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We've been trying to "flat Pattern" items using "sheet metal" here in our wonderfully sunny office and have failed terribly. Following the instructions given in the help topics just make the "flat pattern" button click to show us a face of the object rather than laying it out for fabrication.
We've tried this on trays / eccentric reducers / random objects drawn to try and get it to work.
No Joy!
Could anyone please tell us how it is done and suggest ISBN numbers of good Inventor tutorial books that cover more advanced things than "how to print and turn the computer on"
1) when creating the part I always start with a sheet metal template
2) my parts are simple, only being flanged "UP" not "DOWN" so from the base surface my thickness is always "DOWN" not the default "UP".
3) I add flanges as required, position holes, notches etc.
4) click the button and get my unfolded flat pattern
Try something simple. When testing I always start with a rectangle sketch, create a flat plate part, add a hole somewhere, then flange up two adjcent edges.
No problem with me?
New part from sheet metal template
Sketch and dimension a rectangle
Return to part
Select sheet metal style
Select face
Select direction
Select flange
Select two adjcent edges on top face select UP and apply
Select face
Select Flat Pattern
We've managed to get it creating very simple boxes. But not the boxes we require - more practice required!!
Could anyone tell me how we'd go about creating a flat pattern view of an eccentric reducer cone? (I don't seem able to attach a drawing right now but imagine one 139.7 mm to 129 mm) If this even possible? Would we need to create a "cut" in it or does Inventor do this automatically?
If you want to attach an inventor file you have to zip it first. It is also a good idea to pull the end of part marker to the top of the browser efectively suppressing all features in a part. This cuts down on file size.
Parts must have uniform thickness. The sheet metal
parameter THICKNESS must be equal to the thickness of the part. If you have
"converted" a non-sheet metal part to sheet metal, this is often over
looked.
Parts must have a rip (or split) that would allow
the model to flatten (just as a physical model would require this opening or
gap). If this gap doesn't exist: the part won't flatten.
Formed parts will not (currently) flatten. The part
must decompose into: flat faces, bends or flat faces that have been rolled.
Anything that would require die-forming will not flatten in the current
release.
-- Gary R. Smith Autodesk Manufacturing
Solutions Division Technical Publications - Subject Matter
Expert Portland, OR 2.33GHz 2GB IBM ThinkPad T60p; XP pro SP2 ATI
Mobility FireGL V5250 driver: 8.293.1.0
-- Dennis Jeffrey, Autodesk Inventor Certified Expert Autodesk
Manufacturing Implementation Certified Expert. Instructor/Author/Sr. App
Engr. AIP 2008 SP2, AIP 2009 PcCillin AV HP zv5000 AMD64
2GB Geforce Go 440, Driver: .8185 XP Pro SP2, Windows XP Silver
Theme http://teknigroup.com
If
you want to attach an inventor file you have to zip it first. It is also a
good idea to pull the end of part marker to the top of the browser efectively
suppressing all features in a part. This cuts down on file
size.
"Mastering Inventor 2009........" is now available from Sybex,
Wiley & Sons and Amazon. The Sheet Metal chapter was written by Autodesker
Seth Hindman.
-- Dennis Jeffrey, Autodesk Inventor Certified Expert Autodesk
Manufacturing Implementation Certified Expert. Instructor/Author/Sr. App
Engr. AIP 2008 SP2, AIP 2009 PcCillin AV HP zv5000 AMD64
2GB Geforce Go 440, Driver: .8185 XP Pro SP2, Windows XP Silver
Theme http://teknigroup.com
Morning
All. We've been trying to "flat Pattern" items using "sheet metal" here in our
wonderfully sunny office and have failed terribly. Following the instructions
given in the help topics just make the "flat pattern" button click to show us
a face of the object rather than laying it out for fabrication. We've tried
this on trays / eccentric reducers / random objects drawn to try and get it to
work. No Joy! Could anyone please tell us how it is done and suggest ISBN
numbers of good Inventor tutorial books that cover more advanced things than
"how to print and turn the computer on" Many thanks!!
Clara.
We have, from the beginning, been applying the uniform thickness in the "sheet metal styles" area. We also cut the model (you say "rip or split" are these technical function on Inventor or just another way of saying cut?) to indicate where it should be flattened.
By formed parts do you mean something that has, for instance, been lofted and then shelled? I can't think of another way to create a eccentric reducer unfortunately but an concentric reducer flat pattern works fine with a revolve. Any suggestions as to how I might over come the need to flatten the eccentric reducer?
Thanks. I hadn't realised that a file at 319.00 KB would need zipping.
I've very quickly bashed together a copy of an eccentric reducer - to the same measurements as the one we want to achieve to be able to flat pattern it.
How would we go about drawing such an item so that it can be flat patterned? It seems that lofting and shelling would not be permitted.
Many thanks for your assistance on this - it's driving the office, and our fabricators, insane.
Unfortunately it seems that a zipped .ipt at 120KB wont upload - quite possibly it's my computer security settings not allowing me. Agh. Thank goodness it's Friday.
Post back here when it's uploaded. Currently this NG is having
problems with attachments.
-- Dennis Jeffrey, Autodesk Inventor Certified Expert Autodesk
Manufacturing Implementation Certified Expert. Instructor/Author/Sr. App
Engr. AIP 2008 SP2, AIP 2009 PcCillin AV HP zv5000 AMD64
2GB Geforce Go 440, Driver: .8185 XP Pro SP2, Windows XP Silver
Theme http://teknigroup.com
Thanks.
I hadn't realised that a file at 319.00 KB would need zipping. I've very
quickly bashed together a copy of an eccentric reducer - to the same
measurements as the one we want to achieve to be able to flat pattern it. How
would we go about drawing such an item so that it can be flat patterned? It
seems that lofting and shelling would not be permitted. Many thanks for your
assistance on this - it's driving the office, and our fabricators, insane.
Unfortunately it seems that a zipped .ipt at 120KB wont upload - quite
possibly it's my computer security settings not allowing me. Agh. Thank
goodness it's Friday.
Yes, when I said "rip" and "split" I meant the same
as your use of "cut". We have been talking a lot lately (internally) about a
"rip" - I meant "split" in the sense that a part that forms a "tube" for example
would have to have the same opening (call it what you will: cut, gap, split,
rip, whatever...) in order for it to flatten using the flat pattern
functionality.
By "formed" part, I meant anything that you
can not fabricate using a straight die in a press brake or a set of straight
rollers.
I've never seen any previous postings by Naethan
Cadavarice and I have no idea how he would have any insight into what we have
working internally or what we are planning.
Inventor will of course flatten cylinders and cones
as I intended to convey with my statement about flat faces that were
rolled.
Inventor will not currently flatten a part that was
created using lofts and shells (even if all the resulting walls are the same
thickness) presuming the lofted shape transitions from one shape to another
along a non-straight path.
