3 4 5 6 7 Next Last 104 Replies Latest reply on Jun 9, 2018 4:48 PM by Matt Lombard Go to original post Branched to a new discussion.
      • 90. Re: modeling methods
        Matt Lombard

        Yeah, when you start changing how the bodies are split, there's no telling what might happen. Here's an excerpt from chapter 33 in the new book that mentions what you're talking about:

        Here’s a quick summary of the four master model tools that this chapter covers:

         

        • Insert Part: This function enables you to pull all the solid and surface bodies, sketches, reference geometry, and even features from an existing part into the current part. It’s available as a toolbar icon and from the Insert menu.
        • Insert Into New Part: This function enables you to insert a selection of solid and surface bodies from the current part into a brand-new part. Even though this function is initiated from the parent document, it’s classified as a Pull function because it doesn’t leave a feature in the parent but does leave one in the child. This function doesn’t have an icon.

         

        • Split: This function enables you to split a single solid body into multiple solid bodies and save (push) each body to a separate part file. This function is available as a toolbar icon and a menu entry in the Insert  Features menu. It creates a feature in the FeatureManager of the originating (parent) part file.
        • Save Bodies: This function enables you to save (push) all the solid bodies from a part out to separate part files. This function is available only through the RMB menu on the solid bodies folder. It doesn’t create a feature in the FeatureManager of the parent part and doesn’t have an icon. This is different from Keep/Delete Bodies.

        The one common weakness of all these tools is on the file management side, or more precisely, the body management side. It comes down to a question of what happens to the child document if you rearrange the bodies in the parent document. Body management issues can arise in a number of ways. The Insert Part feature is the one that has received the most development attention from SolidWorks when it comes to the robustness of file and body management issues, but Insert Part still doesn’t cover all the functionality. (You cannot insert selective bodies; you must insert all solids or all surface bodies.)

        • 91. Re: modeling methods
          Matt Peneguy

          Thanks Matt,

          You've definitely given a lot of information to investigate.  But, at the root of it all, everything has its pluses and minuses. It's just sorting through the different options for an application and finding what works for you.  And that is the hard part because everyone's needs are different.

          I have heard or read about most of what you listed.  But, I haven't investigated using them.  Part of the problem with SW features/tools/methods is that they often don't work the way you think they will and it takes a lot of time to really investigate something to get it to the point that it can be part of your workflow.  I have made that investment in Weldments and really like the result.  I may have to do some more leg work.

          • 92. Re: modeling methods
            Dwight Livingston

            Matt

             

            That is a good summary. Mark Biosotti gave a really good master model seminar at the 2017 SWW, which changed my thinking on various topics. I must say, though, that I have not done a master model project since then so I don't have my own experience to go by.

             

            From Mark's presentation, I would think that Save Bodies would work better than you say above. It sounds robust, anyway. Here is his slide on that:

            Capture.PNG

            This at least sounds like it will keep bodies straight, especially if you name them.

             

            On a related topic, I have always wished that SW would take all the export body stuff out of the Split feature and make Split more like other modeling features, just a sketch, split, and done. Use the Save Bodies when you have to, for the very few times you need it, compared to the many times you use Split. And stick that sketch inside the feature, instead of leaving it hanging in the tree.

            • 93. Re: modeling methods
              Matt Peneguy

              Jim Steinmeyer,

              To follow up on my question:

              What happens if you check out, say a Master Sketch part and make a change and one of the parts affected isn't checked out to you?

              I just got off the phone with the VAR, I asked them to answer this question while I had them on the phone.  Basically, in PDM if you check out a Master Part and make a change that affects a part not checked out to you it flags the assembly and part that it needs to be rebuilt.  So, you'll know what needs to be updated and what doesn't.  When you push the revision, if you have the below checkbox marked, users won't be able to push the revision for the parts.  They will have to check-out, rebuild and check back in the parts with the change.

              If you aren't using PDM, this is definitely a concern.  I'd be interested to hear how others using a folder approach deal with this situation.  Maybe John Stoltzfus has some ideas?

              • 94. Re: modeling methods
                Jim Sculley

                Matt Peneguy wrote:

                 

                That is definitely something to carefully consider. I'm sure PDM could help with this particular problem. And it brings up a good question. What happens if you check out, say a Master Sketch part and make a change and one of the parts affected isn't checked out to you?

                I'm going to have to go down that rabbit hole because we are in the process of rolling out PDM for collaborative work.

                Nothing happens.  Until you check it in and then open the affected part.  Which is the same thing that happens if you change a model and don't have its drawing checked out, or an assembly where the part is used.

