69 Replies Latest reply on Jun 15, 2010 11:13 AM by Lenny Bucholz

    Solidworks 2010 is a piece of !#$%@.

    Emilio Graff

      I cannot work with this crap anymore. For about 6 hours now I've been working on an assembly, which Solidworks is succesfully ruined for the third time. Sometimes I open the file, and all the mates are "overdefined", even though I had been working with it without problems for hours before.

       

      Now even though I have "don't you dare flip the alignments on my ^^%^%* mates", it's flipping them. Something new---that I've never seen---it's asking me to flip mates when I rebuild! Are you &#$&#% crazy?

       

      So after carefully manipulating this assembly, I check it and hit save and.... too bad. A mate was flipped and now I have to start over again.

       

      *DON'T* buy Solidworks until SP5.0. And *DON'T* get support. I'm not even going to try to explain this to them. "Can I have your assembly?", they'll ask. No, you can't.

      • Reply
        • Re: Solidworks 2010 is a piece of !#$%@.
          Tom Smith

          You're too angry.  Relax.  It's Friday, go home and it'll work great on Monday.

           

          Did you just change your avatar or has it been the image of you smashing the computer for a while? 

          I figure it's been for a while because your previous rant topics include:

           

          The Awesome Error Message Thread

          The $8000 vector plot

          Who else hates the left-click pop-up menu

          Favorite thing to do while Solidworks thinks

          Not yet implemented

           

          I don't know, man.. Maybe this SolidWorks thing isn't for you.

            • Re: Solidworks 2010 is a piece of !#$%@.
              Emilio Graff

              Believe it or not, the avatar is straight out of a promotional email from Solidworks about a year ago....

               

              It's been a while because I gave support an honest chance. Now I have a good collection of ER's and SR's and never-gonna-happen's. And the fact that I wasted the entire day trying to get a 10 part assembly not flip itself inside out every time I look away from the screen for 10 seconds is just the straw that broke the camel's back.

               

              I drag a part by hand and everything updates correctly. If I set a mate for that part that keeps it just a fraction of a mm from where I dragged it the whole thing turns inside out.

               

              There's been some changes to the way mates are handled and 2010 is very sensitive to having overconstraints, like the "easy" 3-plane mate which overconstrains a part. In 2007 it wouldn't cause a problem until you had thousands of mates. In 2009 it was more sensitive, and now you can't have even 50 mates before it @#$^@# itself.

               

              So if you correctly constrain parts (plane, line, and point) then it randomly flips the orientations whether you like it or not.

               

              My real problem is that I'm trying to use Solidworks to make models. What I should do is just give it up and treat it like a fancy drawing program.

                • Re: Solidworks 2010 is a piece of !#$%@.
                  Dustin Biber
                  Do you have incontext parts? Or at least features that reference features of other parts in the assembly?
                      • Re: Solidworks 2010 is a piece of !#$%@.
                        Dustin Biber

                        I have found in assemblies that had a non-clear hierarchy of driving features, that I would have similar issues... in addition to rebuild icons always staying on.  Basically a circular reference.  Not a circular reference in the traditional sense where there is no one driving the bus, but one that bogs solidworks down nonetheless.

                         

                        I tried to find a link that Matt Lombard used to have on his site.  It did a good job explaining the circular reference problem.  He has a section on it in his book.  I will paraphrase it here.  All due credit to Matt:

                         

                        Mating parts to in-context features creates a parametric daisy chain, thus establishing an order in which assembly features and mates must be solved.

                         

                        He goes on to explain:

                         

                        The Assembly FeatureManage is solved in this order, or an order that is very similar

                         

                        1.  Solve reference geometry and sketches that are listed before parts in order, at the top of the design tree

                        2.  Rebuild individual parts as necessary

                        3.  Solve the mates and locate the parts

                        4.  Solve in-context features in parts.

                        5.  Solve reference geometry and sketches listed after the mates

                        6.  Solve assembly features and component patterns

                        7.  Loop to step 3 to solve mates that are connected to anything that was solved after the first round on the mates

                        8.  Continue to loop until complete

                         


                        So if you have a primary part that gets stuff mated to it and then gets some in-context features based on those mated parts... you may have the beginnings of a circular reference issue.  If those mated parts also get some in-context features based on different features on the primary part, the assembly will quicky become overworked.

                         

                        A best practice is to attempt to create your mating structure and in-context relationships as linear as possible... so the rebuild only goes through the list once.  This will help prevent SolidWorks from losing its marbles.  It will also speed up large assemblies.  One method for doing this is the use of skeleton sketches.  Do a search on here for "skeleton sketch" specifically posts from Mauricio Martinez-Saez.

                        Here is a good one to start with:

                        https://forum.solidworks.com/thread/27640

                         

                        Good Luck

                          • Re: Solidworks 2010 is a piece of !#$%@.
                            Emilio Graff

                            Dustin,

                             

                            It's nice to have a concise summary here. Thanks for that.

                             

                            However, I'm 90% sure in this case I have not even an inkling of a circular reference. I've used SolidWaits since 2003. In 2006 I had my first taste of circular reference, and embarked on the skeleton sketch approach. Last time I had an accidental circular reference (that I knew about) was in late 2008. Since I've joined this forum to start complaining I've made a concerted effort to learn the techniques required to "work around" (or "follow", depending on whether or not your glass is half empty) SolidWaits's "methods".

