13 Replies Latest reply on Oct 22, 2018 3:53 PM by Steve Calvert

    New to SW, extending parts

    Steve S.

      I'm new to SW and for my first project I'm designing a deck.


      When you want to extend a part (in this case, a board) to another board, do you have to create a new part for the length you need, or is there a way to do it in the assy?


      In my picture, I want to extend the studs up to the rafter, notching them out, and making the tops of each stud flush with the rafter.



        • Re: New to SW, extending parts
          Albie Waterton

          Steve, you should be able to do what we call 'in-context' modelling, to update those parts.


          If you select the part you wish to change, then on the Assembly tab of the Command manager, you will see the option to edit component.



          This will then allow you to update the part/extrusion so that its end condition meets the requirements you want.

          Once you have chosen to edit the part, it will turn blue by default in the Feature Tree. Within here you will be able to update the features as you wish.

          If you then edit the feature in question you will be able to edit the end conditions so that they go up to the body you want.



          Hope this helps



          • Re: New to SW, extending parts
            Rob Edwards

            Hi Steve


            You might like to also consider using a weldment.  I find they're a nice fit for timber structures.

            Structural Members in Weldments have a Trim/Extend feature available and also other advantages such as cutlists, but you would probably have to create your own custom profiles and have a play around.


            2018 SOLIDWORKS Help - Weldments

              • Re: New to SW, extending parts
                Steve S.

                I have been reading about weldments, and it's an attractive idea to have that cut list at the end, but like you said, not sure how much up front setup is needed.

                  • Re: New to SW, extending parts
                    Paul Risley

                    It is not that difficult, setting up weld profiles is pretty straight forward. Just use standard sizing 2 x 4 etc. Myself personally I have 1 weld profile that is configured with all of the board sizes I use on a regular basis and 1 square profile for posts.


                    This was a pergola concept for someone all done in weldment with 1 3D sketch. I modelled their deck in another weldment to assembled them together in 1 assembly. It worked ok for sizing and proof of concept.(no connection joints or hardware/ bracing added) They decided to go with a prefab pergola instead but you get the idea. With a welment you can cut specific bodies vs. having multiple configurations of parts so if you have an x direction member that is the same length as a y direction member your cut list will recognize both as the same body part until you cut 1 then it will sort them into 2 different items. Yet it is still 1 weldment file.

                    • Re: New to SW, extending parts
                      Erik Bilello



                      As you've probably gathered, not much "up front setup" at all is needed to use weldments. I can think of a couple of people who resisted weldments (and other SolidWorks features) because they needed to get stuff done, and didn't have time to learn something new (I.E. how to save time).  I call people like that "not lazy enough".  Once they finally slowed down enough to figure weldments out they were mad at me for not making them do it sooner.  If you haven't already, I can almost guarantee that once you try using weldments, you'll wonder why you didn't do it sooner.  Be lazy, try weldments.

                      Also, I seem to recall someone at our last user group meeting saying that they found a library of standard lumber profiles (in weldment format) available for download somewhere, but I don't recall where, that's what Google is for. I've just been making my own as I go, which would be another good learning experience for you, it's really quite easy.



                  • Re: New to SW, extending parts
                    Glenn Schroeder

                    This may give you an idea of the benefits of using weldments.  It took about 20 minutes for this sample from start.



                    All the cut list properties were automatically generated except Body Name.  I didn't bother entering Body Names for all the bodies, but you get the idea.  The lengths are odd numbers because I didn't take the time to fully define the sketches since this is just an example.


                    • Re: New to SW, extending parts
                      Rob Edwards

                      Hi Steve


                      If you decide to have a play here's two useful tips I picked up off Deepak and Ingvar.


                      In your Library Feature Part (where you sketch your profile)  Add some custom properties..  these will populate as weldment properties when you use it.


                      What's especially nice is using the sketch dimensions for width and thickness.  If you like you can copy these to the description as well.

                      It's possible to get the length in there using the special syntax


                      You can create configured weldment profiles if you like but I generally need an infinite amount of sizes so this one profile will do for all square edged profiles ... here I call it PAR (Planed All Round)

                      The cutlist folders can be named by the description in settings and that's about it.

                      you have all the properties you added in your cutlist


                      Example file attached

                      • Re: New to SW, extending parts
                        Glenn Schroeder



                        That works well for some cases, and I've done something similar for flat plate (Using Plate in Weldments ), but I'm afraid that might not work for lumber since the sizes are nominal.  For example, when we go to the lumber yard and ask for a 2x4, the actual size is 1-1/2" thick and 3-1/2" wide, and a 1x6 is 3/4" thick and 5-1/2" wide.  Because of that linking the dimension to a custom property in the .sldlfp would cause problems.  In my lumber profiles I've just entered text for the Descriptions (2x4, 1x6, etc).  Is lumber sold by the actual size in the UK?