I'm new in world of Inventor 2012. Some months ago i got a job in a company that is using Inventor 2012. From couple days i'm trying to figure what is wrong with some of sheet metal parts. For some reason they look corrupted after a short period of time.
Sometimes it helps to rebuild the part but it helps only for a short time.
Maybe someone can take a look on this and help me with this issue.
Solved! Go to Solution.
Can you attach the part file that this file was derived from?
I would not use Splines to create a sheet metal part.
If I did use splines - 2-point splines could be used to replace these splines.
Do not use Split to trim sheet metal parts - you can see that the result is incorrect by changing the 3mm thickness to 300mm and then go to Flat Pattern (I do not understand the purpose for the Unfold/Refold in your feature tree).
I would do the curves as tangent lines and arcs.
Or I would do them with 2-point splines using the multi-node splines only for reference in adjusting the curvature.
Workplane1 is not needed - is is the same as the XZ plane as far as creating Sketch2 and using Sketch2.
I would do a trimmed extruded surface and then thicken rather than use Split features that return incorrect sheet metal (sides not perpendicular to flat).
The unfold/refold feature is added for future use. I need to place some features in flat state later. This part is a side shell plate of a boat and i would like to have it as a flat pattern for CNC cutting. I agree about workplane1, it was no necessary. But i'm not sure how to get this shape without using Split.
Last i can try to replace splines with something else...
... But i'm not sure how to get this shape without using Split....
Extrude Surface (rather than Contoured Flange feature)
Trim the surface.
Thicken the surface.
I have done it like you wrote. It seems that it is OK now, but i found this same problem with Sweep. After a while they look corrupted but after rebuilding everything seems to be ok. Other thing is that some times it take long time to calculate sweep. Is it possible that it happens when i'm using splines as a path?
I,m attaching a smaple sweep that cause some problems so if you have some time maybe you can look on it.
Previously i was working in Solidworks 2013 and i don't remember such problems.
I would use the intersection of 2 2D sketches to create your 3D path sketch.
How would you edit that?
It is a lot easier to edit 2D sketches.
I know about creating 3d intersection curves.
I don't need to edit this patch. Once it's created it is not necessary to edit it.
This 3D path is taken from a part that will not change. I'm just curios why it takes long time to compute this sweep.
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