                             

                            In this case my assembly has but 10 parts or so. I've made skeleton sketches so that I am not mating relative to features that may change. In fact, I have given up having the origin in a logical place and now I just mate parts that I will design in context simply to the origin of the main part (one step beyond just leaving it fixed on insertion). Parts that I need to move around to evaluate design options (the main reason I'm doing things with references) I made to planes and sketches instead of features.

                             

                            I'll give you an example of what happens. I have a gear train laid out. The distances between gears is defined, but not their position, that is, I will later move them around each other to "fold" the gear train into a volume I can pack according to other things in the system. All of a sudden, I want to move a gear out farther. Its face is mated to a line on a sketch. So I edit the sketch, create a new line, exit, then edit the mate and change it. Boom, the whole thing explodes. If I cancel the mate, the explosion is only half contained, and undo won't fix it. So mates have flipped and there's no way I can get it back without a backup copy. So you save all the time in case it crashes, but if you save all the time....

                             

                            If I instead delete the mate, drag the gear towards the new line, and rebuild, everything is fine. If, once it's close to the line, I apply the new mate, it works. So yeah, great, I have a "workaround" (my glass is half-empty, in case you can't tell). But there goes the three hours it took to bring everything back to where I was before the first explosion. I'm pretty sure we can all agree that reversing a wild train of SolidWaits mate flips is impossible without deleting every mate and starting over.

                             

                            And every time an explosion happens, even if cancelling the mate successfully unexplodes things, inevitably *every* semicircular arc tangent to straight lines (otherwise known as a machinable slot) will flip the arcs to the other side of the "end" of the slot (so it looks like a really wide letter i in a serif font). The only way to "flip" them back is to delete them and redraw them, as far as I know. Thank goodness they didn't block the ALT+ keys for sketch relations.

                             

                            I don't plan on pretending that I can even begin to understand the algorithms required to figure out mate flipping logic. But what I *do* understand is that SolidWaits engineers don't understand them either. There seems to be no effort to attempt to guess which combination of flips results in the least number of flips. Again, I can't say much here because I can't write pseudocode to solve the problem. But I'd be willing to bet even if I could write C code it would be $6k of subscription until I saw it implemented.

                             

                            Oh, and you may say, "You should check the option to have it warn you about flipping mates before doing it." Trust me, when I found out about that option it was like a miracle. In 2009 it did the job. But I'm convinced that in 2010 it gets partially ignored. In fact, After the first explosion, it started asking me about mate flipping about 15 times each rebuild. I have *never* seen it ask me during a rebuild before.

                             

                            The only other possibility is that construction lines are getting changed back to "real" lines in sketches---akin to 2009's "Let me randomly change your dimensions during rebuild and not tell you about it." Because this mate flipping is such a pain that one part which I've had to continuously rotate and mirror in evaluating design options I simply sketched it in four different orientations and just switch back and forth between construction and real lines instead of trying to flip it with mates. And that part, my friends, has flipped before my eyes at least twice. The first time, I thought I had made a mistake, so I repositioned everything that is based on it, not knowing that it had flipped. So of course when I bring this in to the main assembly everything is backwards, and I had to start over. Then the explosions started....

                             

                            What I *do* know about mate flipping is that it used to be almost 100% preventable by overconstraining parts. Say, three plane-to-plane mates. I know that as far back as 2007 if you tried to properly constrain parts the mates would flip much more often. In 2009 this "technique" could still be used, but 2010 is much more sensitive to "locking up" with both overconstrained mates and sketch relations. Never until this version have I had to delete sketch entities in the simplest of sketches and start over simply because I couldn't for the life of me figure out why it wasn't solvable. All SolidWaits versions that I remember had this problem, but only once I got to the thousands of mates or hundreds of relations in crazy unnecessarily pretty sketches.

                             

                            Oh, and as far as rebuild goes, SolidWaits most certainly does way more rebuilds than it needs. And if you have a repetititve feature (say, teeth on a rack) you will be reading this. Because whether or not you tell SolidWaits to suppress automatic rebuilds, it will forget in a few cycles. If there's even a hint of a mate to the complex part, it will get rebuilt for no reason.

                             

                            I'm running this on the highest clock rate Intel makes with 12 gigs of RAM and it's not that much better than your old "inspiron". I already gave up on it actually using multiple processors for anything but rendering so I just opted for the highest clock rate I could get. And, well, I guess I can still get a second batchelor's degree with the fastest processor money can buy. Don't even get me started on Simulation, where you get latent error messages 45 minutes into a single-processor analysis....

                             

                            The only change in SolidWaits I've been able to inspire in them (or at least I think I did) was to be able to deactivate the license without running the program. My Price Added Reseller has flat out told me they don't know how to deactivate licenses. So if your hard drive crashes, well.... That feature isn't coming until 2011, and, by then, my subscription will have expired, and I doubt I'll renew.

                             

                            The *real* question is---you pay a gazillion dollars for Catia: does that guarantee anything? Isn't it all Wallet D'Assault? Is everything else based on Parasolid the same garbage?

                             

                            If you get to this line you either need to simplify your assembly or find a book to read.

                              • Re: Solidworks 2010 is a piece of !#$%@.
                                Kelvin Lamport
                                I want to move a gear out farther. Its face is mated to a line on a sketch. So I edit the sketch, create a new line, exit, then edit the mate and change it.

                                Why not just move the line the gear is mated to? Why draw a new line and re-mate?

