Outside Dimensions for non-90° Sheet Metal bends in SOLIDWORKS

Article by John Lee, CSWE updated February 22, 2023

Article

When detailing a bent/formed sheet metal drawing, and generating a flat pattern, it is important to confirm that the flat pattern size is accurate.  A practical way to do that is to use the Bend Deduction formula which relies on OD’s (Outside Dimensions) which can be physically checked with calipers when doing a bend test or at inspection. This is easy enough for 90° bends:

outside dimensions of 90 degree bend

Outside dimensions of 90 degree bend

For non-90° bends, things get more complicated. Fortunately, there are some time-saving tricks in SOLIDWORKS:

Case: OD of edge to >90° bend

For this we want to measure the OD from the thickness face created by the punch/shear/cutter to the tangent arc of the bend, just like would be done with calipers (see picture below). To speed that up in SOLIDWORKS, hold down the Shift key while selecting the arc, to ensure that the dimension is to the apex of the arc rather than to its center point.  This saves the step of having to adjust the dimension afterward in Dimension Properties > Leaders > Arc Condition

outside dimensions of edge to 90 degree bend

Outside dimensions of edge to 90-degree bend

Case: OD of edge to <90° bend

Although it is a challenge to measure the OD physically with any accuracy using calipers, due to the virtual sharp being located off the part (see pictures below), we can still dimension it in the drawing and use it in calculating the flat pattern length.

  1. Start the dimension from the thickness face created by the punch/shear/cutter
  2. Right-click one of the flange edges > Find Intersection
  3. Left-click the other edge flange to complete the Find Intersection Note that a virtual sharp is created. The dimension is actually measuring to this virtual sharp, where the flanges would have intersected if the bend was sharp instead of rounded.
  4. Place the dimension.

Case: OD between bends

When generating an OD between two adjacent non-90° bends, one more trick is needed to ensure that the dimension is taken parallel to the flange face, rather than projected or skewed in some way. For this it is helpful to sketch a short line (see picture below). We then dimension from that line.

OD between bends

OD between bends

The role of the short line is twofold:

  • It is given a perpendicular relation to the flange whose OD we’re dimensioning, ensuring that the OD is parallel to that flange. To do that, Ctrl-select the flange face and the sketched line > add a Perpendicular
  • One of its endpoints is given an intersection relation to the two flange faces adjacent to the bend. To do that, Ctrl-select endpoint, edge 1, and edge 2 > choose Intersection. This locates the endpoint in exactly the same position as the virtual sharp would be, ensuring that the OD measures the correct distance.

Note that if dimensioning OD between two adjacent <90° bends, we can sketch that line at one bend and use Find Intersection at the other:

OD between 90 bends

OD between 90 bends

Learn more tips and tricks in our SOLIDWORKS Sheet Metal training course!

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John Lee, CSWE

John Lee is inherently lazy in that he prefers to work smarter - not harder. A CSWE with fifteen years of experience using SOLIDWORKS and a background in mechanical design, John has used SOLIDWORKS in various industries requiring design for injection molding, sheet metal, weldments and structural steel.