59 Replies Latest reply on Nov 23, 2015 11:00 AM by Deepak Gupta

    New(ish) to Solidworks coming from ProE

    Frank Schiavone

      My company has handed me Solidworks 2014 to learn as we've aquired several smaller companies that use it, so I'll be tasked to learn and use it in addition to Pro/E so I'm here to seek opinions and help learning it.  I'm planning on being an expert-level on SW in time as well.  Looks good on the resume, right? 

       

       

      Background:

      I'm a guru-level Pro/E user (not bragging, it is what it is), having started on it in '96 (V 15), and had been the same level user on AutoCAD starting in '86 (V 2.18).  I played around with CV (hated it) before AutoCAD, and also in the late '80's spent time learning Wavefront professional animation software.  I also spent 6 months on Solidworks in the 2004 timeframe and became pretty good at it at the time.  We're currently still stuck on an old version of Pro/E (creo elements/pro 5.0) that has THE worst interface by far of all the Pro/E versions I've ever used, so it's not an apples-to-apples comparison, but we have creo 3 that I will be loading and learning soon.  For reference, I do a lot of top-down design of IM plastic parts/assemblies, die-castings, and other heavily surfaced parts with draft, rounds, etc..

       

       

      Reason for learning SW:

      As I mentioned, we buy smaller companies that have designs in it, but also management is going to want high-level user input on what software to use for our NEW designs going forward.  I want to be able to give them an apples-to-apples comparison of features and capabilities.....and limitations.

       

      As I remember, when I used SW in '04, I didn't like it at all, and found it's capabilities vs. Wildfire frustrating.  I spent the morning yesterday playing with 2014, and have to say I liked it better.  Some things I like better than my current (old) version of Pro/E, some things I don't.  Being forced to create stand-alone sketches seems to be gone, though with my limited time on it, don't know if all the top-down design and surfacing limitations that drove me nuts are still there.  Still stumbling around learning, but am happy that in just a couple hours with no tutorials, I made a part with several features, and found things like the ability to have multiple radiii in a round feature, although I have to say that's one area Pro/E seems to have far more capability, by being able to drag the size in the creation, and, more importantly, have the ability to create multiple "sets" within the same feature, with each set being able to have a different radius and even being able to have a different type of round (circular vs. varieties of conic, etc.), and also having a lot more capabilities in specifying transitions, and end conditions.

       

      So, my questions then to the SW experts are:

      1.  Are there graph features that can be used to control curves from equations based on a CS?

       

      2.  If so, can these graph features be used in other features to drive the section, as in a swept section?

       

      3.  In Pro/E, there is a feature called a spinal bend where you can bend geometry (surface or solid) based on a 2D curve, is there a similar feature, if so, what is it?

       

      4.  There is a toroidial bend like the above, say, for making tires, where you can bend geometry in 2 different directions, is there a similar feature, if so, what is it?

       

      5.  There is a feature called a Variable Section Sweep (VSS, that I believe is absorbed into the sweep feature now) where you can specify a spine trajectory, and use other trajectories to push and pull on a section.  Also you can specify that the section always remain normal to the spine, or always remain parallel to a plane regardless of what the spine or other curves do (to a pint of course).  In additon, you can write equations in the sketch (to produce sine waves, etc.).  Is there a similar feature, if so, what is it?

       

      6.  There is an "evaluate" feature in Pro/E, where you can use a straight line curve (of, say a hydraulic line detailed in a dwg) to drive the length of a curved line (hydraulic line at assembly), or use it to drive the curve controlling a spinal bend.  Is there a similar feature, if so, what is it?

       

      7.  Coming from a Pro/E background, what could I do to help myself learn SW faster/better?  Any tips, techniques, sources of training/info?

       

       

      Those are all the direct questions I can think of now, please feel free to chime in with whatever (tips, tricks, favorite guacamole recipe!)

       

       

      Grazie!

       

       

      Frank

        • Re: New(ish) to Solidworks coming from ProE
          Roland Schwarz

          Man, I miss variable section sweeps! SW does a better job than they used to. Look into guide curves. Section sketches used for sweeps need additional pierce constraints to attach to guide curves.