                                 

                                If the original line was drawn from top to bottom (or left to right) and the new line was drawn bottom to top (or right to left), that might be causing the flip.

                                 

                                I've made skeleton sketches so that I am not mating relative to features that may change. In fact, I have given up having the origin in a logical place

                                You need to read the many posts Mauricio Martinez has made on this in-context approach. He is probably the foremost expert on this technique.

                                • Re: Solidworks 2010 is a piece of !#$%@.
                                  Mauricio Martinez-Saez

                                  Emilio,

                                   

                                  I understand your frustation, however, there may be an small possibility that the cause of your problems may be the result of an incorrect way to build the assembly.  I say this without knowing your model because all the work we do is parametric and we never experienced those problems.

                                   

                                  Believe me we are aware of the many problems and "bugs" inside SW, and we know that with few exceptions, VAR's can not solve the majority of user's real life problems, we also know that SW is not a 100% perfect CAD application (so far we do not found any without problems), but in our experience it is not a complete piece of !#$%@.

                                   

                                  If you post or send me a small example of what you are trying to do showing the problem (a small assembly with some simple parts), I may take a look at it and see if I found the problem.

                                    • Re: Solidworks 2010 is a piece of !#$%@.
                                      Emilio Graff

                                      Mauricio,

                                       

                                      As much as I look forward to any opportunity to learn from you directly, I cannot send out this assembly, which is often the case with the work I do.

                                       

                                      However I will have to decide at some point to set some time aside and try to reproduce this and other problems as simply as possible.

                                       

                                      When I get to it, I'll post back here.

                                        • Re: Solidworks 2010 is a piece of !#$%@.
                                          Emilio Graff

                                          Here's one example, although not of mate flipping.

                                           

                                          Try to add a midpoint relation between the endpoint of the blue construction line and the other blue construction line. Sketch freezes up; unsolvable. Why?

                                            • Re: Solidworks 2010 is a piece of !#$%@.
                                              Emilio Graff

                                              In this assembly (when it had all the parts in it, which I can't upload) an angle mate between two planes flipped without warning during one of the rebuilds. As in I mated the part, make other parts relate to this part, work for two hours, and all of a sudden I come back and the angle is wrong. Since it was 45, I don't know if it flipped orientation or what.

                                              • Re: Solidworks 2010 is a piece of !#$%@.
                                                Mauricio Martinez-Saez

                                                Emilio,

                                                 

                                                At this moment I only have SW 2009 loaded on this machine (we are finishg a large project and we will not place 2010 in production work until this project is not finish), so I can not see your example, if you can load an example in 2009 I will take a look.

                                                 

                                                Let me say that from time to time we experinced something similar with sketches, particularly if we use any sketch path inside the sketch, then when we anlayze the sketch we allways discover that the sketch was overdefined in a way that when entities try to move the software can not found a solution for the relations.  Normally this hapen to us when creating very large and complex sketchs and then add or modify part of it adding more relations.  Normally the sketch don not show the "overdefine" error until the sketch don't change dimensions or position of some of the entities, while being driven by a DT or by another upper level sketch.

                                                 

                                                But I must say that so far in all cases the error was produced between the computer screen and the backrest of the seat in front of the computer....

                                                  • Re: Solidworks 2010 is a piece of !#$%@.
                                                    Emilio Graff

                                                    Mauricio,

                                                     

                                                    The sketch I uploaded is as simple as it gets. See the screenshot. As others have mentioned, dragging the end point first, then trying the relation, or simply dragging the endpoint to create the relation works. It is a 3D sketch, which always have more issues than 2D sketches, but this is really ridiculous.

                                                     

                                                    sketch.png

                                                      • Re: Solidworks 2010 is a piece of !#$%@.
                                                        Damian Gillespie
                                                        Go figure http://www.youtube.com/watch?v=nQmlQWI_d68 This is a video of the issue with what i am seeing. A concentric mate. Is that right
                                                          • Re: Solidworks 2010 is a piece of !#$%@.
                                                            Emilio Graff
                                                            Great video. Wayne should link to it in the report to his VAR. (I have my VAR busy with a few other things.)
                                                              • Re: Solidworks 2010 is a piece of !#$%@.
                                                                Mauricio Martinez-Saez

                                                                Emilio,

                                                                 

                                                                In my opinion, what the video at Youtube show is just the incorrect way to try to achieve something with a non "solid" construction of geometry.  Always there are several ways to do something, and sometimes some of them are not the most proper way.

                                                                 

                                                                As ypu know, geometry inside a CAD is just mathematics and internal equations,  therefore geometric construction should be build in a way that it uses the most simple math possible or at least build it on a way that a complex calculation is split into more simple expressions that can be resolved linearly.

                                                                 

                                                                We all know that SW is not able to do everithing, but sometimes, people try to do things in a way that they convert the possible into the impossible, the video at Youtube is an example of one of those instances.

                                                                  • Re: Solidworks 2010 is a piece of !#$%@.
                                                                    Emilio Graff

                                                                    Mauricio, the YouTube video is of what happens in the sketch I posted here. It is a 3D sketch with a few lines and very few relations. It perhaps shows too many attempts, but basically when you try to make the endpoint the midpoint of the construction line, it cannot solve the sketch unless you drag the endpoint first or simply drag it directly to the midpoint to make the relation that way.

