• What and Why?
• Sketch
• Creating Weldment
• Custom Profiles

Weldments are for designing frame made from tubes of a common cross section. Using weldments makes it easier to design these frames because you can rough out the frame shape and make all the component members in one part. This improves performance in addition to making design easier. Drawings of weldment parts can also have a cut list table listing what stock to cut and to what lengths to cut it to.

To make a weldment start with a sketch (or multiple sketches) that has lines for each member of the frame (you don't have to use all the lines of the sketch). The sketch can be 2D or 3D depending on the application. By default the members will be centered around the lines although this can be changed.

Use the "Structural Member" command to start a weldment.

The "Standard" "Type" and "Size" to select the type of profile you want. This example uses a custom profile, something we will typically use, which will be explained later.

Groups are used to apply settings like profile location and angle to members in that group.

Things to note:

• The trip order is determined by default based on when the groups are made.
• Solid works automatically extends members to be flush to one another.
• Members in groups have to be either all connected or all disconnected.
• You can change the trim order by clicking on the nodes where members meet. Members with a higher trim order number get cut to make way for members with lower numbers.

As we saw above profiles are sorted by "Standard" "Type" and "Size". When creating a custom profile the standard is file the template file is under. The Type is the name of the template file name. The Size is the configuration name.

If this doesn't work for your situation

The Standard and Type can both be folders the profile is under (Standard>Type>Size.sldlfp). Don't be lazy and do this when you can do a configuration as this would make it hard to add similar profiles.

Use one sketch make the custom profile that you want use the equation manager to change the profiles dimensions in different configurations. Also assign a file configuration property "Description" that is the same as the configuration name or size. Assign the material the profile is made from

With the sketch selected do file>save as and save the file as a "Lib Feat Part" .sldlfp file. Save the file to the appropriate folder and the custom profile has been created.