Thursday September 13, 2018 at 4:07pm
For the final part on this blog series Will explains the process of importing a DWG of a sheet metal flat pattern and bending it into it's finished state inside SOLIDWORKS.
Introduction
For the final part on this blog series Will explains the process of importing a DWG of a sheet metal flat pattern and bending it into it's finished state inside SOLIDWORKS.
Importing a DWG File and Using a Sketch
Bend
The DWG file format is used for storing
two and three dimensional design data. A number of CAD packages use this as a
native file format including AutoCAD and DraftSight. Importing and converting a
DWG file into SOLIDWORKS can allow you to create folded sheet metal parts from
a 2D sketch.
1) Open
the DWG file from inside SOLIDWORKS and the following menu will appear:
2) Select the “Import to a new part as:” and “2D sketch” options and click “Next”
3) Select Next on the following “Document
Settings” menu. Note that various settings may be changed in this menu
including “Import Layers”
4) On this
“Drawing Layer Mapping” menu the origin of the drawing may be repositioned with
the “Define Sketch Origin” button.
You may also delete unwanted entities in the drawing with the “Remove Entities” button
5) Select the “Finish” button once the entities
editing is finished
6) If the
sketch that is created is correct then confirm the sketch in the “Confirmation
Corner”
7) Now apply a Base Flange Sheet Metal feature to the
sketch and set the options of the part as required. These options include Sheet
Metal Parameters, Bend Allowance and Auto Relief
8) Create a
sketch on the top face of the part and Convert
Entities on the construction lines of the original sketch which represent
the bend lines. These lines may be hidden in the new sketch so “Show” these.
The lines will allow a Sketched Bend
feature to be used and therefore allow the part to be folded
9) Select the
new sketch for the desired bend line/lines and then select the “Sketched Bend” feature from the Sheet Metal tab. Note that separate
sketches and separate sketched bends must be created in order to create bends
with varying properties such as Bend Angles and Bend Positions
In the Feature Manager select the “fixed face” of the part. A preview will
appear and show how the bends will be made once confirmed. A number of bend
parameters can be changed from this menu including the Bend Position,
the Bend Angle and the Bend Radius
10) Once the
desired parameters have been set, confirm the Sketched Bend
William Blower