8 Replies Latest reply on Apr 21, 2017 11:47 AM by Jim Steinmeyer

    How to drag an un-linked part copy from design library?

    Joel Murphy
    Joel Murphy Apr 21, 2017 10:06 AM

      Hello,

      I have a part in my design library that I would like to be able to drag and drop non-linked copies of into my assembly. The idea is that my library part has undefined dimensions, and when I drop it in I can then define the dimensions to my assembly without changing the original as there will be multiple variations of the same part. I understand there are ways to do this with pack and go and what not but I am looking to do this easily. I am using 2016.

       

      Thanks

        • Re: How to drag an un-linked part copy from design library?
          Frank Ruepp
          Frank Ruepp Employee Apr 21, 2017 10:18 AM (in response to Joel Murphy)

          Hi Joel,

           

          there are several ways to do this (without claiming that these are all):

          1. You could use "Make independent":

            You will be asked to save the component to a different location.

          2. You could convert the part to become a virtual component:

            Creating a virtual component will break the link to the original part and later on you could save it to your desired location.

          3. You could open the part in a separate window and make a save as:

            You will get different options whether the newly created part will be used as the new reference or not.

          Hope this helps.

          Kind regards

          Frank

          SOLIDWORKS Product Definition Team

            • Re: How to drag an un-linked part copy from design library?
              Joel Murphy
              Joel Murphy Apr 21, 2017 11:07 AM (in response to Frank Ruepp)

              Thanks Frank,

               

              I found that 'make independent' shortly after I posted. That seems to be my best option. I was really hoping that  there was a keyboard modifier I was missing to be able to do this from dragging from the library, but it guess it doesn't exist. Maybe a future feature?

               

              Thanks again,

              • Re: How to drag an un-linked part copy from design library?
                Jim Steinmeyer
                Jim Steinmeyer Apr 21, 2017 10:57 AM (in response to Frank Ruepp)

                Frank,

                I think this is related so maybe you can clear this up for me. Like Joel I have part profiles (the profile of a structural I-beam for example) that I will drag from the design library and place as a new part and I am asked if I want a Derived part or not. As a rule I desire to make this part unlinked to the original and save it as a new part number. Commonly the library part is stored as a 12" long part and I want to save it at a different length and give it a new part number and description saving the material information.

                     What is the difference between derived or not?

                  • Re: How to drag an un-linked part copy from design library?
                    Frank Ruepp
                    Frank Ruepp Employee Apr 21, 2017 11:12 AM (in response to Jim Steinmeyer)

                    Hi Jim,

                     

                    are you talking about this message:

                     

                    Kind regards

                    Frank

                    SOLIDWORKS Product Definition Team

                        • Re: How to drag an un-linked part copy from design library?
                          Frank Ruepp
                          Frank Ruepp Employee Apr 21, 2017 11:32 AM (in response to Jim Steinmeyer)

                          Hi Jim,

                           

                          you will always get this message when you drag a part into another part.  This is different from dragging a part into an assembly:

                          1. When you drag a part into another part you will get the above message:
                          2. Now when you choose yes you will get the "Insert Part" Property Manager where you can define which geometry should be inserted into the receiving part:
                          3. Depending on your selections you will get different results but you will always get a "feature" in the receiving part that shows you what you have inserted:

                            We keep the inserted geometry in different folders so that you can comprehend why the entities are listed.

                          4. This will create a geometrical copy of the design library part and you can add features on top of the inserted geometry.

                           

                          Possible workflows are that you have i.e. a generic stock component that gets individually modified based on i.e. customer requirements.  Imagine a valve housing that is always identical but based on customer requirements it will get individual holes.

                           

                          Whereas when you insert the design library part into an assembly you won't see this message and you can apply the different methods to make the part independent mentioned earlier.

                           

                          Kind regards

                          Frank

                          SOLIDWORKS Product Definition Team

                            • Re: How to drag an un-linked part copy from design library?
                              Jim Steinmeyer
                              Jim Steinmeyer Apr 21, 2017 11:47 AM (in response to Frank Ruepp)

                              Frank,

                              That does help make it clearer as to what is happening and what to choose. If I select no I get an extruded feature that can be edited and does not change the original part.

                                       One other example for selecting a derived part would be for machining a part. I could place a cast or welded part in a new part and then add the machining steps to get a new part for the finished product. This has potential.

                               

                              Thank you