You can create your own
weldment
profiles
(external link to YouTube.com) to use when creating weldment structural
members. You create the profile as a library feature part, then file it in a defined
location so it is available for selection.
Additional weldment profiles are available on the
Design Library tab
. Under
SOLIDWORKS Content
, in the
Weldments folder,
Ctrl +
click items to download
.zip
files.
To create a weldment profile:
-
Open a new part.
-
Sketch a profile. Keep in mind that when you create a weldment
structural member using the profile:
- The origin of the sketch becomes the default pierce
point.
- You can select any vertex or sketch point in the sketch
as an alternate pierce point.
-
Close the sketch.
In the case of multiple sketches, select the specific
sketch from the FeatureManager design tree before you save it.
-
Click .
-
In the dialog box:
-
In Save in,
browse to install_dir\data\weldment profiles and select or create
appropriate <standard> and
<type> subfolders. See
Weldments - File Location for Custom
Profiles.
-
In Save as type,
select Lib Feat Part
(*.sldlfp).
-
Type a name for Filename.
-
Click Save.
The name that you give to the library
feature part appears in the Size list in the Structural Member PropertyManager when you create a
weldment structural member. For example, if you name the profile
1x1x.125.sldlfp, then
1x1x.125 appears in
Size. If you name the
part big.sldlfp, then
big appears in Size.