           

          Nothing like trajpar. STILL!

           

          Coordinate systems? Feh! Tick Talk on EsoxRepublic.com » SW Coordinate Systems Are Nearly Useless

           

          No graph feature, but at least they now have t-parametric equation-driven curves.

           

          There are some things SW is great for. Often, these are things that drive hard-line Pro/E users crazy. SW is fast and loose with not requiring things to be fully constrained. Maybe not so cool for people working in dark little boxes, but way cool for doing broad-stroke conceptual work. I can throw a gear train around in SW to minimize space just by dragging. Couldn't do that in Pro/E (maybe they've changed?).

            • Re: New(ish) to Solidworks coming from ProE
              Frank Schiavone

              'Morning Roland!

               

              Yeah, trajpar is one of my fave tools, along with graphs.  Using the 2 together and you can do some amazing stuff.

               

              Not having it in SW does pose issues for me.

               

              Yeah, just from my tinkering with it, it seemed that way.  You can just fudge everything, no dimensions needed!  I was also able to drag a hole from the top surface of a cube to any of the sides.  Kinda neat from a "whiz-bang hey look at this!" perspective, but kinda scary in real life.  What if you did this at an assembly level without realizing it?  Honestly, I can see a legit need to drag a hole from the top to the side.  Usually, even conceptually, you have SOME idea of your direction.

            • Re: New(ish) to Solidworks coming from ProE
              Alin Vargatu

              Frank Schiavone wrote:

               

               

              1.  Are there graph features that can be used to control curves from equations based on a CS?

               

              2.  If so, can these graph features be used in other features to drive the section, as in a swept section?

               

              3.  In Pro/E, there is a feature called a spinal bend where you can bend geometry (surface or solid) based on a 2D curve, is there a similar feature, if so, what is it?

               

              4.  There is a toroidial bend like the above, say, for making tires, where you can bend geometry in 2 different directions, is there a similar feature, if so, what is it?

               

              5.  There is a feature called a Variable Section Sweep (VSS, that I believe is absorbed into the sweep feature now) where you can specify a spine trajectory, and use other trajectories to push and pull on a section.  Also you can specify that the section always remain normal to the spine, or always remain parallel to a plane regardless of what the spine or other curves do (to a pint of course).  In additon, you can write equations in the sketch (to produce sine waves, etc.).  Is there a similar feature, if so, what is it?

               

              6.  There is an "evaluate" feature in Pro/E, where you can use a straight line curve (of, say a hydraulic line detailed in a dwg) to drive the length of a curved line (hydraulic line at assembly), or use it to drive the curve controlling a spinal bend.  Is there a similar feature, if so, what is it?

               

              7.  Coming from a Pro/E background, what could I do to help myself learn SW faster/better?  Any tips, techniques, sources of training/info?

               

               

               

               

               

              1. Not sure what a graphs feature is, but SW has equation driven curves. 2016 SOLIDWORKS Help - Equation Driven Curves

              2. Curves can be used for sweeps, lofts, boundaries and fills.

              3. We have the Deform feature that allows the deformation of an edge (and the attached faces) based on a curve. 2016 SOLIDWORKS Help - Deform - Curve to Curve Options

              4. Not sure. Look up Flex. 2016 SOLIDWORKS Help - Flexes

              5. Sweep with guide curves? 2016 SOLIDWORKS Help - Recommendations for Sweeps with Guide Curves

              6. Of course we have that in SW.

              7. Fastest way to get up to speed in 2-3 days while learning best practices, productivity techniques, troubleshooting techniques in order to master SW super fast is to take an Advanced Update course delivered by a top SOLIDWORKS expert. The best VARs offer this course both in-class and online.

                • Re: New(ish) to Solidworks coming from ProE
                  Frank Schiavone

                  Thanks for the tips Alin!