                                                                     

                                                                    I'm no good at probability, but I seriously doubt that I randomly put that endpoint in space at a place where there is a singularity in the equations. I'm willing to bet the bug is much simpler than that. As I've said before I cannot imagine the sophistication of the algorithms behind mating and relations. But if the simplest of 3D sketches cannot work, then, as you said, there's no point in trying to use that feature.

                                                                     

                                                                    Yesterday I redid this small assembly following your advice of using planes and 2D sketches. Since it's a simple arrangement, it's hard to tell whether it's more stable. But it certainly was more complicated for me, especially because I had to use the new reference plane creation interface which at a few times made no sense to me. The new interface is much like mating, except it seems to absolutely prohibit both underconstraining and overconstraining the definition of the plane. I had trouble deciding how to create one of the planes because what I thought was a proper set of relations it thought it was overconstrained.

                                                                     

                                                                    If I'm laying out optics in 3D for a system with even 20 elements I can imagine trying to do it with 2D sketches will be an art form to learn in itself.

                                                                     

                                                                    I should also note that simple sketches "jamming" like this is new to 2010 as far as I can remember. 2009 is already a blur to me but I don't remember having problems with sketches this simple. And I certainly didn't have problems like this in 2007.

                                                                      • Re: Solidworks 2010 is a piece of !#$%@.
                                                                        Mauricio Martinez-Saez

                                                                        Emilio,

                                                                         

                                                                        Maybe in 2010 SW have an "additional" bug in the 3D sketches, I do not know that since we do not use 2010 yet in actual production work (first we need to finish a large project on which we do not want to take any chances).  To bad if 2010 have a serious regression on the alrady defective functionality of the 3D sketches...

                                                                         

                                                                        By looking at the sketch appear to me that you are modeling a Prism system, such as a Pellin-Broca, Abbe, etc. to filter a particula wave lenght, or perhaps something like an Amici prism to use on spectrometry, etc..  On any event, optical instuments of any complexity can be modeled in SW using "solid" construction geometry to be fully parametric, in some cases 3D sketches will work if their entities are created using the propper secuency (so SW can resolve the math, without creating an error), on other cases a construction using 2D sketches and planes will be more solid and will not produce errors as input parameters are changed to produce another geometry.

                                                                         

                                                                        As mention I am not a fan of 3D sketches or part feature to part feature mates, and as much as possible I try to not use that functionality, so far I was able to model almost anything I tryed using more basic functions, and believeme we do very complex models some of them with geometry as complex as what is needed on complex optical devices.

                                                                          • Re: Solidworks 2010 is a piece of !#$%@.
                                                                            Emilio Graff

                                                                            Mauricio,

                                                                             

                                                                            In this case the optics are extremely simple---I'm simply trying to place two fold mirrors which may or may not provide a 90-degree beam change. So I draw the "ray" in solid lines, then take construction lines at where the mirror would be, and make one line join the incoming and outgoing beam, and the other line go from the mirror point and the midpoint of the construction line. Then make the two construction lines perpendicular. All this is doing is making one construction line the angle bisector of the incoming and outgoing ray. So then I take my mirror and mate its origin (on the reflecting surface) to the intersection of the incoming and outgoing beam, and make a plane perpendicular to the angle bisector. So if my beams change from a 90 degree angle, the angle bisector will set the correct angle on the mirror.

                                                                             

                                                                            Being able to drive optical components around with "ray sketches" is integral in the early stages of the design. It is simply too difficult to do this with optical design software (which has a spreadsheet interface for positioning elements, and obviously does not show any mechanical parts). Once the optical layout is close to final in SolidWaits, you can transfer this to optical design software, and from there export a 3D model to import into SolidWaits and see that everything is where you thought it was. From there you can also export rays, etc., and avoid having to do much with sketches in SolidWaits.
                                                                              • Re: Solidworks 2010 is a piece of !#$%@.
                                                                                Mauricio Martinez-Saez

                                                                                Emilio,

                                                                                 

                                                                                About the "reflection" system you are trying to model... let me know if on the optical sistem you are trying to do you just need to reflect the beam in the same plane (origing (A), reflection point 1 (B), refection point 2 (B) and destination point of the ray (C) being co-planar), changing the angle of reflection and perhaps the possition of the plane, or do you need to do the reflection of the ray with points (A, B, C, D) being not on the same plane.   For example having the origing of the ray in a fix position and moving the mirrors in order to place the destination of the ray on any posible coordinate (for example this will be the case of a mirror system for a 3D laser scanner).  If you explain a little more your needs and constrains, I will try to do a parametric sketch (or sistem of sketches) to do that (and maybe can be done in 3D sketch if controlled properly).

                                                                                 

                                                                                I have done some similar work for large 3D scanners and for Topographical Laser Total Stations (a long time ago) and in fact I done exactly what you descrive (use the 3D CAD to simulate and test the lay-out before using the optical design software (which at the time have no graphical interface at all, just numbers and more numbers...), then we do the final calculations on the ODS and produce a data file to feed back into the CAD and drive the geometry to exact positions.

                                                                                 

                                                                                At that time I was not working with SW, but I believe that SW can do the job, even better that the CAD software we use at the time.

                                                                                 

                                                                                If I interpret correctly what you need to do... you will like to build a parametric model to which you can feed back the data from the optical design software to control the position of the components (perhaps using a DT, or feeding the data directly into SW variables using an API) and automate the model.  Is this correct?