                 

                PDM doesn't help maintain in-context references at all aside from letting you more easily see see when a file has them without actually opening the file.  You have to have an overarching process that people follow to ensure changes are made in a sensible manner and notifies the necessary parties, but the same is true for parts with no in-context references.  In theory, you could have PDM keep track of master parts (via a custom property linked to a data card variable) and when they are changed (via state change) a notification could be sent to users or groups.  However, in my experience, notifications are largely ignored.

                 

                I've been reading the thread and haven't seen a compelling reason to use any of the modelling methods listed for the type of work I do: one-off custom machines where nearly every part is a moving part and nearly every part can be made using a standard lathe and/or mill.  in-context references lead to confusion when checking parts in and out because the referenced files show up in the check-in/out dialogs.  If you have a master part, what do you call it?  Do you give it a part number?  Where do you store the file?  I prefer to keep the process simple, and maintaining in-context references is anything but simple.

                • 95. Re: modeling methods
                  Alex Lachance

                  Speaking for myself, we don't do a lot of multi-user projects. When we do them, generally they are split accordingly; One user does the master modeling and others do sub assemblies and parts.

                   

                  It is all about defining what needs to be built around your master and what doesn't. For instance, a door for a trailer can be installed on multiple trailers so it is imperative that the door be built without any link to the master assembly of the project. It is generally mated consequential so that if there is indeed a change that affects the length/width of the door that it can be easily spotted. If the door is to be built in context for some reason then the door will become a ''project'' instead of a product''.

                   

                  A part that can and is built in context to a master would be the main beam of a trailer. If the master sketch of the main beam changes, then the main beam needs to change accordingly to it.

                   

                  It's important to be conscientious of what your master affects.

                  • 96. Re: modeling methods
                    Deepak Gupta

                    Dwight Livingston wrote:

                     

                    On a related topic, I have always wished that SW would take all the export body stuff out of the Split feature and make Split more like other modeling features, just a sketch, split, and done. Use the Save Bodies when you have to, for the very few times you need it, compared to the many times you use Split.

                    If you do not rename the bodies in the split feature manager, then no need to save bodies OR in other words, you are not prompted to save bodies

                    • 97. Re: modeling methods
                      Matt Peneguy

                      Jim Sculley wrote:

                       

                      Matt Peneguy wrote:

                       

                      That is definitely something to carefully consider. I'm sure PDM could help with this particular problem. And it brings up a good question. What happens if you check out, say a Master Sketch part and make a change and one of the parts affected isn't checked out to you?

                      I'm going to have to go down that rabbit hole because we are in the process of rolling out PDM for collaborative work.

                      Nothing happens. Until you check it in and then open the affected part. Which is the same thing that happens if you change a model and don't have its drawing checked out, or an assembly where the part is used.

                       

                      PDM doesn't help maintain in-context references at all aside from letting you more easily see see when a file has them without actually opening the file. You have to have an overarching process that people follow to ensure changes are made in a sensible manner and notifies the necessary parties, but the same is true for parts with no in-context references. In theory, you could have PDM keep track of master parts (via a custom property linked to a data card variable) and when they are changed (via state change) a notification could be sent to users or groups. However, in my experience, notifications are largely ignored.

                      When bumping a revision the setting in the picture in my previous post makes it to where the part can't be "bumped" and will always remain needing rebuilding until it is checked-out, rebuilt and checked in.  But otherwise, yes users have to know what they are doing and how everything works.

                       

                      I've been reading the thread and haven't seen a compelling reason to use any of the modelling methods listed for the type of work I do:

                      I had come up with a pretty slick subassembly modelling method with no external references and compartmentalized mates, complete with rules and all.  It worked, but it had a fundamental flaw...What if I needed to change something?  So, I learned the SSP method and changes are soooo much easier now.  I'm not trying to contradict you...You know your workflow and methods posted may not work for it.  I'm just stating my experience.

                       

                      I've been reading the thread and haven't seen a compelling reason to use any of the modelling methods listed for the type of work I do: one-off custom machines where nearly every part is a moving part and nearly every part can be made using a standard lathe and/or mill. in-context references lead to confusion when checking parts in and out because the referenced files show up in the check-in/out dialogs.

                      This could be handled by training.

                       

                      If you have a master part, what do you call it? Do you give it a part number? Where do you store the file? I prefer to keep the process simple, and maintaining in-context references is anything but simple.

                      I call my master part "0.HXXXXX - Assembly or Part Description Sketch"  The 0 designates the level and the "Sketch" indicates it is the SSP.  But, it really doesn't matter what the name is the location in the feature tree makes it easy enough to identify.