                    • Re: New(ish) to Solidworks coming from ProE
                      Alin Vargatu

                      This is to illustrate item #6:

                       

                        • Re: New(ish) to Solidworks coming from ProE
                          Frank Schiavone

                          Thanks for the link Alin!  Actually what I meant was, in Pro/E, we have a separate stand-alone feature we can create, to use to drive other features.  This is very handy, something that in the end of the video he was not able to do.  We also have something similar to what was shown in the video, where at the sketch level we can change a spline, or series of elements (as long as they are connected), select them all, then convert them to a "perimeter" dimension.  Then, if you have a line you want to use as a driving dimension, you write a relation (for SW, I guess it's called an equation) in the sketch to drive the perimeter dim by the line dim.  The advantage in Pro/E is that splines don't cause problems.  The limitation is that you can only have one perimeter dim per sketch.  But, you get around this by using an evaluate feature, to drive as many different features as you wish.

                           

                          Nice to know SW has this capability in some respects, thanks!  It all helps my learning process!

                      • Re: New(ish) to Solidworks coming from ProE
                        Frank Schiavone

                        Alin,

                         

                        Wow, the equation driven curves are a LOT more difficult in SW.  In Pro/E we can choose any coordinate system, and specify a cartesian, cylindrical, or even spherical type curve.

                         

                        For example, making a simple planar 180deg arc (4" radius) in a cylindrical curve type it is:

                               r = 4
                           theta = t * 180
                               z = 0

                         

                         

                        For a helix of 4 turns with a radius of 4" and a height of 4", it is:

                               r = 4
                           theta = t * 4 * 360
                               z = t * 4

                         

                        Then, for any of those variables, I can add some of my own tricks, or put an equation in any one or all of them.

                      • Re: New(ish) to Solidworks coming from ProE
                        Frank Schiavone

                        Oh, and we're on 2014 as I mentioned before.  So, sadly, the new stuff is no help to me.

                        • Re: New(ish) to Solidworks coming from ProE
                          Frank Schiavone

                          Sooo, my new boss, the one who wants us to convert to SW so badly, had MCAD come in for a demo today.  Prior to this, I sent them some surfacing files and other models to try and reproduce.  The guy who came in, showed a new model containing my model (brought in as a STEP) and one next to it he did in SW and it looked good at first.....until I looked at the geometry.  He was not able to reproduce the models I sent, but rather kind of cheated.  Yes, he didn't have a ton of time to work on the models, but he had all of Friday, and the weekend, and this morning, and was not able to reproduce any of them.  There is no graph feature, and the curve by equation wasn't as powerful.  No trajpar, so instead of doing things easily within the VSS, you're forced to make several curves, and they're not as easy as doing it in Pro/E.  No spinal bend either.

                           

                          I figured he wouldn't be able to make most of them, but I was more disappointed that instead of simply saying he couldn't quite do it, he showed us a zoomed-out view of "sorta" the geometry that I wanted, then claimed he had made the geometry and then wanted to switch to something else.....until I stopped him and showed that he had not actually made the geometry.  I'm sure vendors like that HATE me, but I wouldn't be doing my job if I didn't make them do the hard stuff.

                           

                          From what I see, SW has closed the gap.....but is not there yet.  Maybe for many, or even most, people, these tools never get used by them and they don't care.  I DO use them as part of my job (Industrial Design), and I DO care.  I'd have to say I plan on becoming an expert in SW also, but for new designs, I'd still recommend Pro/E for it's power.

                           

                          Think of this analogy:  How often do you need to use the emergency Room at the hospital.....but aren't you glad it's always there? 

                           

                          But hey, they brought lunch for us! 

                            • Re: New(ish) to Solidworks coming from ProE
                              John Wayman

                              Frank,

                              It's the little things I miss the most:

                              Middle Mouse button to accept,

                              Create a datum plane on the fly,

                              Roll back an assembly by dragging the bar in the model tree,

                              Being able to see what constraints apply to what at a glance, rather than having a whole heap of derived constraints mixed in with the defining ones,

                              I even miss not being forced to fully define everything! (I still try to, by the way...)

                               

                              6 months in, I'm still rubbish at it!

                               

                               

                              Cheers,

                               

                               

                              John

                                • Re: New(ish) to Solidworks coming from ProE
                                  Frank Schiavone

                                  'Morning John!