                                                                              • Re: Solidworks 2010 is a piece of !#$%@.
                                                                                Emilio Graff

                                                                                In any case, I think I can get used to doing everything with multiple 2D sketches. It's a bit annoying because you can't drag things and see positions change "live", but dragging doesn't work in 3D sketches half the time anyway.

                                                                                 

                                                                                It's obvious the 3D sketching framework came long after the 2D sketches.

                                                                                 

                                                                                But I should say in 2010 I also get inexplicable jams in 2D sketches. Nothing as obvious as this. When it happens I usually delete the troubling entity and redraw it because often that's faster than trying to see if a "snap" created a relation I didn't want.

                                                                                 

                                                                                My advice to you is to not touch 2010 unless you see a feature in "what's new" that you like, and then come here and ask if it's really what you think it is. Even then, I wouldn't touch it until SP5.

                                                                                 

                                                                                The only feature of any use I can think of right now is virtual parts: you can create parts in assemblies that are saved internally, and whenever you want you can switch them to be externally saved. Helps a lot at the early stages of design, but it's nothing that can't be overcome with careful file management.

                                                                                  • Re: Solidworks 2010 is a piece of !#$%@.
                                                                                    Mauricio Martinez-Saez

                                                                                    Emilio,

                                                                                     

                                                                                    Starting in 2007, We never install eny new version before SP 4 or 5,  if you look at my picture (Avatar) that is a picture taken just after updating to a SP 1.0 in 2007 in the middle of a large project and make the mistake of converting the files to the new version...

                                                                                     

                                                                                    Virtual Parts (saven inside the Assembly) exist in 2009, however in some instances they also create a big problem (like suddently dissapearing form the entire assembly, and then there is no file no place in the computer...), so we only use them for things like sealing materials, paint, welding material, etc.

                                                                    • Re: Solidworks 2010 is a piece of !#$%@.
                                                                      Wayne Tiffany

                                                                      I find this 3D sketch quite interesting in that trying to add the midpoint relation as it sits will fail.  But move the end of the line a bit and try again and it will work.  Have you turned this in?  If not, may I?  I think it's a good, concise example of a deficiency that is repeatable.

                                                                       

                                                                      WT

                                                                      • Re: Solidworks 2010 is a piece of !#$%@.
                                                                        TRUNG DO

                                                                        Hi:

                                                                         

                                                                        1. I think I have solved your problem. If you just simply open your sketch and turn on the "front" view, you will notice that your blue construction line with the free endpoint is "snapped" to the longer not fully defined black line. SW has inference that this end point lines somewhere on a plane perpendicular to the screen and passing through the longer horizontal line. I simply picked the free endpoint of the blue sketch and dragged it to the lower right hand area to the right of the 65mm line. Next I selected the free endpoint and added a midpoint mate between it and the other blue construction line. I worked. I hope this is what you are looking for. See below for soem other cases that I have ran across.

                                                                         

                                                                        3. It is my experience that lines/features that are not fully defined sometime will "move" as mates are added to them. I believe that fully defined "solid" lines will help you in creating sketches. I usually add temporary dimensions to 3-D sketches before attempting to add fillets since a fillet with a radius that is larger than a line will cause it to "flip" or appears to have the mates "flipped". I recommend that you use distance of "zero" to replace all "coincident" mates.

                                                                         

                                                                        4. Before switching mates, I usually convert concentric, tangent, and coincident mates to "parallel" mate first. Next, I would then convert the parallel mates to whatever mate that I am trying to do. Parallel mates are like a "neutral" mate.

                                                                         

                                                                        My thought is that SW2010 SP3.1 needs to have the solid black lines fully defined. Try it and see.

                                                                         

                                                                        Sincerely,

                                                                         

                                                                        Trung Do

                                                                        Courion

                                                                        trungqdo@yahoo.com

                                                                  • Re: Solidworks 2010 is a piece of !#$%@.
                                                                    David Demaria

                                                                    Emilio, this may be off-target but I was once warned about this setting in options that can lead to similar issues that I believe your describing here (see attached file).

                                                                     

                                                                    Alternatively, you might want to look further into this thread... https://forum.solidworks.com/message/104102#104102

                                                                     

                                                                    Are you using flexible assemblies in this master assembly by any chance. They have given me the sort of problems your decribing here also.

                                                                     

                                                                    If we can at least eliminate these possibilites as being the likely culprit, then we have a better idea where to go from here.

                                                                      • Re: Solidworks 2010 is a piece of !#$%@.
                                                                        Emilio Graff

                                                                        David,

                                                                         

                                                                        I have this option turned on, because I simply cannot have any sort of top-down design without it turned on. If it's off, then basically you are stuck making a single assembly, which I've tried before (in 2007) and is a total nightmare. At least 2007 was stable enough that I could have thousands of mates before it seized, but I can guarantee you it's impossible to do in 2010.

                                                                         

                                                                        If you were told this advice by a VAR, beware that I've noticed mine sometimes gives "let's assume they're idiots" generic advice. Obviously turning on this feature makes it even easier to add circular references since you really have no idea what you're selecting on the screen when you click on something (unless you use "select other...").

                                                                      • Re: Solidworks 2010 is a piece of !#$%@.
                                                                        John Burrill
                                                                        I think CATIA uses its own kernel.
                                                                      • Re: Solidworks 2010 is a piece of !#$%@.
                                                                        Jay Andrews

                                                                        Enough with the excuses and the assumption that it's just user error.

