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Converting a Solid Part to a Sheet Metal Part

The Convert to Sheet Metal command lets you specify the thickness, bends, and rips necessary to convert a solid part to a sheet metal part.

To convert a solid part to a sheet metal part:

  1. Create the solid part.

  2. Click Convert to Sheet Metal (Sheet Metal toolbar) or Insert > Sheet Metal > Convert To Sheet Metal .
  3. In the PropertyManager, under Sheet Metal Gauges, set options if you want to use a gauge table:
    1. Select Use gauge table.
    2. In Select Table , select a gauge table to use, or click Browse and browse to a gauge table.
  4. Under Sheet Metal Parameters:
    1. Select a face as the fixed face for the sheet metal part.
    2. Set the sheet thickness and default bend radius.
    3. Select Keep body if you want to keep the solid body to use in another Convert to Sheet Metal feature. When cleared, the body is consumed by the Convert to Sheet Metal feature.
  5. Under Bend Edges, select the model edges that will form bends.

    Change the display style to Hidden Lines Visible to make it easier to select edges.

    The rips required are automatically selected and listed under Rip Edges found.

    In the graphics area, callouts are attached to the bend and rip edges if you selected Show callouts in the PropertyManager. You can use the callouts to change the bend radii and rip gaps.

    You can restore the default value by right-clicking the bend edge or rip edge and selecting Restore Default Value.

  6. Under Corner Defaults, set the rip options. To override these defaults by setting options for individual rips:
    1. Under Rip Edges found, select Show callouts.
    2. In the graphics area, click Default in the gap callout.

    3. In the pop-up window, set the rip options.
    4. In the graphics area, right-click and click OK .
  7. Under Custom Bend Allowance, set a Bend Allowance Type and value.
  8. To add relief cuts for the inserted bends, under Auto Relief, select the type of relief cut: Rectangular, Tear, or Obround.

    Tear reliefs are the minimum size required to insert the bend.

    If you select Rectangular or Obround, specify a Relief Ratio.

  9. Click .
  10. Click Flatten (Sheet Metal toolbar) to flatten the part using the bends and rips you specified.

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