6 Replies Latest reply on Nov 4, 2008 7:24 PM by Scott Salmon

    Lost edges

    Scott Salmon
      Hi all. I'm new here, and to SolidWorks, but I'm pretty experienced in Pro/E, and top-down modeling.

      I'm working on a model that has three bodies that have been inserted into new parts. For the most part, everything has survived changes well, but where I have used edges to create a seal detail between parts, the references get lost when nearly any change is made to the master part, including minor dimensional changes. I can live with that, but all of the referenced features fail when I redefine the sketch to correct the problem. I can sort through it all, but it has become very time consuming.

      With Pro/E, there is a replace entity command that lets me swap orphaned references with newly created entities so that subsequent features don't fail. Is there such a command or a work-around in SW (2008, sp5)

      Also, is there a way to prevent these edges from forgetting where they came from? I'm not deleting basic geometry, just making minor changes to dimensions.

      Thanks in advance for any advice.
        • Lost edges
          Charles Culp
          Scott,

          It is imperative to use "convert entities" to get those edges into the dependent part. It is best to use "convert entities" on the sketches in the parent part, not the actual model edges.

          As for reassigning links, it can be done, but it is cumbersome. Edit the sketch with the faulty reference. Then go to Tools>Relations>Display/Delete Relations..., or use the button on the toolbar. There you will see a listing of all the relations in the sketch. You can narrow the types in the dropbox (or click on it in the viewing area), then select the relation that is bad. Under the "entities" header below, you will see the two items that are constrained to each other. Click on the "replace" button to replace a constraint.

          A little time in Solidworks and you will learn the best pratices so this isn't such a large problem in the future. One suggestion is to use sketches in the assembly as a "skeleton".
            • Lost edges
              Scott Salmon
              Thanks for the response.

              Charles Culp wrote:

               

              It is imperative to use "convert entities" to get those edges into the dependent part. It is best to use "convert entities" on the sketches in the parent part, not the actual model edges.

              I do have the three parts re-assembled in a construction assembly, but not the master. I suppose I could add that, but the geometry I need to reference is a mix between edges that have been inherited from the master, and edges that have been added to the referenced parts. (For example, shell edges from the master, and boss edges from the referenced part.) Is it best practice to put as much common geometry into the master as possible, or is it better to keep the master minimal?



               

              As for reassigning links, it can be done, but it is cumbersome. Edit the sketch with the faulty reference. Then go to Tools>Relations>Display/Delete Relations..., or use the button on the toolbar. There you will see a listing of all the relations in the sketch. You can narrow the types in the dropbox (or click on it in the viewing area), then select the relation that is bad. Under the "entities" header below, you will see the two items that are constrained to each other. Click on the "replace" button to replace a constraint.

              Nothing could be more cumbersome than what I am doing now. I'll give it a shot. Much of the geometry is edge chains or loops. What is strange is most of the edges seem to be remembered, but just one or two get lost.



               

              A little time in Solidworks and you will learn the best pratices so this isn't such a large problem in the future. One suggestion is to use sketches in the assembly as a "skeleton".

              That was my initial thought, but I was disappointed to see that sketches do not come along for the ride from the master when you insert a body into a part. I find it awkward to try to access sketches in an assembly where there are a lot of coincidental edges and sketches. My own unfamiliarity and preconceptions, no doubt.

                • Lost edges
                  Charles Culp

                  Scott Salmon wrote:

                   

                  Is it best practice to put as much common geometry into the master as possible, or is it better to keep the master minimal?

                  Good question. I'm sure there is someone else here who can answer this better than I can.

                   

                  That was my initial thought, but I was disappointed to see that sketches do not come along for the ride from the master when you insert a body into a part. I find it awkward to try to access sketches in an assembly where there are a lot of coincidental edges and sketches. My own unfamiliarity and preconceptions, no doubt.

