18 Replies Latest reply on Sep 13, 2017 6:24 PM by Andreas Rhomberg

    Insert new part in assembly as floating by default?

    Marty Winters

      When I insert a new (virtual) part into an assembly, it is always fixed.  I would like it floating.  Is there a default setting for this?  I can't find it.  Also, I would prefer to be automatically prompted to enter a name.  All the extra button clicks to do both every time start to wear me down.  In case you want background, I am making piping systems (but don't have routing).  I place all the components (all external files) with mates in the assembly. Then, as a last step, I link them together with pipes that I leave virtual.  With many pipes to add, every extra action adds up.

       

      Thanks,

       

      Marty

        • Re: Insert new part in assembly as floating by default?
          Deepak Gupta

          The default behavior is fixed part. The way out might be using a macro that can take care of the things.

          • Re: Insert new part in assembly as floating by default?
            John Stoltzfus

            Could you show us screen shots on your process -

             

            How do you place or mate your components - with a Sketch?? or just measurements?

             

            I wouldn't be comfortable having a new component float and not fully defined.

             

            You mentioned

            Also, I would prefer to be automatically prompted to enter a name.

             

            If I understand you correctly this is what you want

             

              • Re: Insert new part in assembly as floating by default?
                Marty Winters

                Included is a screen shot of a piping manifold I am working on.  All of the valves and fittings (Tee's, Elbows, etc.) are are external, pre-existing parts and assemblies that I insert into the to assembly.  When I insert existing parts/assemblies, they generally inserted as floating, which makes sense to me (I do have to locate after inserting).  I use mates in top level assembly to locate.  The ones that are not fully defined are generally circular and I don't bother with a rotational mate.

                 

                For the pipes, I generally do them last and create a new virtual part for each.  I keep them virtual since they are 1) individual/independent since each length is custom,  2) have no potential to be used elsewhere, 3) keep them from cluttering up my assembly directory.  For straight sections, they are extrusions using convert entities and extrude up to surface.  For pipes with bends, they are generally 3D sketch and weldment.  As such they generally rely on feature and sketch relations to locate, not mates.

                 

                I don't see why any part (new or existing) would be inserted into an assembly as fixed since I always need to locate them after inserting.  I must be missing something.  Concerning the naming, if I change my practice to save every new part in an external file, then I will be prompted.  I just thought I should be able to do so with new virtual parts as well.  To illustrate my point, is there anyone who just leaves the auto-generated virtual part names as is?  I wouldn't think that is common so why not prompt?


                Thanks,

                 

                 

                Marty

                Solidworks Screenshot.jpg

                  • Re: Insert new part in assembly as floating by default?
                    John Stoltzfus

                    Having used SW for years and remembering some of the crazy assemblies that were screwed up by not having things fixed or mated to where they can't move, I still cringe

                     

                    The same as Sketches not being fully defined - so quickly things can get really messed up

                     

                    Are you taking all the piping and pulling them into a drawing?? If not I would make only one part being a pipe, if all you're doing is measuring lengths. Make a 3d Sketch of every connection and for each sketch use a sweep extrude

                      • Re: Insert new part in assembly as floating by default?
                        Marty Winters

                        If I have multiple pipes, none of them touching each other, is you suggestion that I put them all into 1 pipe part file? (Instead of individual files for each part.)

                         

                        I should note that I am not trying to create exact cut lists.  I leave it to the fitters to figure out the lengths they need.  I dimension between components only.  The pipes mainly serve as

                         

                        For straight pipes I use a an extrusion just because I can do them quicker.  For 3D sketches, the biggest problem I have is mating (with sketch relations) to the components.  The component (which I often get from the manufacturer) has the open end of a pipe/tube that I need to mate to.  I have found that Solidworks allows me to mate to the center point of the pipe end only when I am drawing the sketch line.  If I try to add a sketch relation  from the end of an existing sketch line to the center point of the pipe end, Solidworks will not "find" the center point on the component pipe.  Likewise, Solidworks does not allow me use the face of the pipe end for an "on plane" relation with the end point of the sketch line.  I can't understand why in either case.

                         

                        If you have any advice for this I would appreciate it.  I would provide an example but I don't seem to be able to add a Solidworks file to this message.

                         

                        I am getting better at fully defining items as I have had assemblies turn themselves into unrecoverable pretzels very late in the process.  One problem is that during the model built, as I am working out the layout, I sometimes want to maintain certain degrees of freedom until the correct layout emerges.  This can be very dangerous.

                         

                        Thanks,

                         

                        Marty

                          • Re: Insert new part in assembly as floating by default?
                            Marty Winters

                            Sorry for the dangling sentence in the 2nd paragraph.  I meant "The pipes mainly serve aesthetics to so I an the fitters can correctly interpret the layout".

                              • Re: Insert new part in assembly as floating by default?
                                Scott Lyon

                                First I'll admit to not reading every word from above so if I'm out of sorts, sorry.

                                I do a lot of the same thing you do: set parts and pretty them up with pipe looking sweeps. I have had pretty good luck using a single part for all the pipes by having multiple sweep features. Since you "keep them virtual since they are 1) individual/independent since each length is custom,  2) have no potential to be used elsewhere, 3) keep them from cluttering up my assembly directory." it shouldn't be required to have a separate part for each pipe. If you do end up needing such you can save out the bodies (pipes) individually or as a whole referenced assembly.

