11 Replies Latest reply on Nov 30, 2017 7:20 AM by Brian Rauchbach

    Making Threads in an Assembly File?

    Brian Rauchbach

      Is there a way to add a thread feature in an assembly file? The part and assembly drawings correspond to the order of machining and assembly welding steps, so since the part is threaded later on in an assembly, I do not want to add the thread in the part file. Since the thread feature or helical curve and sweep features are not available in an assembly I am not sure how to go about this. The only option I can think of, that still won't work, but lets me add a thread, is inserting a new part and drawing it in the assembly itself, however I would not be able to cut the threads from the sub assembly. I would have to instead extrude/sweep the threads as a new part then, and would have to account for that space for the extruded threads in the sub assemblies, so it will not work either.

        • Re: Making Threads in an Assembly File?
          Dennis Dohogne

          Brian Rauchbach wrote:

           

          Is there a way to add a thread feature in an assembly file? The part and assembly drawings correspond to the order of machining and assembly welding steps, so since the part is threaded later on in an assembly, I do not want to add the thread in the part file. Since the thread feature or helical curve and sweep features are not available in an assembly I am not sure how to go about this. The only option I can think of, that still won't work, but lets me add a thread, is inserting a new part and drawing it in the assembly itself, however I would not be able to cut the threads from the sub assembly. I would have to instead extrude/sweep the threads as a new part then, and would have to account for that space for the extruded threads in the sub assemblies, so it will not work either.

          If you use the Hole Wizard to create your threads this is certainly available in the assembly file.  If you are suggesting to create actual helical threads then I hope it is only for a couple of holes and only for some visual reference, otherwise you will bog down your system as helical features are computationally intensive.

           

          In an assembly you can do all manner of cuts, including helical sweeps, so you can do a cut thread if you really need to.  Your statement underlined above is incorrect.  What you cannot do in an assembly, at least not without some trickery, is to add material (not counting welds).

            • Re: Making Threads in an Assembly File?
              Brian Rauchbach

              Hi Dennis,

               

              The threading is for hydraulic cylinders for threaded connections between barrels/sleeves and glands so there are only a couple threads in the top level assembly so it shouldn't affect and slow it down too much. I want to model the actual helical threads so that I can get a more accurate simulations results and compare those to hand calculations.

               

              In order to cut helical threads using the sweep, I need to make a helix and spiral curve for the thread path (sweep path) and that feature is not available in an assembly file.

                • Re: Making Threads in an Assembly File?
                  Dennis Dohogne

                  Brian Rauchbach wrote:

                   

                  In order to cut helical threads using the sweep, I need to make a helix and spiral curve for the thread path (sweep path) and that feature is not available in an assembly file.

                  I stand corrected.  Thank you for revealing this.  I did not know that you could not insert curves in the assembly as you can in a part file.

                   

                  You have a couple of options.  One is to create the threads in the part file as Glenn suggested.  I cannot think why this would not be the preferred solution for your situation.  Unless you have parts that are mate-drilled and tapped at assembly the parts will otherwise have their threads prior to coming into the assembly.  If it is for purposes of having the threads properly "clocked" then that is not at all difficult to achieve in the part file either.  Another option is to create the helix curve in one of the parts and use that for the sweep path cut in the assembly

                    • Re: Making Threads in an Assembly File?
                      Brian Rauchbach

                      Dennis,

                       

                      I did not know that either until I tried to do so unfortunately haha.

                       

                      I just addressed my concerns/questions regarding the configurations method in a reply to Glenn's post. The part itself isn't threaded until after it is already in an upper level assembly because there are machining and welding processes prior to that. I'm not I understand what you mean by the threads being properly "clocked."

                       

                      I haven't thought of using a helix and spiral curve from the original part file. I've just tried this out, but unfortunately the error "Selected object is already owned by a feature" pops up when I try the select the helix and spiral curve from a part file as the sweep cut path in an assembly as shown below. Maybe I am doing it wrong or made a mistake?

                       

                      Thanks again for your quick response!

                • Re: Making Threads in an Assembly File?
                  Glenn Schroeder

                  Have you considered adding the thread feature in the Part file, and having two configurations of the Part, with the threads suppressed in one of them?  I'd suggest using the Part with the suppressed threads in the Assembly if there are more than one or two instances.

                    • Re: Making Threads in an Assembly File?
                      Brian Rauchbach

                      Glenn,

                       

                      I have thought about that somewhat. Currently almost all the machining processes are portrayed in one model and sheet drawing, but my boss wants me to separate all those processes step by step so that each step has a new part number. There are several steps before the part gets threaded, including some welding assembly steps and machining steps. For example there is a honing step after a component is already welded on all prior to the threading of one end for most sleeves. This would mean I would have to make a new configuration for all steps where the barrel/sleeve is machined all the way up to the threading step. I have worked with configurations a few times before but am by no means an expert on the topic. How would I even be able to change the configurations of the original part file in the top level assembly then?

                       

                      Thanks for the response!

                        • Re: Making Threads in an Assembly File?
                          Glenn Schroeder

                          It really sounds like configurations of a single Part would be the way to go.  As you said, you can have a separate configuration for each stage of fabrication you need to show.  As far as the separate Part Numbers that's simple enough also.  Just assign configuration specific Part Numbers (although I'd use a different name for the property to avoid confusion with the built-in PART NUMBER property).  You could then insert a drawing view of the Part in the first stage of manufacture (first configuration) and place a note referencing the Part Number.  Copy and paste the view (or whole sheet, depending on your needs), then switch which configuration the new view references.  If the note calling out the Part Number was properly linked it will also update.