                                                                         

                                                                        Here I have super frustration.  Already behind schedule with a drawing package due to making the mistake of upgrading to 2010.  As you can see here, there are no error messages or flags or whatever, my concentric mate is perfectly happy sitting there out of position perpendicularly.  If I enable the coincident mate there, it says can't do it, parts are constrained at 90 degrees or something to that affect that goes along with the snapshot you see here.

                                                                         

                                                                        I am disgusted at the direction of non-usability that SW seems to go more and more over the years.

                                                                         

                                                                        Although the OP seems too angry, so do I, and I don't like it, but we are trying to do a professional job here, and this expensive professional program just works against you more and more with each release.  This morning I told my supervisor if it were up to me I would switch to Autodesk Inventor because I am so sick of these productivity drains and just general non-reliability.  I upgraded to 2010 to get past the bugs in 2008, but surprise, all of my same bugs I was avoiding have still not been fixed by 2010 sp 3.1 !!!!!!!!!!!!!!!!!!!!!!!!!!!!!  Plus of course there are three-fold more new ones it seems for good measure.

                                                                         

                                                                        NOTACIRCULARREFERENCE.JPG

                                                              • Re: Solidworks 2010 is a piece of !#$%@.
                                                                David Anderson

                                                                i feelyour pain man!

                                                                 

                                                                hang in there, monday is a long way off!

                                                                 

                                                                 

                                                                however, i must concur that SW2010 is following the trend established by previous versions of more "features" and less "function".

                                                                 

                                                                i would like to buy  seat of SW that has less "features" and more "function". for example, i'd trade dimension pallete, all the "expert" features and mouse gestures for design tables that work. seems like a fair trade to me!

                                                                • Re: Solidworks 2010 is a piece of !#$%@.
                                                                  Kelvin Lamport

                                                                  "I'm not even going to try to explain this to them. "Can I have your  assembly?", they'll ask. No, you can't."

                                                                   

                                                                  Why not?

                                                                    • Re: Solidworks 2010 is a piece of !#$%@.
                                                                      Mauricio Martinez-Saez

                                                                      Kevin,

                                                                       

                                                                      In several ocassions SW requested form us the assembly file to try to identify a problem or a bug, however, in our case, we can not release a complete assembly outside our company, since they contain proprietary technology.  Sometimes we can supply a Sub-Assembly, or create a "fake" product assembly that can show the same problem, but we can not do that with a 950Mb assembly having 2500 parts (create a "fake" of that size will take a couple of weeks and we need to work).

                                                                       

                                                                      We will have no problems with the VAR coming to our office and try to identify the problem, so he can make a test model and send it to SW, but they do not do that, they what us to provide the assembly so SW can identify a software problem... I believe that the VAR should do that work, but that is only my opinion.

                                                                        • Re: Solidworks 2010 is a piece of !#$%@.
                                                                          Matthew Lorono
                                                                          Non-disclosure Agreements are par for the course in issues of proprietary IP.  Our VAR has signed one, and I'm sure SolidWorks themselves would sign one too if asked.
                                                                            • Re: Solidworks 2010 is a piece of !#$%@.
                                                                              Derek Bishop
                                                                              I hope you are spared the pain of ever having to get SolidWorks to sign a non disclosure agreement. I did it once and would work hard to avoid doing it again. It has to go through their lawyers. Lets just say they work to a different time frame to designers and engineers. Based on my experience allow at least a week for them to review the agreement and expect them to request changes. You the designer ends up with the monkey on your back.
                                                                              • Re: Solidworks 2010 is a piece of !#$%@.
                                                                                Mauricio Martinez-Saez

                                                                                Matthew,

                                                                                 

                                                                                I will have no problem to provide a complete assembly to SW if they sign a "Non-Disclosure Agreement" to protect our ITP, or even a simple letter acknowledging the receipt of confidential proprietary information, since they have the size and assets to respond for any violation and since they know how to handle and control confidential information.  However with local VAR's in this country I will not do that, since they can not control what their people can do with such information, on the other hand labor laws in this country will never allow a "confidentiality agreement" between an employer (the VAR) and his employees, to be used to take any legal action against a worker, not even to be fired without paying compensation provided by the Mexican Federal Labor Law.

                                                                                 

                                                                                We allready have some bad experiences with suppliers of components disclosing information to competitors and nothing can be done...

                                                                                 

                                                                                On any way, I believe that if we have a problem, and since the VAR is the "bridge" for comunications between users and SW, the VAR should make any efford required to understand the problem and provide SW with whatever explanation and examples showing the problem so SW can identify it and resolve the issue,  not go the easy way and request the user a copy of the model, without taking any time to understant the problem and how it happen.

                                                                                  • Re: Solidworks 2010 is a piece of !#$%@.
                                                                                    Emilio Graff

                                                                                    On any way, I believe that if we have a problem, and since the VAR is the "bridge" for comunications between users and SW, the VAR should make any efford required to understand the problem and provide SW with whatever explanation and examples showing the problem so SW can identify it and resolve the issue,  not go the easy way and request the user a copy of the model, without taking any time to understant the problem and how it happen.


                                                                                    Absolutely! I have mentioned this in other posts. Does anyone here believe that the giant assemblies they use to render pretty little splash screens have no problems? Why aren't they being used for testing? Actually, I should correct myself---they should be used for development.