                                 

                                Using this method makes fixed or floating a mute point. the 3D sketches are secured with 2 relations at each end, an on plane and a concentric. Each pipe is them defined by the sketch and can rebuild however needed. If you move a valve, the pipes follow.

                                 

                                I even use 3D sketches to make the profile after setting the path sketch. That way I don't have to mess with planes or faces to sketch on.

                                  • Re: Insert new part in assembly as floating by default?
                                    Marty Winters

                                    Thanks Scott,

                                    I just filled in a whole bunch of pipes on another model and settled on a method that seemed to work well, at least for straight pipes, even though it didn't follow the one file method.

                                     

                                    I made a 1" long part file for each pipe diameter.  Sequence:

                                    1. Insert pipe part
                                    2. Make virtual
                                    3. Mate one end (concentric and coincident)
                                    4. Edit extrusion from blind to "up to surface" and choose the mating surface.

                                    That leaves me with a virtual part with mates so I can use "copy with mates".  For copies, sequence is:

                                    1. Copy with Mates to anchor new pipe.
                                    2. Make independent
                                    3. Edit extrusion and pick new ending surface.

                                    It seemed to work quite efficiently.  For bent tubing, I will still have to go with 3D sketches and a bit more work.  That is OK since these are in the minority and inherently take more work anyway.

                                     

                                    Thanks,

                                     

                                    Marty

                                • Re: Insert new part in assembly as floating by default?
                                  John Stoltzfus

                                  Marty

                                   

                                  According to your note above I would definitely use 3D sketches and make it one part even if the ends are 10 feet apart, for each run open up a 3D sketch, select a circle of the fitting and convert the entities and make it a construction line, then you have your center point to attach a line to. The tricky part is making sure you select the proper orientation which take a little practice till you get it right....

                                   

                                   

                                   

                                  Once you connect the fittings with a line add whatever fillets you need and close the sketch go from one fitting to the other stop and add a plane if you need it by selecting a straight line and a vertex at the end of the line and add a plane, then draw your pipe circle on that plane and do a sweep extrude -

                                   

                                   

                                   

                                   

                                  Do each connection like that and drop the final part in your drawing in an ISO view so you can easily dimension everything

                                   

                                   

                                  That is how I would approach it if you don't need individual pipes - however if it gets to full you can split it in more that one part as well.

                                   

                                  By using the 3D sketch method you can move around the fittings, however you may have to readjust your 3D sketch if you move the fittings in line with each other etc.......

                                    • Re: Insert new part in assembly as floating by default?
                                      Glenn Schroeder

                                      John,

                                       

                                      I do something similar to what you proposed, but I take it one step further.  I have pipe profiles saved as .sldlfp files to use for cases like this.  After creating the 3d sketch for the path I use the Structural Member function for Weldments to create the pipe.  Then there is no need to create a plane and a sketch at the end of the 3d sketch line.  I also have simple round profiles saved for when I have cable in an assembly, or for when I'm modeling rebar.

                                        • Re: Insert new part in assembly as floating by default?
                                          John Stoltzfus

                                          Glenn,

                                           

                                          Sounds like a good idea to go that way, I hardly ever work with assemblies similar to Marty's - but I know the frustrations that come with a model being almost done and bam all the sketches get screwed up -

                                           

                                          Marty,

                                           

                                          One of the things I missed was if it ever happens that your assembly and sketches would throw all kinds of errors, don't panic lol - just suppress every component and then start at the top of your feature manager tree and un-suppress each item one by one, normally the errors are pretty easy to find this way,

                                           

                                          Later,

                                           

                                          John

                                            • Re: Insert new part in assembly as floating by default?
                                              Mike Bartlett

                                              I Use the same method Glenn has stated. the 3D sketch can be drawn in context to the positions of the pumps. This allows for future changes without turning the assembly into a birds nest. Also then allowing for an accurate and simple cutting list/BOM for the pipe length and costings.

                                               

                                              Kind regards,

                                               

                                              Mike

                                                • Re: Insert new part in assembly as floating by default?
                                                  Michael Locascio

                                                  IF I was making a part that looked anything like piping (as this does appear to be) I would use the CORRECT module, specifically piping. It appears that this thread got way offline. The initial question had to do with making the first component come in floating. That's how it is done in Pro/E. The system wants to fix the first component because it knows that some users (slackers) won't do what they should be doing as designers, etc.

                                                   

                                                  I don't want to see a fixed component in any of my assemblies. Why? Because it usually doesn't show the design intent that I am looking for. Technically anyone who claims to be a CAD guy should be fully constraining their parts.

                                                   

                                                  So, I need an answer that makes sense. Writing some bogus macro to do what the so-called CAD software should be doing doesn't make any sense. That sounds way too much like AutoCad to me.

                                            • Re: Insert new part in assembly as floating by default?
                                              Andreas Rhomberg

                                              FYI.

                                              in 2017 it is no longer necessary to sketch the circle. select Circle Profile and thin feature for Quick Tube or Pipe.

                                               

                                               

                                      • Re: Insert new part in assembly as floating by default?
                                        Michael Locascio

                                        You would not leave the component floating. The idea is not to have an unconstrained component. The idea is not to have to break the fixed component so that you can properly place the first component.

                                      • Re: Insert new part in assembly as floating by default?
                                        Dave Hoder

                                        Wow this thread took a turn off topic! I'd also like to see new (virtual) parts inserted as floating. We build entire assemblies from virtual parts until the design is finalized and it's a pain to float every new part. They're also usually stuck in some spot where you have to find them first.