13 Replies Latest reply on Mar 16, 2018 10:09 AM by Frank Ruepp

    Mate reference on smart components

    Stefan Fredriksson

      Hi

       

      I'm trying to get mate reference to work togheter with smart componets without sucess!

       

      I my assembly my goal is to drag a small vent (own part) that I use frequently. The part has 7 different configurations, (different diamater of a cylinder). In another part I have made an cut extrude with let say 7mm dept and diameter 15. From that hole I created another hole with diameter 13 that goes deeper. The smart component that I'm trying to insert in the assembly should be able to "read" the diameter of the hole and choose the right configuration of the part. So far so good.

       

      The thing is that i also want it to mate conecntric with the hole AND coincident with the small ledge that forms between the different diameter 15 and 13 7mm down. Even though I made mate references in that part it doesnt work. Today I have a coincident on the circle and concentric with the diameter.

       

      It feels like SW doesnt care about the mate referenses but only the smart component autosize..

       

      Anyone has any idea?

        • Re: Mate reference on smart components
          Frank Ruepp

          Hi Stefan,

           

          can you please upload a picture and if possible your model in order to make it easier to understand what you are trying to achieve?

           

          Kind regards

          Frank

          SOLIDWORKS Product Definition Team

          • Re: Mate reference on smart components
            Frank Ruepp

            Hi Stefan,

             

            Mate References do not behave like they will sequentially run through all defined mate references and automatically select a matching entity that is close to the mate reference or will ask you to point to a matching entity.

            Mate References will select the first entity that matches the first defined mate reference and that's it.

            You definitely can set up more specific mate references that will create several mates based on the mate reference entities but you will also have to have a mate reference with the same name in a part in the receiving assembly.

            I.e. if you had defined a Mate Reference "FullyMated" where the first reference is a cylindrical face (concentric), the second reference a planar face (coincident) and the third reference also a planar face (parallel), you would require a mate reference with the same name ("FullyMated") with the matching mate references in the correct order in a part of the receiving assembly or in the receiving assembly itself in order to automatically get the component fully mated.

            As long as there is a cylindrical face involved in the mate reference it is a good idea to select a circular edge to get concentric and coincident mate in one shot.  However Smart Components really require a cylindrical face in order to determine the correct diameter for the samrt component.

             

            I did a presentation about Smart Components at this year's SOLIDWORKS World and I have attached the presentation to this reply.

             

            Hope the presentation is of any use for you.

             

            Kind regards

            Frank

            SOLIDWORKS Product Definition Team

              • Re: Mate reference on smart components
                Stefan Fredriksson

                Ok,

                 

                so If I understand you correct there is no point in making 3 different mates in the mate referens cause it's only using the first one that it fit.

                I dont need it to be fully mated, a coincident mates will do If it will hook on the the right edge. The problem now is that the model adjust to the right size but then it doesnt stuck on the mate.

                 

                And I do not have any mates in the recieving part. The holes are made by a library feature in the part, is it possible to create a reference togehter with the library feature so that every hole like this will introduce a mate reference so when the venting is getting near it will be fully mated?

                 

                //Stefan

                  • Re: Mate reference on smart components
                    Frank Ruepp

                    Hi Stefan,

                     

                    no, this is not what I was trying to convey.  Basically you can create a mate reference with three references underneath and all three references will be used when you have a mate reference with the same name somewhere in the assembly with matching reference entities.

                    In the presentation there is some explanation how to make a smart componet adjust to existing geometry.  But once again in a nutshell:

                    When you define the smart component you can specify a reference face that is used to determine the correct diameter:

                    After you have selected the correct face (the cylindrical face in the center) you can push the Configurator Table... button:

                    In this Configurator Table you can specify which configuration should be applied to which matching diameters.  Like in my example the Flange 20x75x75 will be chosen when the receiving geometry is inbetween 19 and 21 millimeter.  So when I drag this flange onto a shaft that has a diameter of i.e. 19.5 mm, the configuration FL - 20 x 75 x 75 will be automatically selected and a concentric mate between my reference and the receiving cylindrical face will be automatically created.

                     

                    I just tried and you cannot add a mate reference to a library feature.

                     

                    Hope I have clarified my thoughts

                     

                    Kind regards

                    Frank

                    SOLIDWORKS Product Definition Team

                      • Re: Mate reference on smart components
                        Stefan Fredriksson

                        Hi again,

                         

                        sorry for all the dumb questions..

                        I have now tried. And the diameter is adjusting according to your descritpipion above. And when I insert a mate reference in ONE of the holes in my files and named it the same name as in the other part file it all went fine. (Is both adjusted and get fully mated) But the thing is then that I have multiple instances (holes with different diameter and I need to be able to bring in multiple part of the one that adjusted the diameter. That's why I wonder how I will be able to introduce a new mate referens for all the holes or it there another way around.

                        Perhaps it is possible to start by drag in the "vent" in place and the let it Performed the cut-extude (read hole) after?

                         

                        Many thank for your help so far!!

                          • Re: Mate reference on smart components
                            Frank Ruepp

                            Hi Stefan,

                             

                            no worries.  There are no dumb questions and I am totally aware how difficult it can be to get used to new functionality (yes, we also have to adjust to new functionality ).

                             

                            The basic question is what you are trying to achieve?  When you create a smart component you basically expect some additional benefit from a smart component like additional features automatically added, additional components automatically added and so on.  In my example with the flange bearing the bearing will automatically insert all the necessary cuts and will also add the required fasteners automatically:

                            My bearing will automatically insert all of its fasteners.

                            But also all of its required cuts in the underlying plate.

                             

                            So when you drag the bearing onto a shaft in an assembly it will automatically size itself:

                            It will automatically add a concentic mate:

                            And after I have added two additional mates to place it on that table and align it parallel to that table:

                            Just a quick note that you can mate several instances in one shot to one reference entity (on the picture above you can see that all instances of the bearing will be mated to the Face<1>@DeskPlate-1; of course you have to select all the faces but you do not have to create several mates).

                            I can add my smart features:

                            I have to specify my reference entities:

                            And when I click OK I will get all my features and fasteners automatically added:

                             

                            So this is the actual purpose of smart components that they will do additional steps for you after you have mated them into place.

                             

                            Kind regards

                            Frank

                            SOLIDWORKS Product Definition Team