16 Replies Latest reply on Mar 15, 2017 5:39 AM by Carlos Goncalves

    Placing Assembly Features Into Folders?

    Jacob Steinmetz

      I am trying to organize my assembly Feature Manager Design tree by placing components and sub assemblies and such into categorized folders. This way I can show/hide each category as needed.

       

      I have multiple linear components and mirrored features in the design tree that I also want in these folders. When I try to drag them in, I get an error message saying "Cannot reorder after an assembly component."

       

      Is there any way around this? Or am I pretty much stuck with how it is?

        • Re: Placing Assembly Features Into Folders?
          Anthony Macke

          I have found when using folders in assemblies, sometimes it will not let you drag and drop something into the folder, but if you delete the folder re-select everything you want and re-add it to a new folder, it works like a charm.

          • Re: Placing Assembly Features Into Folders?
            Glenn Schroeder

            I don't believe you can put inserted components into the same folder as assembly features.  Is that what you're trying to do?

            • Re: Placing Assembly Features Into Folders?
              Tom Gagnon

              When I need to accomplish this, here's what I used to do, as a counter-recommendation. Dissolve the Pattern, available in right-click menu on the feature. Patterned components (hereafter including sub-assemblies) then become just components, and can be moved into folders. They appear in the same order as they were in when they were part of the pattern. Virtual components which were fixed in the source of the pattern become floated, and it's likely a good idea to re-fix them. Mates no longer exist between components within the pattern, nor mates between patterned source components and components outside the pattern. As such, this process can be either tedious to re-mate, troublesome with unrestrained components, or inflexible if you choose to simply fix all dissolved items. Another weakness of this action is that you cannot later alter the properties of the pattern as a feature, such as altering the distance(s) or direction(s) of a linear pattern, altering the mirror plane of a mirror pattern, adding/removing pattern instances, or adding/removing components to the pattern. Avoid this unless it's a very simple pattern.

               

              A better solution that I prefer is to create multiple similar Patterns for each category of components (TL,DR) which I would otherwise separate by folders, and edit the name of the pattern to append same categorical labels to the pattern feature's name. They still remain outside of the folder, but can be ordered similarly in the tree so that control of hide or suppress is repeated similarly both above and below the Mates tree item.

               

              (OFF TOPIC) The Mates folder in the tree is always the separator between components and features in an assembly, as I understand it. In other words, what Glenn Schroeder said more simply. This separation includes all assembly features (like a component's mounting hole in a support frame), not just patterns, although I prefer to keep these assembly-context features inside the component instead of using Assembly Features due to unique customization in my designs. If an assembly-context featured component is to be reused in a different assembly context, be sure to explicitly dimension or fix the feature's sketch entities instead of just automatically relating sketches to entities. Not doing this will produce out-of-context errors until removed from within additional contexts. To me it is easiest to allow automatic relations in a sketch, then delete relations, and dimension to reference planes/axes/origin or just fix them immediately afterward. Extensive measurements help to remove contextual feature definitions such as Up To Vertex Extruded Cut replaced with a Blind Extruded Cut or such, but cannot replace the flexibility of something like Up to Surface Extruded Cut where terminating curvature is involved.

               

              The choice between dissolving patterns or creating multiple patterns clearly depends on the complexity and scope of the included components.

                • Re: Placing Assembly Features Into Folders?
                  Jacob Steinmetz

                  Similarly to your first suggestion, I tried to dissolve the pattern, and then instead of going through each individual part, I selected all the parts through the feature tree and created a sub-assembly out of them. That way I could at least keep all the parts together and organized into a folder..

                   

                  Still not the ideal solution, however, because I then cannot go back and edit the features of the pattern.

                   

                  I also tried to make a sub assembly out of the component and pattern before dissolving the pattern, but for some reason it didn't get rid of the pattern feature on the feature tree under the mate selection.. I was expecting that all to be eliminated and combined into a single sub assembly above the mate divider.

                    • Re: Placing Assembly Features Into Folders?
                      Jacob Steinmetz

                      Just to clarify on that last part- I selected a sub assembly and the pattern feature of that sub assembly, and tried to make that into a new sub assembly within the main assembly. I've only tried to combine parts/sub-assemblies into a sub assembly, I have never tried to include a feature in that...

                       

                      Not sure what happened, when I look at the "undo" bar, it looks like a new sub-assembly was made, but nothing appears differently in the feature tree and the pop-up section "Assembly Structure Editing" did not show up either.