                           

                          Choosing which configuration to use in an Assembly can be done several ways.  The simplest, assuming you have only one configuration of the Assembly, is to click on the Part and choose the desired configuration from the drop-down.

                           

                           

                          Another option, especially if you have multiple configurations of the Assembly, is to right-click on the component and choose "Configure Component" from the drop-down.  That will open a simplified design table where you can choose which configuration of the Part you want to use for each configuration of the Assembly.  The screenshot below only shows one configuration of the Assembly because this particular Assembly only contains one.

                           

                           

                          By the way, this table can also be used in your Part to set up your configurations.  Just create a feature, right-click on it, and choose "Configure Feature" from the drop-down.  Or create all the features first and open this table, then double-click on each feature that will need to be suppressed to add columns.  You can create as many new configurations as you need right there and get them all set up.  You can even name this table at the very bottom and save it for future edits.  If you don't name and save it the changes you make in it will still be in effect, but you won't be able to retrieve the table (although you can always set up another one).

                           

                          I know I wrote a small book here, and I left out a lot of details, but I don't know how much of this you already know.  I'm about to leave for the day, but if you have more questions please post them.  Someone else will be able to help, or I'll get back with you tomorrow.

                            • Re: Making Threads in an Assembly File?
                              Brian Rauchbach

                              I have only used the simplified design table once and forgot how to access it so that I can control and manage the configurations easier. This is definitely something I will discuss with my coworkers as a solution to our problem. I'll definitely look into this since I have several cuts and a hone that would change the diameter of the component where the thread goes prior to the actual threading process.

                               

                              Thanks again!

                            • Re: Making Threads in an Assembly File?
                              David Hurayt

                              not a problem

                              in your assembly you will have multiple configurations

                              each of these assembly configurations can reference difference  part configurations

                               

                              Ex:

                              Your assembly has configurations A, B, C, & D.  For simplicity lest say there are only two components (parts) in your assembly.  I have some hydraulic cylinder experience so lest say your parts are the outer tube and the gland nut.

                              Now for the parts they each have configurations also.  Lets say the outer tube has a "thread" configuration and a "non-threaded" configuration.  And for the gland nut there is a "thread" configuration and a configuration that has a cross hole for pinning the gland nut in place, we will call this the "pinned" configuration.

                               

                              So quick review:

                              the assembly has configurations A, B, C, & D

                              the tube has configurations threaded and non-threaded

                              and the nut has configurations threaded and pinned

                               

                              On your "assembly process" process drawings (cutting the tube, threading the tube, installing the nut, and pinning the nut in place) you will have:

                              • assembly configuration A consist of preparing the outer tube, it is cut to length.
                                • this configuration will have the outer tube component with configuration "non-threaded"
                                • and the gland nut will be suppressed
                                • you now have a model for your process A print
                              • the next step in the process (assembly configuration B) is the threading of the tube
                                • you will change the configuration of the tube to "threaded"
                                • the gland nut will remain suppressed
                                • you now have a threaded tube model for you process B print
                              • the next step in the process (assembly configuration C) is to install the gland nut
                                • your tube configuration will remain as "threaded"
                                • and your gland nut will be unsuppressed with its "threaded" configuration
                                • there is your model for process C print
                              • finally we need to pin the gland nut in place
                                • same tube configuration" threaded
                                • your gland nut configuration will be changed to "pinned"
                                • now you have a model with a hole in the nut for the pin

                               

                              We do assembly models all the time like this for a family of parts that may have interchangeable component depending upon the particular model. then all the view we need be it assembly and/or process prints come from one model with many configurations.

                                • Re: Making Threads in an Assembly File?
                                  Brian Rauchbach

                                  David,

                                   

                                  I do need all these processes as separate part numbers so making each step as its own assembly file is more convenient and easy to follow and maintain. If I used the configurations in an assembly to outline the different steps that could get messy if there are multiple steps prior to the threading step. I see now that I'll have to suppress my features in whatever order I'll need them in the separate part configurations and that a combination of suppressing parts and part features will help.

                                   

                                  Thanks for the response!

                            • Re: Making Threads in an Assembly File?
                              Dennis Dohogne

                              Brian,

                              Instead of configurations I think you will avoid more problems if you use Insert Part.  This is perfectly suited to what you are doing, especially since you have different part numbers for the different steps/operations.  The way I have used Insert Part is with a casting that gets machined and then gets painted any of several colors (with the added outer surface thickening).  It goes like this:

                              Part1 is the casting.  It is fully detailed and has its own part number.

                              Part2 is the casting after it is machined.  Its first "feature" is Part1.  This appears as a dumb solid in the tree.  You can add and subtract on it all you want to complete the features for Part2.  Part2 has a different part number (file name) than Part1.

                              Part3 is the next operation.  It has as its first "feature" Part2, which also appears as a dumb solid and ready for whatever features are necessary to define it.  It has a different part number than the other parts.

                              . . .et cetera

                               

                              This is really a lot easier to manage without errors.  If you try to do the progression of part numbers and features with configurations all within one part file it will be very easy for a change in one configuration to have an influence on another configuration where you don't want it.  With the Insert Part approach you are working only on the features that take the part from its starting point to the final definition for that intermediate part number.  It is so much easier to keep things straight.  And you still have a parametric relationship between these parts!  If you make a change to Part1 it will be reflected all the way through the others as you would epect it to.  Give it a shot, I thinkyou will find it a much easier to manage method.

                               

                              Another benefit is that you can keep all these things in the part environment.  That might help you avoid the problem you initially reported about not being able to cut threads in an assembly.