                                   

                                  I was looking for "datum on the fly" as well, and wasn't seeing it.  Drat!

                                   

                                  Thanks for your heads up on these items, going to have to look for a workaround.......

                                    • Re: New(ish) to Solidworks coming from ProE
                                      Alin Vargatu

                                      Frank Schiavone wrote:

                                       

                                       

                                       

                                      I was looking for "datum on the fly" as well, and wasn't seeing it.  Drat!

                                       

                                       

                                      Frank, maybe I rushed with my reply, not fully understanding what you meant. What is "datum on the fly"?

                                        • Re: New(ish) to Solidworks coming from ProE
                                          Frank Schiavone

                                          It's where, if you do not want a permanent plane (or point,or axis) sitting in your model tree, you can create a feature without a predefined sketching plane, then when it asks for one, you create it on the fly, use it, perhaps even create another to, say, extrude up to (offset from something else), then end the command.  Any datum features you create are buried in the feature itself, not cluttering up your model tree.  There are also other uses, say, for points, where you can reference them internal to the feature created.  You can also create multiple datums if needed to get what you want.

                                      • Re: New(ish) to Solidworks coming from ProE
                                        Alin Vargatu

                                        John Wayman wrote:

                                         

                                        Frank,

                                        It's the little things I miss the most:

                                        1. Middle Mouse button to accept,

                                        2. Create a datum plane on the fly,

                                        3. Roll back an assembly by dragging the bar in the model tree,

                                        4. Being able to see what constraints apply to what at a glance, rather than having a whole heap of derived constraints mixed in with the defining ones,

                                        5. I even miss not being forced to fully define everything! (I still try to, by the way...)

                                         

                                        6 months in, I'm still rubbish at it!

                                         

                                         

                                        Cheers,

                                         

                                         

                                        John

                                         

                                        1. RMB in SW

                                        2. Doable in SW 2016

                                        3, Works in SW for assembly level features

                                        4. Same in SW.

                                        5. You are not forced to fully define anything in SW.

                                          • Re: New(ish) to Solidworks coming from ProE
                                            Jim Proctor

                                            How is #4 the same as SW?

                                            • Re: New(ish) to Solidworks coming from ProE
                                              John Wayman

                                              Alin,

                                              Thank you for the response.

                                              The RMB for accept is a step in the same direction as MMB for accept in Pro/E, but (apart from a few inconsistencies) it is much more generally available in Pro/E, as it is the equivalent of clicking 'OK' in the menu structure that lurks beneath the shiny user interface.

                                              Datum plane on the fly is a significant benefit (one of the first I have identified) of 2016. I look forward to it. Still on 2014 here because the server is running an older version of Windows server OS, and 2015/2016 will not run on it, apparently.

                                              Rolling back assembly-level features would be great, if I were in the habit of making them. In Pro/E, the process of building an assembly is very sequential, so you can readily drag the insertion point up the tree and every component below it is suppressed. I can do almost the same by selecting, right-clicking and suppressing, but I find it doesn't always work as I expect. The placement of component patterns at the bottom of the tree appears to make things more difficult, in my mind.

                                              I am not used to seeing the constraints that a second part uses to attach itself to the first part mixed in with the constraints that fix the first part. That does not happen with Pro/E. The symbol indicating that a constraint is a defining one is helpful. That the defining constraints are not always listed as the first 3 (or 4) in the list of constraints, but seem to move about in the list is not so helpful.

                                              My users tell me they "Fully define what needs to be fully defined, and not what doesn't". My response is 'How do you know?'. I cannot tell, at a glance, whether a part or feature is sufficiently defined or poised to bite me in the backside whenever I make a minor change.

                                               

                                              I'll get used to it, I know. There are certainly aspects in which SW is better than Pro/E, as well as vice versa. I was just letting Frank know he was not alone!

                                               

                                              Cheers,

                                               

                                               

                                              John

                                                • Re: New(ish) to Solidworks coming from ProE
                                                  Frank Schiavone

                                                  Interesting stuff John, thanks!  It's helpful, trying to learn it.

