16 Replies Latest reply on Jan 29, 2015 7:04 PM by Josh Killalea

    Editing individual assembly without changing the originals?

    Erik Pucci

      I am fairly new to Solidworks, but our company is planning on switching to it for most of our work, so I am still in the feeling out phase of this program.  Most of the issues I have had, I have been able to work through, except for one problem.  We are a pipe and duct work company, and another coworker made a few test assemblies of our product, and I created a new assembly to combine them together.  As you can see from the picture below, in my assembly I have 3 pieces of pipe connected to an elbow, and a single piece of pipe on the other end of the elbow.  All of my company's pipe is 120in. long, but we can also cut them to be shorter (we call these pieces "cut pieces") to adjust to fit what we need to make in a customer's plant.  I can click on any of these pipes and choose edit feature, and I can change them to however long I want them to be (for example, 80in. long) but when I do that it changes all of the pieces to the new dimension, which is not what I want to accomplish.  I understand why it is happening, but what I really want to do is edit the single piece of pipe to a certain dimension without it affecting the other 3 pieces of pipe in the assembly, and I am just not sure on how to accomplish this.

       

      I also understand that I could make a new assembly for the pipe and bring it into my current assembly, but our company works with tolerances up to 1/16in, and I don't want to have to go through the process of creating a new assembly for every cut piece I want to make (which can range from 3-4 cut pieces all the way up to over 100, depending on the size of the project)

       

      Surely there must be a way to bring in 4 assemblies of pipe, and edit one without editing the other 3?

      screenshot1.png

        • Re: Editing individual assembly without changing the originals?
          Matthew Hiser

          Hi Erik,

           

          I think I have a solution to your problem, though it may take a little getting used to as you said you're new to SolidWorks. You can make separate configurations of each of your assemblies (i.e. Your custom cut pipe lengths) and then change to them within your larger assembly.

           

          For example, you could go into your 14in.pipe assembly, create a configuration for an 80in. long pipe (NOTE: I suggest using the forum, tutorials, or even You Tube videos as helpful guide on how to make and organize multiple configurations) and then within your PIPE RUN assembly, for the sections of pipe you want to be 80in. long, just right click the pipe assembly you want to change, go to properties and select that configuration. Once you get accustomed to using configurations, I would advise using design tables to keep your dimensions organized within your smaller assemblies with your multiple configurations.

           

          The advantage to configurations is that is saves you loads of time in not duplicating work (like you said) and allows fast and easy design changes to be made within your larger assemblies. You can also customize your configurations per detail drawing, BOM's you name it. I hope this answers your question and also peaks your interest in looking into what SolidWorks can do.

            • Re: Editing individual assembly without changing the originals?
              Erik Pucci

              We have used configurations and design tables with a few other things here, and it seems like this is the way we are going to have to do this.  Which isn't a big deal, it is just a completely different way of thinking from the program we use currently (Cadkey 19, don't laugh please).

               

              What I am thinking is once the design table is set up, I could measure the distance I need to hit for my cut piece, and then make another configuration in the design table called "14in pipe cut piece 1" and just copy all the values over from the default configuration and change the d1 measurement (which is my length) to what I measured.

               

              I was just wondering if there was a quicker way to do it, because we don't necessarily need to keep a copy of it for BOM or anything, because when the job is installed we send a normal 120in piece of pipe and the onsite mechanic cuts it to fit.  It isn't really slower with design tables, just a different way of thinking about it, which I think is going to be the biggest hurdle we have.

               

              Thank you for your input Matthew.

            • Re: Editing individual assembly without changing the originals?
              Glenn Schroeder

              There are several ways to approach your problem.  You might want to try them and see which works best for your company.

               

              1.  You can create configurations of the pipe.  In your case, that will allow you to have multiple different lengths of pipe in the same part file.  You can control which configuration of the part is used in each individual instance of an assembly.

              2.  You can have an assembly cut, which would cut one or more pieces of the pipe in the assembly only (see the screenshot below).  There is a setting near the bottom of the assembly cut's PropertyManager where you choose whether or not to have the cut affect the part file.  In your case it sounds like you would choose not to.

