We’re going to start making lumber profiles to be used as weldments and smart blocks (in later articles). With a regular SOLIDWORKS part template open we’re going to modify this heavily. I’ll start with adding in a material of Spruce. If you don’t know how to create a SOLIDWORKS custom material check out our article.
I’m going to create a basic rectangle on the Front Plane. I’m using the Center Rectangle option with the From Midpoints selected.
I prefer having my reference geometry running vertical and horizontal rather than on angles. I’m going to create many configurations, but I’m starting with the smallest lumber profile first.
From here I’m going to modify some of the options. Tools > Options > Document Properties > Virtual Sharp and I’m changing this to the Star option.
I’m accepting this and going back to the sketch I want to add in a Virtual sharp to all the corners.
At this point we’re done with the sketch but will need to add to the File Properties. Your company may have a standard on what Properties they want shown, as an example this is what I have. Since we’re adding in configurations, it’s important to remember to add in Configuration Specific Properties.
I’m going to add in Length and Height and link these to the dimension in the sketch. I do this is for the first configurations so that all the configurations that follow will have the same format. If these Properties are created after the configurations, then we have to manually link them.
Now the lengthy part of this is adding in the configurations. A few ways you can do this is by making a Design Table or Configure Feature. I’m going to add in lumber profiles up to 6″ x 6″.
Once we’re done that the next step is to save the profile out as a weldment profile you first must click on the Sketch > Save As > select where you want to save > Save As Type will be Lib Feat Part (*.sldlfp) > enter a file name and Save.
Last thing we need to do is specify where to save the profile. It’s a good idea to back up all your profiles and to keep the profile saved outside of a SOLIDWORKS folder. This is in case your files become corrupt or if SOLIDWORKS gets uninstalled, and if your files are backed up you won’t risk losing your creations.
When linking your profiles it’s important to make sure you have the correct file structure. You may need to create or select a file deeper or above.