                                                   

                                                  Does SW have the "Restructure" functionality Pro/E does, where I can change the level at which a component is assembled to another level?

                                                  • Re: New(ish) to Solidworks coming from ProE
                                                    Jackie Yip

                                                    New for 2016: Confirmation Corner

                                                     

                                                    2016 What's New in SOLIDWORKS - Moving the Confirmation Corner Options to the Pointer

                                                     

                                                    Press D and i will bring up a window so you can click accept anywhere.

                                                      • Re: New(ish) to Solidworks coming from ProE
                                                        Frank Schiavone

                                                        "Confirmation Corner"......is that for Catholics only? 

                                                         

                                                        I was using the check and X features there, although it would be easier to use a middle click or mouse click.

                                                          • Re: New(ish) to Solidworks coming from ProE
                                                            Jim Wilkinson

                                                            Hi Frank,


                                                            Have you discovered Mouse Gestures yet? I put both OK and Cancel in the mouse gestures so they are always there with a swipe of the mouse. For me, I turn on 8 gestures and then use the upper right corner for OK and the lower left for cancel.

                                                            2015 SOLIDWORKS Help - Using Mouse Gestures

                                                             

                                                            Thanks,

                                                            Jim

                                                              • Re: New(ish) to Solidworks coming from ProE
                                                                John Wayman

                                                                Jim,

                                                                Mouse gestures are good, but you have to click in free space to get them up (I think). When I am in the middle of an assembly, trying to sort out mad mates, there is frequently no free space to click on. In that case, it's back to mousing all over the world to find the green tick.

                                                                 

                                                                The 'D' in 2016 looks promising, as long as I program a SpaceMouse button to be a 'D'.

                                                                 

                                                                 

                                                                John

                                                                  • Re: New(ish) to Solidworks coming from ProE
                                                                    John Stoltzfus

                                                                    A quick right click and swipe is all you need, quick and right there, just wish there would be 16 feature choices instead of 8

                                                                    • Re: New(ish) to Solidworks coming from ProE
                                                                      Jim Wilkinson

                                                                      Hi John,

                                                                       

                                                                      RMB drag is used for rotate component in assemblies and we didn't want to regress that long standing behavior. Therefore, when on a component in assemblies, if you hold the Alt key while dragging the right mouse button, you can access the mouse gestures. That is documented in the help topic I referenced in my last post (it is in a shaded section with a light bulb which is our standard designation in the help for a useful note).

                                                                       

                                                                      I hope this helps,

                                                                      Jim

                                                                        • Re: New(ish) to Solidworks coming from ProE
                                                                          John Stoltzfus

                                                                          Is there any discussion within your group to expand the mouse gestures, would be awesome if you could.  I use Alpha Cam for our CNC programming and they have 2 different wheels and also within the wheel, they also expand further...

                                                                            • Re: New(ish) to Solidworks coming from ProE
                                                                              Glenn Schroeder

                                                                              John Stoltzfus wrote:

                                                                               

                                                                              Is there any discussion within your group to expand the mouse gestures, would be awesome if you could.  I use Alpha Cam for our CNC programming and they have 2 different wheels and also within the wheel, they also expand further...

                                                                              John,

                                                                               

                                                                              Did you see this Idea: Increase mouse gestures abilities (radial menus of radial menus) ?

                                                                              • Re: New(ish) to Solidworks coming from ProE
                                                                                Jim Wilkinson

                                                                                Hi John,

                                                                                 

                                                                                I believe you are talking about the radial menu in Alphacam. The interaction with that is quite different than mouse gestures. Mouse gestures are intended to be a very quick stroke of the mouse to execute a command without even needing to interact with any user interface. The UI that we do show is purely for learning purposes and once you memorize the mouse gestures, you generally will never see it again (since we have the timing on it such that it doesn't even appear if you move your mouse fast enough). We don't want to "spoil" the quickness of using mouse gestures or change it to require fine mouse movements and picking. Increasing it to 16 quadrants would likely not work using a gesture approach because despite your best intentions, as your mouse moves in a certain direction, it wanders a bit and you would likely often miss the intended quadrant and get an adjacent one. We think that 8 is about the maximum that can be used effectively (and that is even hard for some, hence the option to use 4 instead).