              3.  There is a new feature with SW2015 that might work for you, but I haven't used it yet, so I can't personally say, but it might be worth looking into:  2015 What's New in SolidWorks - Saving Component Instances as New Files .

               

                • Re: Editing individual assembly without changing the originals?
                  Brian McEwen

                  Glenn's list sounds good (but option 3 is just a fancy Save As command I think).  For length configurations the Configuration Publisher would also work.

                   

                  ""I don't want to have to go through the process of creating a new assembly for every cut piece I want to make"" I think you mean part (.sldprt) file for each piece of pipe. Your aversion is understandable.  However it would work okay to have 100 part files, just save them all in one project folder. If you don't want to go into each part to change the length you could look at Top Down modeling. So you have 1 sketch that drives the length of all the pipes... However a Weldment is an easier way of doing this.

                   

                  I think you could do this as a Weldment (in one .sldprt files). If you don't need to make drawings of individual parts it is easier to accomplish. You would need to edit the weldment profile sketches (store in shared location if more than one SolidWorks user) to have all the sizes you use. The main thing to test, that I'm not sure about, is if the Cutlist comes out in a way that is helpful to you.  Hmm, junctions of rectangular ducts might be tricky too - you should do some experiments.

                   

                  (FYI - You can't make individual drawings of Virtual Parts. )

                   

                  I think the configuration for length sounds the best. That is a great use of configurations. And once you have one pipe or duct size  set up you could copy it for new projects (always make unique filenames) - which is probably safer than reusing one part file for multiple projects. You could even control diameter and wall thickness with configurations, but there are tradeoffs.

                    • Re: Editing individual assembly without changing the originals?
                      Brian McEwen

                      What version of SolidWorks do you have? I created an example of a pipe set up for Configuration Publisher - it is in SolidWorks 2014.  Insert it into an assembly and the dialogue will automatically pop up where it asks for the length.

                       

                      The cool thing is it only creates the configurations you need. They are stored in a Design Table and the Config Publisher is just a slick interface.

                        • Re: Editing individual assembly without changing the originals?
                          Erik Pucci

                          I have 2014, I used your example, it was pretty awesome how you just toss in the length and give the computer a second to do it's magic and go from there.  I also like how it adds it to the design table automatically as well.  I am going to have to tinker with this a bit (because we have pipe but it has rings on it for connection purposes) but this could be our solution.

                           

                          Thank you for the example, I will have to check out a tutorial on the internet for using Config Publisher.  Do you know if it's possible to do this with assemblies as well (since your example was a part)?  I would assume so, it would just take some extra setting up most likely.

                            • Re: Editing individual assembly without changing the originals?
                              Brian McEwen

                              Config Publisher is possible in an assembly, but I'm not sure of the details in this case. If you want to change any of the features on the parts - like the length of the pipe - then you get into a Top Down modelling situation where the sub assembly controls the length of the part, per configuration. It would be more complex. Need configs at the assy level and at the part level. Yuck.

                               

                              The other thing to consider - can your pipe subassy actually be made into a part? From the image you show it seems likely - unless you need to be able to change out the type of connection ring you use or something. You would just model the rings as bodies in the part (see Multibody in Help).

                               

                              By the way if you use an assembly cut (in the top level assy) you would be chopping off the ends of the pipes and the rings, unless you did the cut in each sub assy (hmmm I guess that would work)... Why not just add the rings at the top assembly? Instead of in a sub assy?  Lots of decisions to make.

                               

                              Did you look at weldments? Single sketch (or 3D sketch) to control all section lengths would be cool.

                                • Re: Editing individual assembly without changing the originals?
                                  Erik Pucci

                                  Well before you gave the example of the Config Publisher, myself and a couple of others in our engineering department were tossing around the idea of making the pipe plus the 2 rings as one part, instead of combining them into an assembly.  That is likely what the final outcome will be, which would make it easy to use the publisher as well as not having to deal with sub-assemblies all the time (especially when projects can have hundreds of pipes in addition to the machinery they connect to).

