Parametric Flat Pattern of Bent Rod/Tube in SOLIDWORKS

SOLIDWORKS Sheet Metal tools provide the ability to obtain the flat shape from a bent part.  The flat length of each bend is based on defined parameters.  This can be defined with K-factors, Bend Allowance or Bend Deduction.  For more information on Sheet Metal calculations, check out the following articles:

• What Are Bend Allowance, Bend Deduction and K-Factor?
• Calculating Bend Allowance, Bend Deduction, and K-Factor
• Bend Allowance, Bend Deduction and K-Factor Tables in SOLIDWORKS

When it comes to bent pipes or rods, Sheet Metal tools cannot be used as it’s no longer uniform thickness through the bend.  The use of SOLIDWORKS Weldments or Routing provides an easy way to generate the design and determine the total length of each piece.

While it’s not common to show the flattened state of a pipe or rod, this could be accomplished with a sweep feature that is parametrically linked to the original shape.  If needed, we could specify a “bend factor” similar to a K-factor to define the neutral location of the bend.  Then the arc length can be used to define the length of each bend section.

Take a paperclip as an example.

Paperclip example model

We can define a bend factor as a global variable and multiple this by the size of the profile to get the position of the neutral axis, in this case a factor of 0.5 with a profile size of 1mm.  An offset from the inside of each bend with this dimension gives an arc.  The length of this arc gives the final length of the bent region.

SOLIDWORKS Equation for Arc Position

SOLIDWORKS Reference Dimension of Arc Length

Create a new sweep feature made up of sketch segments for each region.  The straight sections are linked as equal to the original geometry.  The length of the bent regions are linked to the reference arc length dimensions.

SOLIDWORKS Flat Pattern Bend Length

Create separate configurations for the original body features and the flat pattern sweep to obtain a fully parametric model that updates the length as the geometry changes.  A drawing view can be created with centerlines defined between edges of the bent regions.

SOLIDWORKS Flat Pattern

SOLIDWORKS Flat Drawing View

If the dimensions and locations of each bent regions are not important, you could obtain the overall path length and then simply reference this dimension for the length of the new sweep feature.

SOLIDWORKS Path Length Dimension