                                                                                 

                                                                                The radial menu in Alphacam is a replacement for the right mouse button menu (called shortcut menus in Microsoft and SOLIDWORKS). The interaction is generally the same; right click to bring it up, then move over the item you want and click to select it. You may need to click within the menu to expand a submenu to get more options. So, from an interaction standpoint, this is all exactly the same as the SOLIDWORKS right mouse button menus, just the layout is different. It also looks to be more customizable. I can see benefits to each of them. The text and categorization in the SOLIDWORKS shortcut menus is useful since there is more "order" to it so it is easier to find things that you may use infrequently. In SOLIDWORKS, as you probably know, we also have the shortcut bar (S key), which IS fully customizable. We decided to go with a standard toolbar layout for that instead of a radial layout, but we could have decided to go for a radial approach instead.

                                                                                 

                                                                                So, in summary, we have:

                                                                                • Shortcut Menus: fully contextual and dependent upon the selection(s) and therefore there are 1000's of permutations of them in SOLIDWORKS because there are so many different types of objects and modes. Due to that, it is extremely difficult to provide full customizability, hence why we have the ability to hide/show items in the menu portion at the bottom, and only the ability to add items to the context toolbar portion at the top (with some limited "modes" in which those customized items show).
                                                                                • Shortcut Bar: fully customizable, available in 4 modes (parts, assemblies, drawings, and sketch). Used for access to almost any command you like (but most of those are non-contextual type commands).
                                                                                • Mouse gestures: fully customizable, available in 4 modes (parts, assemblies, drawings, and sketch). Used for quick access to almost any command you like (but most of those are non-contextual type commands).

                                                                                 

                                                                                I just wanted to give you a bit of background on the different types of UI's that we have for command access in the graphics area/on the model, what they are intended for, and why they are defined as they are. Can we consider changing these or adding functionality to them? Sure, but we need to be very careful not to do it in a way that spoils the benefits of each of them. Could we add additional types of UI's like a radial menu (with a click-click type behavior)? Sure, but we are already pretty full up on all of the available types of interactions with the mouse and keyboard to bring up such interfaces in an intuitive way.

                                                                                 

                                                                                Of course, we'd be interested to hear user's thoughts on these topics, but probably best to start a new thread on that subject if you want as to not hijack this one.

                                                                                 

                                                                                Thanks,

                                                                                Jim

                                                                    • Re: New(ish) to Solidworks coming from ProE
                                                                      Glenn Schroeder

                                                                      John Wayman wrote:

                                                                       

                                                                      The symbol indicating that a constraint is a defining one is helpful. That the defining constraints are not always listed as the first 3 (or 4) in the list of constraints, but seem to move about in the list is not so helpful.  I'm not in front of SW at the moment so I can't double check, but I'm pretty sure SW will list the mates in the order they're created.

                                                                       

                                                                      My users tell me they "Fully define what needs to be fully defined, and not what doesn't".   Unless it's a flexible sub-assembly I always fully define all components.  In what situations do your users say that's not desirable?  Maybe not locking concentric rotation?

                                                                  • Re: New(ish) to Solidworks coming from ProE
                                                                    Jim Wilkinson

                                                                    Hi John,

                                                                     

                                                                    John Wayman wrote:

                                                                     

                                                                     

                                                                    I even miss not being forced to fully define everything! (I still try to, by the way...)

                                                                    I assume you mean you miss being forced to fully define everything (you said you "miss NOT being forced").

                                                                    SOLIDWORKS has an option for that; see the "Use fully defined sketches" in this help topic:

                                                                    2015 SOLIDWORKS Help - Sketch Options

                                                                     

                                                                    Thanks,

                                                                    Jim

                                                                • Re: New(ish) to Solidworks coming from ProE
                                                                  John Stoltzfus

                                                                  Quick question - How does ProE compare to SW with Custom Properties. 