                                   

                                  We do use a standard connection ring, which is why we have figured making it a part file, so thank you for reinforcing that opinion.  Assembly cut seemed to work, to a certain extent, but the pipe would cut and the ring would not follow the cut because of how it was mated.  Instead of changing the mates or cut each sub-assembly, we could just make it one single part, which is another pro for using Config Publisher.

                                   

                                  We have not taken a look at weldments yet, but will give them a try as soon as we are able to.  Honestly I think Config Publisher will work for what we need it to do, because it takes what we know as of now (design tables) and makes it super simple to drop in and configure on the fly (it saves lots of time, which was the major reason why we still use a very old version of cadkey).

                                   

                                  I will update in the near future, but thank you (and everyone else) again for pointing us in the right direction.

                          • Re: Editing individual assembly without changing the originals?
                            Erik Pucci

                            I think option 1 will probably be best for us, but it is just a different way of thinking about the process.  I will have to give option 2 a try when I have a moment, and I think option 3 is beyond my control at the moment because of the new version of SW we would need.

                          • Re: Editing individual assembly without changing the originals?
                            Andrew Kronquist

                            Another suggestion that I use, but is probably not what you need here is to save the parts in the assembly as "virtual" parts. You can right click the part in the feature tree and choose "make virtual". When you do that the part is saved in the assembly, and the original part file is no longer referenced. It's also easy to save a virtual part to a file if you need to.

                              • Re: Editing individual assembly without changing the originals?
                                Erik Pucci

                                This was one of the options I tried while fiddling around with it, what would happen though is I would make 1 pipe assembly "virtual" but it would also make the 3 other assemblies "virtual."

                                 

                                When I right click on my assembly of a pipe, I would choose "make virtual" and it would pop up a dialogue box that said this will break references to the original part, which is fine so I clicked okay.  But in my design tree, it would make that piece of pipe "copy of 14in pipe" but it also made the other 3 pipes the same thing, so if I make a change to one it still changed all 4.

                                 

                                I could also "make independent" after making an assembly virtual, but that also changed all 4 pieces when I edited a feature of the "independent" assembly.

                              • Re: Editing individual assembly without changing the originals?
                                Brian McEwen

                                Erik - check this out. Post today by  Josh Killalea

                                Re: What is the most efficient Top-Down design flow in terms of rebuild time?

                                 

                                Seems similar to what you want to do. Combination of top down sketch control and configurations for pipes.

                                • Re: Editing individual assembly without changing the originals?
                                  Josh Killalea

                                  i do exactly what you are doing for a living at the moment. it is possible, what you are doing sounds (on the surface) exponentially easier and smaller than what we are doing here. we have our entire mine site in SW with all pipes and everything right down to fabrication detail. as this is what i do for a living and it is where i would like to take the direction of my company (helping people in your situation with solutions) i will not give away to much information, except to say that it is do able and while a lot of the suggestions made so far will work on a smaller scale, when implemented on a larger scale they can be more unstable and some times down right unusable. we found top down modeling was the easiest fastest and most stable way to achieve the pipe runs.

                                   

                                  i would be happy to talk to your employers about taking your company on as a client and helping you achieve what you are looking at in as short a time as possible, but i will not do it for free sorry.

                                   

                                  that said i am happy to help you with some solidworks 101.

                                  the problem you are having is that you are inserting one assembly (the sub-assembly) 4 times into the main assembly, that assembly is only referencing one part (the pipe part) and you are changing that pipe part so naturally it will update in the other 3 instances of the assembly. there is no way to avoid that.

                                   

                                  the fastest way to create a new assembly is to do a save as on your sub-assembly with a new name (cut 1 assem) and then do a save as on your pipe part (cut 1 part) then open cut 1 assem, it will still be referencing the original pipe part, right click on the pipe part and then click the arrow at the bottom of the menu, in the expanded menu you will see a "replace components" option, click that and find the cut 1 part and then click open. it will ask you to confirm the mates, click the green tick and then modify your cut 1 part. then in your main assembly right click and replace the assembly you want with the cut 1 assem. this would be the fastest, easiest and most robust way to do what you want to achieve for now. however there is much faster and easier ways to do the job in the long term.

                                   

                                  i have sent you a PM with my contact details if you or your employer are interested in talking about the solutions i can offer further.