12 Replies Latest reply on Oct 24, 2017 12:55 PM by Chris Pratt

    3D Sketch overdefinition is killing me

    Brian Smiley

      Hi all, first time posting, hope I'm not doing anything wrong.


      I'm trying to make a 3d Sketch for a welded frame I'm designing, and no matter what I do I seem to keep running into weird situations where Solidworks thinks the sketch is overdefined for reasons I can't even begin to imagine. I'll have a perfectly fine sketch, and then I try to draw a line connecting two points, or a circle concentric with another circle, and all of a sudden over half the relations in the sketch turn yellow or red even though I see little or no way in which the added element could possibly conflict with anything. Sometimes it even happens after deleting a sketch element, whereas before adding or deleting it the sketch seemed fine. I can't see how getting rid of elements can ADD to the defined constraints in the sketch.


      Attached is the sketch I'm working on. For an example, in the current version (which, by the by, is one of about 5 iterations I've gone through trying various approaches, so forgive me if the sketch construction seems weird, I've tried going circles then lines, lines then circles, etc.) if I go into the top plane and try to add a circle about the origin, errors pop up. Why on earth can't the sketch accomodate a circle about the origin? What is this conflicting with? Any advice on how to go about making this sketch efficiently? The end design is supposed to look something like a birdcage with weldments accross each circular "stage" as floor frames. These kinds of weird conflicts have been popping up in seemingly random places as I've tried to draw this thing, sometimes while drawing the vertical beams on the sides, sometimes while drawing in the "floor" stages (which aren't included in the attachment because that's where the error pops up this time).


      I really appreciate any help, thanks.

        • Re: 3D Sketch overdefinition is killing me
          Wayne Schafer

          With smart dimension high lited, uncheck(unhighlight) reference dimension icon.

            • Re: 3D Sketch overdefinition is killing me
              Brian Smiley

              Ok... sorry but I'm not seeing what that is supposed to do. As I expected trying it nothing changes in the sketch when I do this.


              I'm starting over again and I'll try to post a more demonstrative example of a sketch with a conflict when I get to one again.




              Here: I just started off drawing each stage on its respective plane, and now at the top circle for some reason it won't let me set the center of the circle as the midpoint of the centerline I want to include for positioning the top cage. If I select the center and the diagonal underdefined centerline and choose midpoint, all sorts of conflicts pop up which I don't understand, especially given that if you look at the level below the top one, such diagonal contruction lines are already included.


              This is very confusing and frustrating.

                • Re: 3D Sketch overdefinition is killing me
                  Kelvin Lamport

                  The top circle was already fully constrained and the ends of the diagonal centreline are already coincident to the top circle, so adding a midpoint constraint would cause the overconstrained error. Adding just a Coincident constraint instead worked for me.

                  • Re: 3D Sketch overdefinition is killing me
                    John Burrill

                    Brian, I understand your frustration.  Sketch constraints are based on solvers that generate a simulteneous solution.  When sketches get very large and complex, finding a stable solution becomes difficult.  For 3D sketches where you have twice as many degrees of freedom, it's not always a straight-forward process to fully constrain a sketch and I've had a couple of cases where I pulled and tugged on every segment and point in my sketch and none of them budged and the sketch was still under defined.  Similarly, if you have a stable solution and remove an element from it, the remaining elements can shift into an unstable solution.  An underdefined sketch is not easier or faster to solve than a fully defined sketch, so you might still get errors if you delete an entity.  Think of it like this, the software either has a solution or it doesn't  and if you change the make-up of the sketch, it's all up for grabs again.

                    Now I do have some advice.

                    First, unlike Pro-E and Inventor, Solidworks will let you add duplicate constraints to your sketches.  As long as there isn't a conflict, Solidworks will let you put a parallel relation between two lines that already have individual vertical relations constraining them without any issues.  However, duplicate constraints can produce a variety of computational eccentricities, so on complex 3D Sketches, you really want to be selective and systematica about how you mate something.

                    For example, deleting the Horizontal4 relation from your sketch will allow you to add the circle you described.  and if you have two arcs with the same center point, than they don't need to be concentric as well and if those same arcs have coincident endpoints, then they don't need to be equal.

                    Finaly, you might also look at making this part with patterned 2D sketches as they'll probably behave better.

                      • Re: 3D Sketch overdefinition is killing me
                        Brian Smiley

                        Thanks John, this is helpful. I've remade the sketch again, doing my best to minimize the number of relations. I got pretty far this time, and even added in three of the vertical series, but do you think you can tell why when I try to draw a series of segments vertically down on the remaining diagonal corners, I get an error when I reach the bottom? In fact, if I try to draw in the top plane, even putting in three arbitrary, unrelated to anything points gets me a bunch of rebuild/relation errors. I feel like I'm getting closer here but am still missing something. I thought that maybe not using sketch planes for the vertical lines, as they should be easy enough to define with already present points and "Along Y" type relations made sense.