                                                                   

                                                                  With SW we have Custom Property Tab Builder and Assembly Visualization - type it once stays till deleted...  - I have a lot of custom properties for every part and assembly and I wish they would expand the amount of columns in the Assembly Visualization..

                                                                  • Re: New(ish) to Solidworks coming from ProE
                                                                    Alin Vargatu

                                                                    Are you using the Property Tab?

                                                                    • Re: New(ish) to Solidworks coming from ProE
                                                                      Frank Schiavone

                                                                      I made 2 identical parts.  In Pro/E I have the ability to define different sets (series of line elements, or faces) of rounds within the same feature, and define the type of round I want.  For each set, I can choose from a section that is circular, conic (with 2 editable parameters), a C2 Continuous (with 2 editable parameters), D1 X D2 Conic (with 3 editable parameters), or a D1 X D2 C2 (with 3 editable parameters).  In SW I only have the option of a conic, and I didn't see a way to add the equation { (sd5 = sqrt(2) - 1 } to create the true arc, and just had to truncate that to .414.

                                                                       

                                                                      Also, i can sketch a curve on the surface of a part, and can make the radius change to follow the curve and have my choice of section type above.

                                                                       

                                                                      So, I did a surface analysis of these 2 parts (the reflection analysis tools having a bunch of options whereas the SW "zebra stripes" has none), and the Pro/E part had nice smooth transitions from the planar surfaces, and the SW part had abrupt contour changes everywhere.

                                                                       

                                                                      Not being familiar with the software, am I missing something?

                                                                      • Re: New(ish) to Solidworks coming from ProE
                                                                        Frank Schiavone

                                                                        In Pro/E, I have "mapkeys", 2 or 3 character shortcuts that can do anything from make a line in the sketcher (li), initiate a simple extrude (xt), to open a dwg, make a change, save, and exit, or even more complicated stuff, with a pause for user input if needed.  Is there a comparable functionality in SW?

                                                                        • Re: New(ish) to Solidworks coming from ProE
                                                                          Mark Biasotti

                                                                          Hi Frank,

                                                                           

                                                                          In my current position I'm using both SW and ProE.  My background -  started with ProE14 and went thru to Wildfire1. With SW I've been using it since SW'96. I do a lot of advanced modeling with both ( with IDEO for 16 years.) In my current position I do consumer products.

                                                                           

                                                                          There are pluses and minuses to both systems but I favor SW (and you'll have to just guess why if you know my previous position :-))

                                                                           

                                                                          I wil take a stab at your questions and then offer a few pluses and minuses of my own: (excuse me for others that have already answered these)

                                                                           

                                                                          So, my questions then to the SW experts are:

                                                                          1.  Are there graph features that can be used to control curves from equations based on a CS?

                                                                           

                                                                          MAB - I think this has already been answered but you can create equation curves in the SW sketcher. There is no graph feature in SW like in Proe. Style splines can be dimensioned with equations.

                                                                           

                                                                          2.  If so, can these graph features be used in other features to drive the section, as in a swept section?

                                                                           

                                                                          MAB - No, One of the great features of Proe of course is Trapar - which I used regularly when I was doing consumer products for IDEO.

                                                                           

                                                                          3.  In Pro/E, there is a feature called a spinal bend where you can bend geometry (surface or solid) based on a 2D curve, is there a similar feature, if so, what is it?

                                                                           

                                                                          MAB - The deform feature in SolidWorks can bend and reshape geometry in a number of different ways. Using the curve-to-curve method you can "map" and existing model edge to a created sketch curve and do a number of sets of these to get something similar to what Spinal bend does.

                                                                           

                                                                          4.  There is a toroidial bend like the above, say, for making tires, where you can bend geometry in 2 different directions, is there a similar feature, if so, what is it?

                                                                           

                                                                          MAB - No, Solidworks has no such feature and this is a clear advantage of Proe over SW. SW does have the flex feature which can do what Toroidal bend can do but only an arc and only one direction (but an do a series of Flex features to get bends in two directions.)