                                                                                     

                                                                                    I've had experiences with our VAR where I simply had to "remind" them (as we say here in the US) that I'm paying for a service and I expect them to do it. I had a very clear cut problem that could be described easily in words and immediately was asked for a model. They should make the effort to create what they can themselves.

                                                                                     

                                                                                    The VAR is a nice human resources simplification, especially when dealing with customers in foreign countries. It is a nice filter for SolidWaits. I don't know why they chose to go with the car dealership model. It would make more sense perhaps if the VARs could be contracted to do design work, so they would run into these problems and do their own "Rx" sessions instead of having paying customers do it.

                                                                                     

                                                                                    And again, I've said it before. The sales model of SolidWaits is "a new version is the same as a service pack", but the development model is "a new version must include new features". So the closer to December you buy your subscription, the more likely you won't be able to use the new version. I remember having *serious* problems with SP4 in 2009 (sketch dimensions randomly changing during rebuild).

                                                                                     

                                                                                    You pay to get the software.

                                                                                    You pay to have the right to complain.

                                                                                    You pay to spend your time creating examples.

                                                                                    You pay to wait for the solution to be implemented.

                                                                                    And, hopefully, you *don't* pay with a mate flip before parts go to fab.

                                                                                     

                                                                                    Really it's a perfect model for SolidWaits. Either the customer learns to work around the problems or he doesn't get the work done. So what's it to them?

                                                                                      • Re: Solidworks 2010 is a piece of !#$%@.
                                                                                        John Jablonski

                                                                                        It would make more sense perhaps if the VARs could be contracted to do design work, so they would run into these problems and do their own "Rx" sessions instead of having paying customers do it.

                                                                                         

                                                                                        That is the most awesomest idea I have ever heard. THAT would be way more likely to get bugs fixed. And it is, unfortunately, where the disconnect between SW development/marketing and actual users seems to be. Come to think of it, that would likely keep a lot of new "features" out as well (to wit: the dimension palette).

                                                                                         

                                                                                        Along a similar vein , it's why I hate canned demos. If you want me to buy your software, you take some of -my- models (after NDA if necessary) and do what I ask you to do to them. And you do at least some of that sight unseen. THAT is how I can get an impression of how good the software actually is.

                                                                                         

                                                                                        And Emilio, I have never, since SW98+ or so, had luck with angle mates. They have ALWAYS been the weakest, most inconsistent mates in SW. You're way better off creating a reference plane at an angle in your part/subassembly and making planes coincident.

                                                                                         

                                                                                        -john

                                                                                        • Re: Solidworks 2010 is a piece of !#$%@.
                                                                                          Mauricio Martinez-Saez


                                                                                          Emilio, I fully agree with you on your comments about the SW User-VAR-SW model... the main problem with that model is the "filter" which sometimes (and I say "sometimes" to make it look nice) don not have the knowledge required to understant what is the problem in a real life "design work" envirenment.

                                                                                           

                                                                                          Back in 1993, one of the companies reporting to me was a PTC VAR (which we adquire just to support our very large Pro-E new CAD installation), that company was very succesfull since as the new CAD system increase productivity of our engineering departments, we transfer engineers to work with them providing contract design work for customers, as well as doing "demos" with models created with actual products design by customers.  I believe that now that company (which we sold in 2001), do not sell any software, since their large business is contract design and tecnical sopport to CAD users (including SW).

                                                                                           

                                                                                          Getting back to your problems, in all our models we avoid as much as possible the utilization of:

                                                                                           

                                                                                          1.- 3D Sketches (you can do the same using 2D sketches and planes, so use 3D sketches only when a combination of 2D sketches will not be able to do the job)

                                                                                           

                                                                                          2.- Mate parts to parts using part features, faces, holes, etc., since we mdel Top-Down we use very few mates, we mate part planes and origing to planes and points on the assembly or sub-assembly containing the part, and we never have any problem with mates.  Since models allways have some components added "bottom-up" (purchased parts) we mate those using planes and origin and mate them to planes and points, that provide a very solid mate.  Mates to features and surfaces of parts, give us problems from time to time, so we avoid them.

                                                                                           

                                                                                          Perhaps we are usign the software utilizing only "basic" functionality, but we create very large anmd complex 100% parametric models that work perfect and give us no problem.  Maybe what happen is that that we have suffer all the bugs, found workarrouds and learn how to live with them,  sometimes we spend a litle more time modeling someting usign "basic" functionality (such as 2D sketches vs. 3D sketches), but at the end we do the job sooner that is we spend our time trying to explain the VAR and SW where the application have a "limitation", and leave SW to found the problem and resolved on some "future" version, when some VAR in some place finally do his job and induce SW to fix the problem.  I know this is not the correct way... but during the pass 30 years I have suffer any CAD software (almost every one that existed) and we know that no one is perfect.

                                                                                           

                                                                                          And as you may know.... mas vale malo conocido que bueno por conocer... 

                                                                                            • Re: Solidworks 2010 is a piece of !#$%@.
                                                                                              Emilio Graff
                                                                                              By the way, 3D sketches are very handy for laying out optical elements in complicated optical instruments. Unfortunately, as you said, they are very prone to problems. Right now I'm converting one of these to a set of 2D sketches and planes and I can already see how much longer it takes... and how much harder it is to keep track of circular references.
                                                                                                • Re: Solidworks 2010 is a piece of !#$%@.
                                                                                                  Mauricio Martinez-Saez

                                                                                                  34717 wrote:

                                                                                                   

                                                                                                  By the way, 3D sketches are very handy for laying out optical elements in complicated optical instruments. Unfortunately, as you said, they are very prone to problems. Right now I'm converting one of these to a set of 2D sketches and planes and I can already see how much longer it takes... and how much harder it is to keep track of circular references.