                        Thanks for your patience.

                          • Re: 3D Sketch overdefinition is killing me
                            John Sutherland

                            What I have just realised is that Property Manager ordinates of 3D points constitute position and constraint but not Fix.  A seperate Fix relation is required to Fully Define the point, and any elements coincident with that point.


                            You may have 3D points, and elements coincident with them.


                            You might find helpful Virtual Sharps where elements intersect without automatically creating a point.

                    • Re: 3D Sketch overdefinition is killing me
                      Josh Killalea

                      i can't (be bothered) to download and check your sketch as it is a pain to transfer it from my laptop to the work computer to see whats going on specifically, but i do have a few do's and don'ts that i have picked up in the past 18mths using pretty much exclusively 3D sketches. a lot of this (pretty much all of it) i don't know the technical how's and why's, but it comes from experience. i have a system now for doing 3d sketches that is ultra stable and i almost never have confusing or troublesome 3D sketches any more. and 3D sketches are now one of my favorite parts of SW.


                      for the record i am writing this here because this came up in a search for me when i was looking for something else to do with 3D sketches. so i appologise if you already know all this but thought it might benifit someone else at some point.


                      DON"T use equals constraints in a 3D sketch. there is something about an equals constraint in a 3D sketch that SW just doesn't like. avoid them like the plauge. if like us you do a pipe run and need to show the bends, just tick the box in the fillet command that adds a dimension to each fillet.


                      DON'T use projected geomtry in a 3d sketch. SW will let you make all sorts of external links with your sketches so there is no need i can think of that you would NEED to do it.


                      DON'T use parrallel constraints. again, SW doesn't like them. eventually it will crack the shits with them and start throwing errors and it will make no sense as to why.


                      DON'T try and do everything in one sketch. i have developed a system for doing our pipe runs here that uses a minimum of 4 sketches to do one pipe run. there are reasons for this beyond what i am about to say, but suffice to say, to much in one sketch will slow it down and increase the risk of a clash. if you can, break what you are doing up into smaller segments. that said you can still get a lot in one sketch, but for us if we try and do a long pipe run in 1 sketch it becomes almost un-useable. plan your attack.


                      DO use a "construction sketch" if you are doing complex runs through 3D space. as above trying to fit everything into one sketch can cause issues and is slow once it goes over a certian size. so use a "construction sketch" if required to give you some points in 3D space to aim for and constrain to. this has a number of benifits also, but it is much easier to work with when adding the weldment members, especially when you have a heap of construstion geometry to hold the lines in the place you want them. you can turn the construction sketch off and are left with your frame or pipe run or whatever you are doing.


                      DO use perpendicular, and axis constraints as much as you possibly can. (with the obvious exception of dimensions, they are probably the only constraints i use in 3D sketches now). if u need to do a pipe run (or something else) that takes a 45 degree turn (or any other angle for that matter) use a X,Y or Z constrained combo of straight lines to constrain the line at an angle and then set an angular dimension off one of those lines to drive the angle. this has a few benifits, but seems to be the most stable. when constraining a circle in 3D space do an X,Y or Z constrained combo of lines to constrain the circle to the "plane" you want to see it in and from your centre point (dependant on the circles orientation) to the edge of the circle and then add the diameter (or radius) dimension. alternately you can add a point to the line and constrain it (with a coincident constraint) to the outside edge of the circle. this method isn't as stable though. teh absolute best bet for circles is to add a plane and do a 2D sketch on the plane. by almeans drive it with 3D geometry, but a circle in 3D space is just to unstable for good design and modeling. especially if you have some configurations in the part/assembly that are in some way related to to circle. sometimes you will run into an issue with the axis constraints "conflicting" because it is effectively doubling up on constraints in some instances, but they are normally easy to workout.


                      DO keep your constraints to a bare minimum. go one line at a time and make sure it is fully constrained before moving on. i know this sounds like it will take longer, but it is much faster because you don't have to go back and work out why your sketch is over constrained and where. it also means that if a sketch gets over constrained it is almost always the last one you added that is the cause, and as a result is much easier to work out where it is going wrong. you will still get pretty quick doing this after time.


                      i am sure that there are others, but these are the main ones i can think of now.


                      i do probably 75-90% of my modelling with 3D sketches and weldments now and stick to these rules and i never get any issues now. just to give you an idea of how stable these methods are my current job consists of about 25 or so pipe runs where the shortest run is 30 meters long in total and the longest is just over 300 meters, with the longest segment of pipe being 6m straight sections. i can run this model (along with a WHOLE lot of other sutff in it total model size of near 7000 parts/assemblies) no problems and get no rebuild errors at all.


                      again, sorry if you knew these things, but it might help someone else.