are linked together when deriving one from another?

Thanks again,

Tim

[CCarreiras]

OK....

First, you have to know that inventor can't solve this, because this is a plastic deformation, not a bending, therefore it will not calculate compensation or give you a flat based in that.

But... it's possible to achieve the flat with some side techniques, using derived part. If you give me a couple of hours, i can do that for you... right now i dont have the time 😞

ps: have you add the derived part and the main part in this zip? i will take a look in a couple of hours... maybe less...

[CCarreiras]

And think a little.... how do you expect that the part flat in the zigzag?!!!! the material will overlap!!!

This is tottally a die part, not bending....

[Anonymous]

Not that I don't believe you, but why could this part not be made in sheetmetal?  I wonder if there is a misunderstanding on what I am trying to make (probably because of the workflow I am using as described in the first post).  If it can't be made this way, that's ok I guess...I can figure out a different method (maybe welding on the flanges needed, or some other material), but I would like to know the reason so I can learn and prevent making the same mistake going forward.  Just so you know, all of the sheetmetal parts will be covered with 1/8 foam and then apholstered with leather.  So perfection as you would need on an assembly line to make precise parts is not needed here.  

Anyway, Just to be sure we are on the same page, the only part in this post that I am trying to make from sheet metal is the skin.  The thick flange part that I used to derive the skin from will be machined out of billet aluminum (or at least that has been my plan) and the skin will be welded along the edge of the inner face.  The reason I brought that part in and derived from it was to capture the arc that the skin needed to follow.  That machined flange was similarly derived from one of the symmetrical sides of the center stack (seen in the image capture of the whole project in my original post).  

[Anonymous]

I think I didn't explain well.  See attached screenshot of what the part would look like in the zigzag area and also the unfolded version of the part with that cut in it.  Part of the problem too, is you are seeing multiple versions of the same part where some of them don't have all the same features.  This is because once I stalled out on the flange along the curved edge, I made different versions starting from scratch to try different techniques just to focus on that one problem.  Once I figured that out, I would go back and implement them all together.

This part unfolds perfectly showing the cutout for the zigzag and glove box door.  It just needs a flange on the opposite end from the zigzag.

[stephenrottloff7259]

It is not that this part cant be made out of sheet metal, it is that inventor does not currently support non-linear deformation.  Your part has a curve, which the flange follows.  Inventor sheet metal does not support that.  In other words, your part may need to be a die formed part, not a press brake formed part.  However, you can model any type of part in Inventor, but to get a proper flat pattern out means no non-linear deformation in sheet metal mode.

Hope this helps.

Stephen R.

[CCarreiras]

---

@Anonymous wrote:

Not that I don't believe you, but why could this part not be made in sheetmetal?  

Yes... you better believe... you are not thinking about what youre saying, sothink again... or better, think with me:

First: if it was made with flated flange, you must have rips (the red lines)

Second: if you flat the flanges, as you can check by the arrows, they bend for the same side, therefore you will have have material on top of material... now, you tell me how to do that??!! Yeeee... Impossible.

You have no clue how to do that, right?

I think there's only three ways:

1 - die form (not bending), but too expensive to produce one or two parts

 2 - two parts welded (i vote in this one)

(and offcourse you will use sheet metal as material raw for both cases, this is not the point, the point is the process, not the material raw)

3 - Or you can produce the solid in 3D Printing and give it a finishing of metal paint aspect (also like this idea)

And for close the case.... Inventor doesn't calculate "die forming".... only "bending".

Of course you can model this.... but, how about to produce?

[stephenrottloff7259]

By the way, very nice model for 3 weeks experience!

Stephen R.

[CCarreiras]

garding the modeling stuff.... my advice is; create one assembly with the 3 parts.

Of course you can use derive part to import info between parts, or edit the parts in the assembly context copying faces,  project geometry, etc.

But you have to maintain sheet metal with only one solid to flat.

Again your files are a mess, and the derived parts doesnt correspond to the main parts you attach..... i think we are losing time trying to help you....

[Anonymous]

Hi Carlos, no.  They are two separate parts.  Not one part.  The skin is sheet metal.  The flange with the threaded holes in it is machined from billet.  These will be welded together after they are each separately produced.  They are only in the part together in order to derive the arc shape of the flange and use it to create a bend profile for the skin.  My understanding is that this would also allow the parts to be linked in such a way that if I needed to change the arc of the flange in some way, that would also translate to the skin.  But, they would be produced in different ways at different times.  I'm gathering by the response though that this is not the standard way to represent such a thing.  I'm open to suggestions for best practices on this too.

Back to the real issue....the flange there in that picture is not the issue.  It's the flange I am trying to bend into the skin on the exact opposite side of the part.  On that side I don't need the structural strenght of a thick, machined part.  I just need a mating surface for another trim cover that will finish off the side of the part so when the door is open, you don't have a hole there where you can see in behind the dash. 

[Anonymous]

Hi Stephen,

Thanks a bunch for the explaination.  I get now the issue the program is having trying to calculate this.  Essentially, it is trying to do the equation in reverse.

My original thought about how it would be made would be to form the primary curve in a rolling machine like the one in this video https://www.youtube.com/watch?v=NuaHvc5MPDg (particularly from 2:00 to 2:15 in the video) to achieve the 3 arcs in the contour.  I then figured  the end of the part I need the flange bent in could be run through a machine similar to this: https://www.youtube.com/watch?v=JqL4Ip5I7rc 

I knew you couldn't first bend a part in a press brake and then try to curve it, I just didn't know what the program was capable of in terms of determining a flat pattern from whatever curved part I modeled. 

So, if the program can't calculate it this way, could it be done more like it would actually be made?  A contour roll on the already bent part somehow?

Tim

[Anonymous]

Thanks, Stephen! 

[stephenrottloff7259 · Accepted solution]

It all depends on what you need after your modeling is complete within Inventor.  If all you need is the model, with no reliance on flat pattern output, you can choose any modeling method to achieve your modeling goal(s).

If you need proper flat pattern output at the end of your modeling, then you are bound by Inventor's capabilities within the sheet metal environment and need to choose your modeling method to coicide with them.  For example, having a flange on the edge of a flat sheet metal part is perfectly fine since it is a linear bend.  But once you model a flange on a bent sheet metal part, the flat pattern output process wont work since it is considered a non-linear bend.

So maybe let us know if you need the flat pattern output or not, and then depending on your answer additional suggestions could be made.

[Anonymous]

Thank you very much, Stephen.  That makes sense.  I will just keep the flat model as it is with an extra half inch on the end and let the fabricator figure it out.  They can run the part through a bead roller after the cuts and main curve are done.  Once I get the part, I can measure and design the cover for the end and send it all off to upholstery.  Mainly, I'm just glad I don't have to keep pulling my hair out on this problem any more!