Loft to Flat Pattern

[Winnovations]

Attached is a sample

My goal here is to take the curved surfaces of the Loft object & retrieve a flattened profile of the face.

1 profile per face is the final goal - not one completely flattened profile.

Any suggestions?

[JDMather]

Have you tried constructing with the sheet metal tools?
Also, I don't generally mirror lofted features as you have done as the results are probably not as intended.

[Winnovations]

I have expiramented with sheet metal tools - but not with great results (or any)

the mirror was just to show final shape - not really necessary (just a shortcut)

[coreyparks · Accepted solution]

Take a look at the attached files.  I have used the derived part so I could keep the base part for modifying and then the flat patterns would update automatically.  The use of the loft as you had it wouldn't work for this as the curved surfaces were warped a bit when created so you can't flat pattern them.  I always try to create the parts with simpler extrudes and such before I resort to lofts, they can be hard to control if your not paying attention.  Besides the part I did had less sketches than the lofted one anyway.  Hope this gives you some ideas on how to use the sheet metal tools a bit more.

[Winnovations]

Thanks Corey,

Your information was just what I needed to get started & get the desired end results.

RB

[oak_roberts]

I'm also having trouble flattening derived components, my goal is the same as Winnovations to flatten the profiles, just a different shape, to flatten the 4 sides individually so i can export the flattened sketch to a laser cutter to cut out the patterns that i would then stick to the ribs i have already made.

I tried deriving the surfaces only into a new sheet metal part, deleting all but one face, thickening and lastly flattening, but it does not flatten. 

I've also tried sweeping a straight line along a curve to produce a surface rather than lofting with the same results.

Am i missing a proccess that gives the part an 'unfold refferance' or something?

Any help would be greatly appreciated,

Regards, Oak.

P.S. I noticed the icon of the derived part is different on mine to the no loft files, could that be an issue?

[Winnovations]

Oak,

We are actually doing something similar (boats)

 -  Before you tell the part to unfold, you have to change the thickness of the part to match the unfolding thickness

-  On the sheet metal tab - the last or next to last icon is the setup or defaults icon.

- first - add a variable (called THK)

- next use the setup and uncheck the box "Use Thickness from Rule"  and change the Thickness box to THK

- I add the THK variable in the original part so I can change material thicknesess down the road if I need to and bring in the variable when I derive the surface to extract.

- when you thicken the surface - use THK as your thickness & it should work 🙂

I got your "extruded attempt.ipt" to work using this method.

Let me know if I can help more.

RB

[oak_roberts]

Thanks for the reply, I've tried but am struggling with adding the variable.

What i tried was adding a user parameter called THK of 1.5mm, then changing the the sheet metal defaults to list parameters -> THK (it seems to drop in a dimension 1mm smaller "THK0.5 mm" but is red and won't accept. Am I barking up the wront tree, with adding a user parameter, i just can't find where i add a variable.

Thanks, Oak.

P.S. I'm using Inventor 2012 if that makes a difference.

[Winnovations]

Oak,

Here is your file that I modified.

first I added THK as a variable (and set it to 0.5mm)
next I changed the "Thicken1" to THK
then I changed the file to a sheet metal part.
I then changed the setup/ defaults dialogue to unchecked box & THK in the thickness box.

I then tested the file by unfolding it.

I think your problem is to completely remove the default entry in the thickness box & manually add THK.

RB

[oak_roberts]

I'm half way there! I've succeeded in unfolding a new file (attatched) but I can't on the full hull design, it brings up an error message, but I can't spot the what it's making a fuss about.

Thanks again for your help! Oak.

[Winnovations]

Oak,

Here are a couple of things that I have learned (the hard way) in making flat patterns.

I'll use "from existing.ipt" as a reference

when you do a sweep (SweepSfr1)- make sure you choose "parallel" & not "path"  -   path creates a complex compression curve that cannot be created.  If you choose parallel the curve created can be seen on one existing plane.  (more on this below)

Your sweeps would be better as an extrude.  I think this would solve most of your issues.

The way the unfold works - if you can see the curve along a plane, with no twisting, then the part will unfold.  A twist will work only if it is between two straight lines.

I changed your file - I extruded Sketch 17 & 18  & suppressed Sweeps 1 & 2.  the parts will now flatten.  

maybe this will get you the remainder of the way

RB

[oak_roberts]

Sorted!! Thought it was that I'd used splines, but then saw your reply and attached file. Cheers for the details on sweeping, I could probably do with reading some in depth articles on certain tools as I think thats where I'm lacking most being self taught.

I'll now spend days trying out twisted flattening, if I can get that working it really will open some oppertunities for some really nice shapes! I'm guessing a loft between 2 lines along a rail?

Thanks very much for all your help, much apreciated!

Oak.

[Brad-Lakeland]

I am also struggling to get my loft to flat pattern, I have tryed your method and still have no result, any chance you could have a look at where i am struggling ? and give me some well needed feed back ? I hope i have attached the file correctly

[coreyparks]

Inventor can only flatten things that are bent in one direction.  When you have something bent in multiple directions it can.t calculate a flat pattern.  So, something that gets formed into say a dish shape, however minor, will not work.  The bow of your hull section is bent in multiple directions so it will not be able to be flattened.

[Brad-Lakeland]

oh ok that makes sense then. So is it possable to achieve that shape in invnetor as flat pattern, my guess is no ?

thanks for your help

[Alexandros.Georgiou]

i am also trying to flatten this but i canot can you help me please ?

[JDMather]

@Alexandros.Georgiou

There are so many issues and this is such an old thread that I recommend you start a new thread on your problem.

Install the latest Service Packs and Updates for your version of Inventor.

You have a surface body rather than a solid body.

You have used splines where arcs can be used.

After these issues are resolved - then an advanced trick with MeshMixer might be required, but first some foundation stuff needs to be addressed.

[JDMather]

@Alexandros.Georgiou

I meant to add - this thread has been marked Solved, so you might get more attention by starting a new thread and link back to this one to show what you have already attempted.