                                                                                                   

                                                                                                  Yes, setting up a set of 2D sketches and planes to create complex 3D parametric geometry will take some more time (not to much once you understand how to do it and conceptualice the entire thing before you start to draw the frist line), but the extra time you will expend creating the geometry will be less that the amount of time you will spend "fixing" problems if you use the 3D sketches.

                                                                                                   

                                                                                                  In reality, a 3D sketch is just an "internal" construction (transparent to the user) of a set of 2D sketches, the disadvantage is that in a 3D sketch you let the application "decide" how to build the construction of the 2D - 3D structure and sometimes this do not produce a "solid" result.

                                                                                              • Re: Solidworks 2010 is a piece of !#$%@.
                                                                                                Mauricio Martinez-Saez

                                                                                                Emilio,

                                                                                                 

                                                                                                I am going to describe our VAR experience...

                                                                                                 

                                                                                                1.- We receive only one call a year from our VAR, the call is placed by an administrative person and the reason for the call is to remind us that our service subscription expire in 30 days and that they are sending the invoice to renew.  Then if we do not send the payment in 15 days we receive a second call and a couple of emails.

                                                                                                 

                                                                                                2.- Once we provide a very large model to "show" a critical problem  (the VAR indicate to us that SW require the model to analyze the problem),  I compress the complete directory into a 245Mb WinRAR which was protected with a password (which will be required to decompress the WinRAR) and upload the WinRAR file to an FTP they indicate to me (... without providing to them the password),  they acknowledged receipt of the compressed file and they indicate that SW was working on the problem... this was in 2006 and up to this date NO ONE CALL US REQUESTING THE PASSWORD TO DECOMPRESS THE WINRAR FILE.  The issue was resolved on the 2008 version...  Maybe the used a password "removal tool" ??? :-) but I doubt this... the password was 47 characters long... and the WinRAR was two levels deep each one with a different password.

                                                                                                 

                                                                                                Draw your own conclusions...

                                                                                                 

                                                                                                By the way we pay subscription service since we want to have the software up-to-date with the last versions, etc, so internally we call it "update subscription cost" no "service cost".

                                                                                                  • Re: Solidworks 2010 is a piece of !#$%@.
                                                                                                    Phil Marra
                                                                                                    Similar thing happened to me, some years ago. I sent a problem to the resellar I had at that time never heard a word about the file or the problem, I had actually assumed my e-mail didnt make it. In the mean time I figured out a work around and forgot about it. 11 months later I get a receipt from Outlook saying the mail was read that day. Pretty sad. But to make matters worse there was no response from the receiptiant.
                                                                                          • Re: Solidworks 2010 is a piece of !#$%@.
                                                                                            John Burrill

                                                                                            One of the down-sides of working in the defense industry is that everything is on a need to know basis.  In our case, we have to go pretty far up the ladder to get an approval to share design data outside of the organization and then they want us to use encrypted zip files or a secure transfer service.  It really does bog down support.

                                                                                            The definition of delicate may involve explaining to network security and legal departments why you need outside help trouble-shooting a software problem without throwing your own IT department under the bus and subsequently alienating them.

                                                                                              • Re: Solidworks 2010 is a piece of !#$%@.
                                                                                                Ryan Laplante

                                                                                                We bought our SW 2010 from Shounco Design in Salem, Northern Oregon, when I email them a question they call me back and walk me through an answer on the computer.  They work with us to get what we need done in SW.

                                                                                                 

                                                                                                Also your Var can do all kinds of things like get you credits for the CSWP and CSWA, help you out with classes and training ect...

                                                                                                 

                                                                                                Sounds like some VAR's just call to remind you that they need to collect their subscription commission again this year, cancell with them and find someone who gives a rats ass, even the mention of looking for another reseller should get them to sweeten the deal up on the next subscription, sorry that so many of you are paying for nothing more than an expensive upgrade package.

                                                                                            • Re: Solidworks 2010 is a piece of !#$%@.
                                                                                              Emilio Graff

                                                                                              Here's another one. No matter how often you rebuild, CTRL+B, CTRL+Q, whatever, not all errors will pop up. I just opened a subassembly I haven't touched in a while and changed a sketch. Bam. References that are not even related to the sketch are now broken, due to changes in the main assembly that I did 3 months ago. Why? Because since 2009 the rebuilds have been sporadic at best. Perhaps they tried to make the loop more effective, but I have consistently had problems in which the rebuilds do not catch all the problems until you somehow trigger them later.

                                                                                               

                                                                                              And the worst part is when you trigger one after you've unkowingly destroyed tens of things. Now you have to put it back together from this mess.

                                                                                              • Re: Solidworks 2010 is a piece of !#$%@.
                                                                                                Joel Kolodziej

                                                                                                One thing I've discovered in my brief time in modeling, is that referencing features on 1 part to features on another part produces NOTHING but headaches later on.  I've found that it is fine to design that way, but once you're design is done, it is definitely in your best interest to go back and remove all external references.

                                                                                                 

                                                                                                It might take a little longer at design time, but it'll save you a ton if revisions or modifications need to be made that may break your assemblies.