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Hi ing.frison,
You can also create a copy of the original part and then mirror the entire part at the part level, without the need for deriving the part. Sometimes it's preferred to use the derive method, but other times this method works just fine. There's an example at this link:
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
Dear JDMather,
this way I would loose the associativity with my "folded model", so it's absolutely "no-go".
Dear -niels-,
to this point I was already (see my first post in the previouse page). Of course it's a valid walkaround, but it's not perfect.
Today I finally got to the point. thanks to a tip from a very good and very expert friend from Italy. Here's how.
First of all: it is not possible to derive the flat pattern of a sheet metal component. It's official now.
...but... 
...we can create an iPart with a member that is "unfolded".
With this iPart we can build an iAssembly with the unfolded member/members...
...and we are done: that's how to make the drawing of the "unfolded assembly", without having to bother about multiple files or non-matching iProperties 
(of course you should be quite good with math and trigonometry to match all the angular joints that become flat joints, especially if your angles are not simple fractions of 360°, but that's absolutely a minor issue!!)
Please mark this response as "Accept as Solution" if it answers your question.
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MaX - Autodesk Inventor rejected certification!!!
@jtt1301 wrote:What information in the table do you put to make a member be in the flat (unfolded)...i am trying to make an assembly from two folded parts in their flat state.
enable or suppress the "unfolding" feature(s) that will flatten your model
BTW
That was one of my first attempts a long time ago...
...working in a business where we constantly need to be able to represent cylindrical/conical stuff on a flattened layout, I had some other and better ideas in the meantime. Unfortunately I cannot post images or drawings because I don't own the intellectual property of the product (but I own the intellectual property of the solution 😉 ).
Point 1: flat patterns cannot be assembled. The best we can do is to assemble a derived sheet metal part that has been flattened, if we are good with handling origins.
Point 2: sometime there is no way to make a flat pattern (CASE 2) but you might still need a flat representation
Point 3 (this should also be mentioned): this task in the 2D world was quite easy. Unfortunately with the upcoming of 3D modeling programs it has became a real mess!!!
The strategy I'm going to describe will give you a possibility to solve this issue in the 3D modeling environment. The only other alternative: make a DWG with AutoCAD and forget about associativity.
THE CASE (1)
In the heat exchanger business, suppliers often like to have a flat representation of the vessel innen plate with the position of all guiding plates of the heating chamber. They mark the position of the plates with a marker in the flat state (easier to measure 😉 ), they roll the main part, so that they find easily the right place where to weld each guiding plate once the main part of the vessel is rolled (second 57 of the video in the next example will give you a visual idea).
This image is an example where the guiding plates are replaced by a half pipe, but the basic concept stays the same and at least we can see the pipe.
THE CASE (2)
In certain cases we have some agitators for the inside of such machines, where all shovels/pins/mixing blades have a "non really regular" position (the need comes from "process specific" issues, but the arrangement can be very strange, or "very skew" if we want to call it like that). Long story short: take a look at second 2:17 (and also 1:10) of this video to see what I mean:
https://www.youtube.com/watch?v=H-0ZUVSjirg
those pins are NOT on a rectangular pattern: they are on a skewed rectangular pattern (once linearized) because if we measure with X the distance of each pin from the shaft bearing there are no 2 pins with the same X
Also in this case the producer prefers to have a "flat view" of the shaft itself and of the shaft assemby to understand how and where each element should be mounted (yes, they are also not all the same with different angles and so on).
THE SOLUTION (currently the only reasonable that I could find)
Leave the iFactory idea of my previous post: I was driven on the wrong way by a good friend who probably never used inventor for "production purposes" (it worked, but it was a mess, and I repeat: he's a good friend 😉 ).
1. In both cases I need to have a flat representation of a part/assembly that WILL NOT be produced
2. Ideally all measures of the flat elements should follow the real one (guiding plates position, pins/blades twisting angles...).
3. you need to be good with math (in particular trigonometry)
4. you need to be good with linking parameters (only parameters, so no need to derive)
5. you need to be very sistematic in naming (and commenting) parameters
6. you need to be inventive
Step 1:
create a simplified flat version of your main component being driven by parameters derived from the REAL component.
.for the drum innen sheet: make it flat, or derive it as sheet metal and unfold it depending on how precise you want/need it (at least now you still have the option to do it). So that you can mount the flattened part.
.for the shaft: no way to derive it. You need to rebuild a flat element where the position of the holes (pins are screwed into the shaft) is driven by parameters derived from the real shaft, and put your best trigonometry at work to linearize those values and skew the patterns properly.
Step 1b:
In case you have a drum with some round guiding plates (second 0:57 of the video, grey elements on the teal sheet metal), you need to build new elements deriving the values (thickness, width and arc) from the real ones. Of course your "arc" parameter will have to be converted into the lenght of the linearized element. This could be a minor case but in our business it always happens
Step 2:
Now you have the basis to build your flat assembly (linear guiding plates, pins and shovels will be actually the same, but mounted onto a flat component; rolled guiding plates will be substituted by their linearized version).
Step 3:
And here comes the trick: this flat assembly should be linked to the mounting parameters from the REAL assembly.
In some cases values can be simply reused (twisting angle of a blade), in other cases they will need to be linearized (the polar position of the guiding plate n°3 will have to be converted to a distance that will place the guiding plate n°3 at a certain offset from the edge of the flat element).
Step 4:
Now it's the right time to start playing with the BOM of the FLAT_assembly.iam so that you position numbers will match your REAL_assembly.iam
I know, it's a little bit annoying but at the end of the story you'll be happy that everything works fine. and that position numbers are the same.
This approach will generally work better than trying to build an iFactory, where you have to do the same job with the teasing additional task of suppressing and re-enabling constrains depending if you are in the rolled or in the flat assembly.
If you have been diligent at the end of the story your FLAT model will reflect the REAL one, your supplier will be happy because he will be able to understand the drawing, your supervisor will be happy because your modelling strategy is safe and your boss will (should) be happy because you solved a problem that nobody else managed to solve 🙂
NOTE:
It's your decision whether to place "mounting parameters" in the REAL_assembly.iam and link them from the FLAT_assembly.iam, or placing those parameters in the REAL_shaft.ipt and link them both from the REAL_assembly.iam and from the FLAT_assembly.iam
The former strategy has the advantage that you can see immediately the effect of changing one value in the REAL_assembly.iam, the latter has the advantage that circular dependencies are better avoided (linking IAM parameters from IPTs is normally a safer strategy than linking from IAMs. Linking IPT patameters from IAMs should be used only for emergencies and as the very last resource).
CONCLUSION
What to say... honestly this is one of the toughest challenges that I took in the past couple of years, but after a little bit struggling at the beginning we got to a functioning solution that we keep reusing each time we end up in that situation.
I hope it helps 😉
Ok, so the second idea that came to my mind (the short and easy) was that "maybe" the command "fold" could bend something not on the "sheet metal" direction.
Trash.
We don't need sheet metal for this, just some math 🙂
I would solve it this way: any change you will perform in the BarBENT.ipt will generate a change in the BarFLAT.ipt
You have the "blank lenght" of the bar in both parts, so that you can use it for your BOM or whatever (actually if you only need the blank lenght for the BOM you don't even need the flat bar model).
Only parameters you have to play with according to your experience are the position of the 2 neutral planes of the 2 different types of bends (I don't know realistic values, sorry). Whatever you change, the flat bar will be driven by the bent one.
Check the distances of the holes from the rod ends, and enjoy!! 😉
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