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.
Solved! Go to Solution.
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.
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)
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.
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,
P.S. I noticed the icon of the derived part is different on mine to the no loft files, could that be an issue?
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.
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.
P.S. I'm using Inventor 2012 if that makes a difference.
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.
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.
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