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ROUND PART FROM FLAT SHEET

Question asked by Scott Cole on May 11, 2017
Latest reply on May 15, 2017 by John Stoltzfus

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I'm not sure if this can be done in sheet metal. I need to take a strip of metal, thin about .060 thick, 12 in long, 2 in wide, two holes in each end so you can bend it into a circle and bolt it together. WHAT WOULD BE THE BEST WAY TO DO THIS?

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Peter Kennedy May 11, 2017 12:17 PM
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I would draw your curve, you'll probably have to use a spline on two planes your thickness apart since you want it to over lap, and then use lofted-bend. You can select the the thickness. After can then extrude a hole through, if you want you can do it in the rolled state or flattened state.
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John Stoltzfus May 11, 2017 12:06 PM
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Sheet metal - overlap the ends..
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Rob Edwards May 11, 2017 12:26 PM
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Hi Scott
sheet metal based on some kind of spiral?
4 partial arcs here - overlapping section concentric, rest tangent

edit: couldn't resist continuing,, in that dodgy metric
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- overlapring.SLDPRT.zip78.2 KB
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- Dan Pihlaja @ Rob Edwards on May 11, 2017 12:26 PM
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  Couldn't you use the Spiral Tool?
  And make the pitch the thickness of your sheet metal
  
  Then extrude/thicken/convert to sheet metal. Or whatever...
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  - John Stoltzfus @ Dan Pihlaja on May 11, 2017 12:29 PM
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    Sheet metal looks a splines and refuses to work, goes on strike etc...
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    - Peter Kennedy @ John Stoltzfus on May 11, 2017 3:34 PM
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      I've used Lofted Bend between two spline sketches on different planes, and it worked fine, was even able to give me a flat pattern as well.
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      - John Stoltzfus @ Peter Kennedy on May 11, 2017 3:37 PM
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        That would definitely be the way to go, I just don't understand why my part didn't throw an error - sheet metals there, just don't flatten..
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  - Rob Edwards @ Dan Pihlaja on May 11, 2017 12:31 PM
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    wasn't sure if sheet can unbend a spiral? + think you need a phd to work out path length of spiral.. beyond me
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  - John Stoltzfus @ Dan Pihlaja on May 11, 2017 12:50 PM
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    I would definitely use this for a sketch controller, in other words create the spline and split into sections, then make it a construction line then add circles that are related with three points, but because of the helix nature you should have at least 4 circle sketches that are trimmed to flow within the spline..
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Tony Cantrell May 11, 2017 12:35 PM
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Here's another way
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- curve SM with hem.SLDPRT.zip79.3 KB
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Wayne Schafer May 11, 2017 2:29 PM
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another way
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- Part4.SLDPRT.zip190.5 KB
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Wayne Schafer May 11, 2017 2:52 PM
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Options galore
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- Round Sheet Metal Part.SLDPRT.zip144.9 KB
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John Stoltzfus May 11, 2017 3:16 PM
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Attached is a 2017 part, I can use Sheet Metal to do the base extrude but it doesn't want to flatten - maybe Frank Ruepp could chime in... I know you can't use any spline sketches, however I used arcs to develop the final sketch...
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- JS-Bent.SLDPRT.zip12.5 MB
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- Frank Ruepp @ John Stoltzfus on May 15, 2017 5:37 AM
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  Hi John,
  
  I had a look at your part and there are a couple of things. Basically you can create two different types of base flanges:
  Base flanges with a closed contour:
  Base flanges with a closed contour are usually flat sheet metal bodies (and this is what you actually did: you have created a very thick sheet metal plate with a very narrow outline). With a closed contour you are sketching the outline of the sheet metal body and the sheet metal thickness gets applied this sketch. In your example you have created a 2 in thick sheet metal "plate":
  
  So basically the sketch contour becomes the top sheet metal face, respectively the bottom sheet metal face. With your approach you can actually create a sketched bend on top of the sketched profile:
  
  To make a long story short: Even though it looks like the real deal, there is a mismatch between what are the top and bottom face and the side walls. In your example the curved faces are the side walls of your flat sheet metal body and it actually should be exactly the opposite way. For the intended geometry the curved faces are supposed to be the top and bottom faces and the flat faces should be the side walls.
  Base flanges with an open contour:
  A base flange with an open contour creates a sheet metal body where the sheet metal thickness gets added to the sketched contour and the width of the sheet metal body is extruded normal to the sketch direction. So I edited your sketch and modified the sketch in order to get an open contour:
  
  In this case the sketch contour gets thickened with the sheet metal thickness and the resulting curved faces become the sheet metal top and bottom faces and the flat faces are the sheet metal side walls:
  
  This way you can unfold the base flange.
  There is a third topic that is relevant to base flanges: Which sketch geometry can be used?
  Possible sketch geometry for a closed profiles can be pretty much everything as long as the sketch geometry is closed. The only limitation is that the sketch may not overlap. But apart from that you can sketch everything you want. You can imagine this as the contour that gets cut by i.e. the laser cutter. So ultimately the complexity of a closed contour base flange is driven by your manufacturing capabilities. If i.e. your numeric control cannot handle splines you should not use splines but SOLIDWORKS does not care if you use splines or not.
  For open contours we only support lines and arcs and nothing else (so no spirals, ellipses, whatever other curves). If you sketch a couple of connected lines SOLIDWORKS automatically adds the specified bend radius to sharp corners what results in a possible limitation that if a sketch line is too short and it would be consumed by the applied bend radii the base flange will fail. Another very basic rule for open profiles is that when you are using lines and arcs or arcs in conjunction with arcs there MUST be a tangent relation between adjacent entities. If there is no tangent relation the base flange will fail. By the way the same rules also apply for the Insert Bends feature.
  Another way to create this type of geometry is to use the lofted bend feature where you sketch the intended geometry in one sketched and in a second step you convert these sketch entities into a sketch on an offseted sketch plane. Lofted bend does not rely on the line arc restriction and you can use spirals, ellipses, curves and other geometrical entities in a sketch as long as the entities are tangent. But you have to be aware that lofted bends use a different algorithm to flatten the geometry and the result might be an approximation (even though in this case the deviation might be neglected).
  
  I hope this has shed some light into the obscurity of sheet metal.
  
  Kind regards
  Frank
  SOLIDWORKS Product Definition Team
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  - BaseFlange.zip24.9 MB
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  - John Stoltzfus @ Frank Ruepp on May 15, 2017 6:23 AM
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    Thanks for the explanation Frank Ruepp
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