Create Sheet Metal Parts from Solid Parts

Create Sheet Metal Parts from Solid Parts

This section explains how to create sheet metal parts from solid parts either imported via intermediate files or created directly in IRONCAD.

Shapes Convertible to Sheet Metal Parts

Example:
Shapes Convertible to Sheet Metal Parts.

Both solid parts created in IRONCAD and those imported via intermediate files can be used.

Solid parts in sheet metal state (box state)

Both shelled solid parts created in IRONCAD and box-shaped solid parts imported from intermediate files can be used.

Procedure:

[1] To convert a solid part into a sheet metal part, then select [Solid part to Sheetmetal part] in the [Sheet Metal] tab .


[2] Since solid parts are created as if already welded, it is necessary to define bend and split sections in order to convert them into sheet metal parts.
To create bend and split sections, configure the items in the property window:
  1. Face Selection: Select the base face
  2. Bend Edge: Select the edge to bend
  3. Default radius: Set the bend radius for the edges
  4. Default lip: Set the gap after bending
  5. Property Options: Set material/thickness (change from the standard stock)
Board thicknesses not in standard stock are set to [Custom Stock].



[3] Order of Face and Edge Selection.
Select the face (①).

Select bend edges (②③④⑤).
 ※There is no required order when selecting edges adjacent to the base face.

Then, select bend edges (⑥⑦).
Bend edges ⑥⑦ cannot be selected before ②③④⑤. Select them after selecting the bend edges adjacent to the base face.


Once the properties are set, the part in the scene will appear as shown in the image:


Light Blue = Base face (topmost face)
Blue edges = Bend sections
Yellow edges = Split sections
 ※Yellow edges are automatically determined and applied after bend edges are selected.

[4] After executing the command, the solid part is converted into a sheet metal part.

The original solid part remains in a suppressed state.

Close-up of the Base Face

The bend and split sections are created.

Now that the part is a sheet metal part, unfolding operations are also available.


Shapes That Cannot Be Converted to Sheet Metal Parts

Case 1: Parts with holes or non-planar surfaces
Example: Block parts with holes


Faces with holes can be selected, but the edges around the holes cannot be selected.


The hole geometry is not created in the sheet metal part, and the hole remains as an open cut.

Because 3D hole shapes cannot be created as part of the sheet metal part, add them manually afterward.

Case 2: Pyramid-like parts with multiple steps

Split sections from the second step onward cannot be recognized.

Case 3: Parts with many freeform surfaces or small surfaces, or overly complex shapes

Split edges adjacent to the base face may be recognized, but due to multiple surface creations, the system cannot determine where to split, making edge recognition or selection impossible.

Case 4: Parts with fillets or chamfers from the beginning

Please remove fillets and chamfers before converting to sheet metal.

Case 5: Sheet metal parts added via welding, etc.

Flat and cylindrical sections must be made into separate sheet metal parts.
They cannot be converted as a single part.

Others:

Some parts created with freeform surfaces or highly complex geometries may not be supported.

We will introduce how to operate elements that can be changed to sheet metal parts.
Please refer to the following video.

IC-035

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