                       

                      Do you give it a part number?

                      If you've got an ERP this may be an issue.  But to answer your question, no. And, I exclude it from the BOM.

                       

                      Where do you store the file? I prefer to keep the process simple, and maintaining in-context references is anything but simple.

                      It's just part of the assembly it goes into the PDM system just like any other part.  I agree there's a learning curve, but maintaining those references isn't overwhelming after some experience.

                      • 98. Re: modeling methods
                        Matt Lombard

                        Interesting that Mark adopted my push/pull terminology. It was just something I invented to help me understand what was going on. I remember talking to him about it when he worked for SW.

                         

                        If you totally rework the method for splitting bodies, and you have features/parts dependent on those bodies, you can orphan a whole lot of data. So just make sure you aren't making that level of change by the time you start adding features to your child documents.

                        • 99. Re: modeling methods
                          Dwight Livingston

                          Matt Lombard wrote:

                           

                          Interesting that Mark adopted my push/pull terminology. It was just something I invented to help me understand what was going on. I remember talking to him about it when he worked for SW.

                           

                          If you totally rework the method for splitting bodies, and you have features/parts dependent on those bodies, you can orphan a whole lot of data. So just make sure you aren't making that level of change by the time you start adding features to your child documents.

                          Sure. Maybe a fine print option to get to the old interface.

                          • 100. Re: modeling methods
                            John Stoltzfus

                            Matt Lombard - All the discussions here are great to follow and very interesting.  Just a quick comment on the Plastic Molded components or surfacing Models such as you show here..

                             

                            Like I mentioned before, we all start our Models the same way, by either using a 3D sketch or selecting a plane and adding lines.....  So the molded components have sketches right? So why not take a few of those sketches and relate the overall layout to those sketches, no different then selecting a solid, btw you can use solids rather then sketches.  I think that people visualize the SSP of being just full of a mass of sketches, your SSP can have just one sketch controlling the size, or you can have a 100 sketches. Most of us know that the more references you create the more it slows down SW.

                             

                            The interesting thing for me is people don't understand how I really use the SSP and apparently it is really difficult for me to explain clearly, I guess.  I've been on that side of the fence a long time and with a lot of collaboration with many people here on the forms a little bit by bit it became very clear that it's all about a process not about a technique.  Approaching every modeling project the same way, it don't matter if it moves or is stationary, or if it's a one off or multiple units, I wouldn't approach any new designs differently, because I know now that all my models are 100% parametric and accurate. My designs over the years have been very inconsistent and I feel for all the people struggling, been there done that.

                             

                            So for me it's not about which technique you use is it SSP, Master Model, Top Down or Bottom up, it is about creating a process that works every time with every project..    Just think of the SSP being a process where, you start here and go step by step till your model is complete, doing it the same way over and over and over, which in turn gives you confidence and 100% robust models every time.

                            • 101. Re: modeling methods
                              John Stoltzfus

                              Matt Peneguy

                               

                              The way I handle components in SolidWorks would make most people cringe.  Here in our production facility we have a very unique system of One Piece Work Flow and my drawing numbers are not inventory components parse.  Therefore each project is a separate entity so we could have literally hundreds of interchangeable components clogging up our computer data space, which doesn't matter as much now as it would have 10 years ago, who would have thought that you could have 100 gig of storage.

                               

                              What I do is Design on Size of that style and then Pack & Go the rest of the sizes after the drawings on the initial one is complete, I don't worry about interchangeable components at all.  If there is one part that is in 5 other sizes of that same style, it is still done as an individual pc. 

                              • 102. Re: modeling methods
                                John Stoltzfus

                                Jim Steinmeyer

                                 

                                Jim Steinmeyer wrote:

                                From my perspective there would be few things worse than making changes to a major part, having 10 minor parts change and only updating prints and dxf for 4 of them. Then the shop would make 6 parts to fit the old design causing a wreck on the floor. To me having to redo the design work is better that bringing the floor to a halt while I figure out what went wrong and getting new parts made. (I do that often enough without help from the software.)

                                There is where I can feel your pain, been there done that soooo many times, it used to make me sick and especially if you had a pressing project and all of a sudden drawings are wrong and the project is late, talk about pressure.. SolidWorks just didn't work, but now I know why.

                                • 103. Re: modeling methods
                                  Dan Golthing

                                  Matt Lombard wrote:

                                   

                                  Dan Golthing wrote:

                                   

                                  We all get that, but the "intelligence" built in is rarely necessary once the design is done.