                  Hopefully the terminology isn't an issue here. If you are using the Insert>Part.. tool to insert a body from one part file into another part file (not assembly) then you can also insert sketches, it is one of the options (make sure to drill down all the headers in the feature manager when you import it). If you are speaking of inserting a part into an assembly, then you should also be able to select the sketch from the part. Make sure sketches are visible (under View>Sketches), and then find the sketch in the feature manager tree, right click on it, and also make it visible.

                  Either way you should always be able to reference underlying sketches, which will typically produce more robust references.
                    • Lost edges
                      Scott Salmon

                       

                      Hopefully the terminology isn't an issue here. If you are using the Insert>Part.. tool to insert a body from one part file into another part file (not assembly) then you can also insert sketches, it is one of the options (make sure to drill down all the headers in the feature manager when you import it). If you are speaking of inserting a part into an assembly, then you should also be able to select the sketch from the part. Make sure sketches are visible (under View>Sketches), and then find the sketch in the feature manager tree, right click on it, and also make it visible.

                      Hmm. You have it right, I think. From the parent part (I've been calling the master), I right clicked on the body I wanted to insert into a new part file. The save as dialog box pops up, and that's the end of it. I didn't see a check box or anything that mentioned sketches. Did I save too much time?



                       

                      Either way you should always be able to reference underlying sketches, which will typically produce more robust references.

                      In some cases, I could have used sketches (if I had figured out how to bring them along), but some of the splits fall in the middle of lofted geometry and drafted surfaces, so the resultant edges are not related to the original sketches. We do a lot of swoopy stuff.

                      I thought about creating reference sketches in the parent part that used edges from splits so that the references wouldn't get consumed by future features, but when I couldn't figure out how to bring them in to the reference parts, I guess I gave up on that plan.

                • Lost edges
                  Charles Culp
                  Scott,

                  You are correct. If you use the Insert>Molds>Split command, or just save off the body, you do not get to save the sketches with them. Now, however, we are in a completely different domain than I originally anticipated with this discussion.

                  I would call this technique a "master model" technique, not necessarily "top down" modeling. When you say "top down" I think of an entire assembly of parts, all controlled at the assembly level. "Master model" to me, says one finished part, or in your case, a pair of parts that mate together.

                  I think there are a couple things for you to consider. One is that Solidworks handles multiple bodies in the same part file. I know that is different than Pro/E, so I didn't know if you were used to designing that way. When I design swoopy plastic parts that mate together (like I am doing as we speak, I'm waiting for a rebuild to finish right now), I do it all in one part file. Then, at the very end, I separate it into multiple pieces/bodies. I add any features defining the mating surface within the one part file (lip/groove, etc). I don't actually ever split into two part files, but you sure can.

                  I suggest doing that and only saving them as separate parts, without adding any features in the child parts. Only do this if you need to control them as separate parts by your PDM/engineering control requirements that say they need to be separate files. You also might want to do it so they are separate files for addition later to a larger assembly, however I don't do it that way. I simply make multiple configurations for each body, and use "delete body" function to delete all but the one that I want.

                  So, I guess I'll end with a question, which is what type of features are you adding to the parts after they are split/saved off as another part file, and can you add those just to the main part file?
                    • Lost edges
                      Scott Salmon
                      Thanks. That's helpful.

                       

                      So, I guess I'll end with a question, which is what type of features are you adding to the parts after they are split/saved off as another part file, and can you add those just to the main part file?

                      That's the question I asked myself when I embarked on this method. Unfortunately, I guessed at the answer.

                      Actually, I did a little more than guess. To compare the two methods, I brought the master to a certain point and added features to the master. I saved a copy, deleted those features and added them to the split/saved parts. At the time, I couldn't see any major advantages or disadvantages so I ended up choosing the latter because I thought I would have trouble splitting parts along the somewhat winding intersections at the lip joints if all of that detail were in the master. The way I have it seems to work well, as long as there are no changes to the master. Unfortunately, there are always changes...