                                                                           

                                                                          5.  There is a feature called a Variable Section Sweep (VSS, that I believe is absorbed into the sweep feature now) where you can specify a spine trajectory, and use other trajectories to push and pull on a section.  Also you can specify that the section always remain normal to the spine, or always remain parallel to a plane regardless of what the spine or other curves do (to a pint of course).  In additon, you can write equations in the sketch (to produce sine waves, etc.).  Is there a similar feature, if so, what is it?

                                                                           

                                                                          MAB - As I mention before, no Trajpar for Variable section Sweep, and also no side curve tangency. SW sweep does allow you to control the normal (this is an option called normal to vector)  SW does offer some very powerful things that SW Sweep can do over Proe:  1st, unlimited Trajectories (which in itself is a workaround for Trajpar) 2nd, you sweep a profile down to zero - what this means is that your can sketch your profile as an ellipse, conic or proportional spline and sweep it on multiple trajectories that all meet at the end of the sweep (even tangent to one another.)

                                                                           

                                                                          6.  There is an "evaluate" feature in Pro/E, where you can use a straight line curve (of, say a hydraulic line detailed in a dwg) to drive the length of a curved line (hydraulic line at assembly), or use it to drive the curve controlling a spinal bend.  Is there a similar feature, if so, what is it?

                                                                           

                                                                          MAB - I'm pretty sure that you can do this in SW (may Alin or someone else can chime in or already has) but I think you can do this by assigning a global variable and then having that "hydraulic line" dimension drive a dimension in your part. SW also now has the ability to dimension and equate the length of a spline.

                                                                           

                                                                          7.  Coming from a Pro/E background, what could I do to help myself learn SW faster/better?  Any tips, techniques, sources of training/info?

                                                                           

                                                                          MAB - go to the Solidworks world presentations site (for the past three years) and sit down and watch some of the presentations. If it is advanced modeling, Charles Culp hosts a site call SWTUTS where there are a number of advanced modeling presentations. This forum is great of course for learning - by posting your problem or model in progress and having someone show you.

                                                                           

                                                                          Now some of my own thoughts - ISDX is a great feature in Pro and I wish SW had it. you can do similar in SW, but you have to great (build up) as series of 2D and 3D sketches and then create a boundary surface, but again it is no ISDX.

                                                                           

                                                                          Creo Pros over SW:

                                                                          - Tree rebuilds faster

                                                                          - more robust parametric relationships - and when they are not you have Reroute

                                                                          - Very powerful patterning (because ref. features can be pattern and then used to pattern child features)

                                                                          - not much has changed: an advantage (I'm not kidding, I was away from Proe for 9.5 years and it was easy to pick it back up because not much changed in 9.5 years - just the UI.)

                                                                          - Autodimension in the sketcher (soft Dimensions) and automatically relationships in the sketcher (although occasionally they can bit you in the A**)

                                                                           

                                                                          SW Pros over ProE:

                                                                           

                                                                          - Multibody modeling... need I say more?

                                                                          - 3D sketches. most of all the versatility you get with 2D sketch but can create 3D sketch geometry - and most importantly Splines. In pro, as you know, curves are not sketches, and are limited.

                                                                          - Configurations, yes you have simplified reps - but not as powerful.

                                                                          - Fill feature, SolidWork's Crown Jewel of surfacing features. ProE has the N-sided patch but it was crap 15 years ago and as far as I can see still is.

                                                                          - Style Spline, more powerful than ISDX or Proe Curves combined.

                                                                          - UI is built for quick conceptual work. I don't know quite how to state it but it seems for most features that I create in SW in one step, it takes about 5 to 8 steps to do the same thing in Pro.

                                                                          - visualization of the 3D model and workspace is superior to Proe.

                                                                          - Hole Wizard Toolbox. Pro has something like it but most Pro users I ask about it tell me not to bother with it (because it isn't worth the effort.) How Pro users live with out Hole wizard is astounding!

                                                                           

                                                                          If your concern is the ability to create complex surface models, I would pick SW over ProE any day of the week. This was not always the case, but in the mid to late 2000's SW over took ProE in this department.

                                                                           

                                                                          Mark