                                   

                                  When is the design ever done? If you ever come back to it or make a version of it, you will have to redo all that from scratch. Plus, you're billing actual time to remove information. And you get no benefit from wasting your time.

                                  I can't think of one example where I felt that it would be better to leave something linked when the project was finished than to cut the ties. And more often than not, when I forget to break those links it bites me in the a$$.

                                  Oh, I don't doubt that, but it's just because you don't know how to handle things. How about this, since you've done everything imaginable, you've probably been in this situation. An assembly where several parts are made from a single complex shape. Like a mouse. You use the outer shape as the master model. Now you split the buttons and top. And now you break the links.

                                  Next, the marketing department wants a child's version of the mouse. Your complex shapes in the buttons and top are all dead. As good as imported geometry. You've got nothing. You have to start again. You've taken 1 hour of work and made it into a week. It just has to happen once to make it possible. Meanwhile breaking links gives you no advantage.

                                  c31f003.png

                                   

                                  And as I mentioned, there may be instances where you are planning on reusing that intelligence, you can just lock those relationships and then after the appropriate pack and go to a new project folder, unlock and start hacking away at the new modified design.

                                  Locking is an entirely different thing. You've got to think of that before you do it. I see no advantage in breaking links at all. You should forget about that function altogether. Unless you're going to make a library part out of something that was originally designed in-context, and that's pretty unlikely. You should also learn about the Freeze capabilities, and how to open parts - even parts with live links - such that they don't see the parent or child document. There are renaming tricks you can use to temporarily sever links, moving files, opening parts without the assemblies, making one assembly for in-context, and another for things like motion or rendering where you need to do stuff that would destroy the links - lots of stuff if you just understand how the links work.

                                   

                                  The only time I can imagine that the links being left in would be useful is in an organization where the output is fairly repetitive and everyone involved is carefully trained on the relationships and how to properly use them.

                                  What is the advantage of breaking the links? It takes extra time to do it, and you lose information/control. Even if you're never going to see that assembly again, what is the advantage? There is none. You're taking extra time to hog-tie yourself.

                                   

                                  Yes, you have to train people on how to manage links between files. It's very possible to manage links successfully. It sounds like you need that training. People make bad decisions (like breaking links) every day just because they don't understand how it works, and they're afraid of it. This breaking links nonsense is one of the fallacies I really wish I could debunk.

                                  Matt,

                                   

                                  I suppose you've managed large projects with teams working on assemblies in excess of 20-40 thousand parts rather than just a mouse with four parts?

                                   

                                  If I wanted to put that mouse to bed, I would break all the links.  What happens when you send file A to vendor 1 and file B to vendor 2 and they're requesting native files?  Now you've got to send multiple files or they get cherry bombs.

                                   

                                  To keep the links for future use, sure, one could archive a version with the links for modification purposes, but I wouldn't want to take the original files and have a new team member start monkeying around with those.

                                   

                                  But you know what's best...you and your four parts.

                                   

                                  Please get back to us when you've linked anything over 1,000 parts together and have successfully had a junior designer successfully make some modifications;-)

                                  • 104. Re: modeling methods
                                    Matt Lombard

                                    Dan,

                                    You don't demonstrate an idea with 1000 parts. In plastics design you don't have a lot of parts, you have a lot of features. Generally large assemblies work with parts with very few features, probably a lot of imported data for purchased parts. Short part trees don't have much complexity. A "mine is bigger than yours" argument really doesn't mean anything. You should learn how to deal with small situations before you get turned loose on large ones. Plus, part of what I'm exploring here is what to do in different types of design situations. It's not a matter of size, it's a matter of matching a process to a set of requirements.

                                     

                                    When I worked as CAD administrator, I made sure people knew how to handle problems, and if they couldn't, I was there to help them. I didn't sacrifice the goals just because one person didn't have a particular skill.  Deleting the value of the design process wasn't part of what I was tasked with doing.

                                     

                                    If you want to give design files to manufacturing people, you have to make sure that they know how to handle it, or just give them what they need. Many times people don't understand what they are asking for.

                                     

                                    Plus, I'm really curious, what's the value of breaking relations over locking them?

                                     

                                    And then there's the question we haven't gotten to yet - what kind of associativity are you creating? Are you making part-to-part links in the context of an assembly (sketch 1 from part 1 references an edge in part 2)? A skeleton part inserted into individual parts? Multi-level links in top level and subassemblies? These are all different levels of complexity and reliability.

                                     

                                    If you are trying to manage rebuild times in assemblies, there are I'm sure some unturned stones we could have a look at. The concepts are the same with the large assembly, it just takes more planning.

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