Creating Primary Members based on Points in SOLIDWORKS 2020 Weldments

SOLIDWORKS 2020 provides you with additional tools and control options for creating primary members in weldment structures. In this article, we are going to review these new options in SOLIDWORKS 2020 for primary members based on “point and length”, members “between points”, members using “up to point” end conditions and members based on “direction”.

When specifying Point and Length, you can set a direction for a primary member by selecting a reference which is a sketch entity. The member extrudes in its direction and you can also reverse the direction of extrusion. As an example, consider the part below which is made of a few sketches for the reference geometries.

Starting sketch for primary members

To start the primary member command, click on Insert > Structure System > Structure System to get into the structure system mode.

Starting the structure system mode

Once you are in this mode, you need to click on Insert > Structure System > Primary Member to start adding primary members to your weldment part. It’s a good practice to Pin the property manager of primary member command to be able to add multiple primary members.

Creating the first primary member

Now, you can select the desired profile from the profile tab in the property manager and then switch to the member tab:

Specifying the profile for the primary member

For our first member type, point-length member is selected:

Creating a point-length member

We select the 4 points from our sketch and specify the length of the members and click OK to confirm.

First set of members using the length end condition

For the next members, we change the end condition of the members from length to point and select the start and end points of the new structural members. SOLIDWORKS will create members between the selected points.

Creating members between two points

The next end condition to explore is “up to point”. Using this end condition we are creating 3 additional members up to a specific point.

Creating a members using the up to point end condition

And the last end condition is to create an structural member based on direction. In the member tab, under end condition we select length and click in the box for member direction. For the direction of the member, a sketch line is selected. The length of the member, also needs to be specified.

Creating a member using the length end condition and choosing a specific direction

Want to learn more about Weldments?

Attend our SOLIDWORKS Weldments training course either live online or in a Canadian city near you.