                        • Re: Placing Assembly Features Into Folders?
                          Glenn Schroeder

                          Are you doing all that just to shorten your FM tree, or is there some other reason?  I assume you know that even though you can't combine features and inserted components in the same folder, you can have folders for features also?  I don't want to offend you by questioning your modeling practices, but it seems like you may be doing a lot of extra work for very little gain.

                            • Re: Placing Assembly Features Into Folders?
                              Jacob Steinmetz

                              Somewhat a combination of a few things- so yes shortening the FM tree is a part of it, but I mostly want to be able to hide/suppress/show a combination of parts/subassemblies/patterns... at a time. I know this could also be done through configurations but there are too many combinations to go through and make each into its own configuration.

                               

                              And yes I know features can have their own folders, but then I end up having to hide/show/suppress two folders every time instead of one. It's not incredibly tedious by any means, so that's what I have been doing. I had just been trying to find a way to combine those so I don't have to do everything twice.

                          • Re: Placing Assembly Features Into Folders?
                            Tom Gagnon

                            Try Copy with Mates on the Subassembly instead of a linear pattern. Note this will only work easily if your external mates are relatively limited. That's another thing I'll use with subassemblies such as you describe, again either configuring the subassembly or making categorized subassemblies. It has the advantage of individualized spacings, like o.c. distances of 8" then 12" then 8" or whatever. Then delete the Pattern as obsolete.

                        • Re: Placing Assembly Features Into Folders?
                          Jacob Steinmetz

                          To essentially answer the question, as Glenn and Tom reaffirmed, you cannot combine features and parts/subassemblies into the same folder without either dissolving the components or editing them in a separate subassembly.

                           

                          Thank you both for your help!

                          • Re: Placing Assembly Features Into Folders?
                            Carlos Goncalves

                            Hello. Imagine that i have a brunch of parts like a bracket, and i need to have two screws to fix this part. I need to duplicate this bracket and screws several times. I find that i can had the set (bracket and screws) to a folder. The questions is if i can duplicate this folder?? If yes, how? If no, what can i use? Creating a new assembly is not the solution that i am searching.

                              • Re: Placing Assembly Features Into Folders?
                                Glenn Schroeder

                                I saw your other post, but the extended explanation here is a big help.  There are a couple of options.  Instead of inserting them separately I'd probably create a sub-assembly of the bracket and screws, and then insert this sub-assembly into the main assembly as many times as needed.  Another option would be to insert the bracket and screws, fully mate them, then select all of them, right-click, and choose "Copy with Mates" from the drop-down.  That function can be a little tricky to learn, but can be a very valuable tool.

                                  • Re: Placing Assembly Features Into Folders?
                                    Tom Gagnon

                                    Or, both of what you said: Create a subassembly then copy the subassembly with mates, or pattern the subassembly.

                                    • Re: Placing Assembly Features Into Folders?
                                      Carlos Goncalves

                                      The problem with creating sub-assembly is that i need to save them all. For example, in CATIA i had this tree organization:

                                       

                                      Fixture Structure

                                      The first element to be placed is a “component” with the customer parts 3D models. All remaining elements on the 3D should be placed related to the customer parts reference planes; (no need to save this)

                                      • The second element to be placed is another “component” with all the elements used for simulation (welding guns, welding torches, etc);(no need to save this)
                                      • Following these two components, all units CATProducts are placed;
                                      • The last element visible at the tree is a CATPart named CG “Center of gravity”.

                                       

                                      Product Structure:

                                      • The first element to be placed is a “component” with the customer parts 3D models. All remaining elements on the 3D should be placed related to the customer parts reference planes;
                                      • The second element visible on the tree is optional. It’s a component used to check open positions of pneumatic elements (cylinders, clamps arms, etc) – should be represented in purple color with 50% opacity;
                                      • For each CATPart, a “component” with the unit and part number should be created (check Part structure for instructions);
                                      • Finally, all pneumatic elements should have its own “component” with unit number and purchase reference.

                                       

                                       

                                      Part Structure:

                                      • The designed CATParts are placed inside this “component”;
                                      • The required buy-parts necessary to assemble this element should be placed inside this “component”.

                                       

                                      UPDATE: Even if i had a previous folder created with mates between the parts inside it (Aluminium Profile), and create a new one (Aluminium Profile 2), copy the parts again inside it and create mate of this second folder with other faces of the general product, it only move the part that i had selected to "mate".

                                       

                                      So, SW dont agroup parts as a folder, just serves to organize pieces in the tree. So this method is off...