12 Replies Latest reply on Jan 15, 2014 8:48 PM by Miklos Hejjas

    Complex Sketching Techniques

    Allen Fisher

      Does anyone have recommendations on how to sketch complex shapes quickly and effeciently?  For instance, I have a lot of geometries in the shape of a residential key.  One complex key shape would be the Schlage key.  You probably have one in your pocket.  On this key there are many fillets, blends to fillets, and other features that make it difficult to sketch.  Any feedback would be appreciated.

        • Re: Complex Sketching Techniques
          Jim Mooney

          Sometimes for really complex shapes I use my 2D drafting package to draw it, it has many more commands for drawing complex shapes.  I then import it into SW sketch as a .dwg.

          • Re: Complex Sketching Techniques
            Lenny Bucholz

            In SW or any Solid software make smaller groups of features, like the top of the key, sketch half, then mirror then extrude.

            make all the corners sharp in the sketch then apply fillets last.

             

            for the grooves to slide in the lock use solid sweep cuts, make them look just like the cutters that would cut them in real life and you'll get the result you want.

             

            to may try to draw the complete detail, small step are easier to fix.

             

            also you can use a pic to trace the shape... go to help and look up picture in a sketch.

             

            Message was edited by: Lenny Bucholz

             

            Message was edited by: Lenny Bucholz

            • Re: Complex Sketching Techniques
              Allen Fisher

              Specifically, I am looking at the outside profile only that includes all the fillets and blends. When sketching each line (even without the fillets) the sketch can blow up when adding dimensions and relations.  What would be the best approach to sketching complex shapes like this?

                • Re: Complex Sketching Techniques
                  Lenny Bucholz

                  As I said, draw the sharps first get the sketch full defined this way, extrude then apply the fillets as a feature.

                   

                  the more complicated the sketch the more problems you'll have when trying to change, been doing this for a long long time, instruct at the University and to machinist and engineers at night at the Community College.

                   

                  easist way to explain in solid modeling is in the real world does one operation make a part or does many smaller operation make a part???

                   

                  You're just making it alot harder than it has to be. Have you used the fully defined sketch tool?? sketch then got to the pulldowns, tools\dimensions\ fully defined sketch, pick how you want the dims to show and click the green arrow...badabing done.

                   

                  just  giving you some Tips and Tricks that have been used by more than just me, SW dealers teach sketching the same way when you take their course.

                    • Re: Complex Sketching Techniques
                      Allen Fisher

                      I currently model the way you are describing. My question is more specific to the sketch itself. When I am creating each line I am approximating the location and lengths relative to each other. After I get it close I will constrain all the geometry with relations and dimensions. In this process sometimes it will flip some geometry over, spin it around, or do something else unexpectedly.

                      So maybe I should rephrase my question. Is it better to apply all relations before or after dimensioning? Or at the same time.  Are there any other techniques that would help?  Is it just experience?

                        • Re: Complex Sketching Techniques
                          John Sutherland

                          If you are receiving unpleasant surprises then your technique is clearly sub optimal.

                           

                          I design a simple geometric skeleton/framework in construction lines, then clothe it with the details.

                           

                          If a polygon will perform the skeleton function then I work out how many sides it will have and apply the polygon tool to the Graphic Area clear of any other geometry.  Then display and delete all relations in the polygon.  Then drag the points of the polygon into the approximate shape of the skeleton.  Then apply relations between the sides to firm the shape.  Then apply relations to other geometry to locate the skeleton in space.  Then apply dimensions to polygon elements one at a time until the skeleton is fully defined.  Then save the document to lock in your gains.

                           

                          When you apply fillets, SW may delete some of your skeleton but you can recover it by creating Virtual Sharps.

                           

                          Avoid the relations Horizontal and Vertical because they will prevent you from tilting/rotating your skeleton down the track.  Sometimes this matters.

                          • Re: Complex Sketching Techniques
                            Patrick O'Hern

                            I find sketches are much easier to work with if you define them as you go, rather that trying to sketch everything, then add dimensions later.   It tends to keep things located where you want them to be, and cuts down on the "flipping" that you are seeing.

                             

                            Another thing you can try, is to temporarily add a "Fixed" relation to sketch entities that you do not want to move. This keeps them in position when dragging other portions of the sketch.  Once you are done, just delete the relation.

                      • Re: Complex Sketching Techniques
                        Daen Hendrickson

                        Allen,

                         

                        I second Lenny's suggestions; break the complex into simpler but multiple steps.

                         

                        Use sketch relations in lieu of dimensions where possible.

                         

                        ****** edited by Daen *****

                         

                        Seems the second half of my message got chopped off????

                         

                        When dimensioning, size the largest features first. This sort of sets the outer bounds and lets the smaller details float inside of those bounds.

                         

                        If you get a combination of relations and dimensions that cause a sketch element to flip and you can't drag it back, you can use the "Display/Delete Relations" tool to temporarily suppress a relation or dimension instead of deleting and recreating it. You can then drag the element to its near proper position and then unsuppress the relation.

                         

                        Daen

                        • Re: Complex Sketching Techniques
                          Matt Lombard

                          Personally, I don't believe in the concept of "complex sketching". If a sketch is going to get complex, I divide it up into multiple features. You might consider using blocks for static shapes. Complex sketches plus sketch fillets = disaster if you ever make a change. I tend to use fillet features rather than sketch fillets, because if a sketch fillet fails, it takes the entire extrude with it. If a feature fails, the troubleshooting is more compartmentalized.

                           

                          For some situations, you might also consider removing shapes rather than adding shapes. Or you could consider using "regions" instead of just closed loops, with a grid of overlapping lines, and just select the boxes you want to use. Although regions can get messy if you make certain changes.

                            • Re: Complex Sketching Techniques
                              Miklos Hejjas

                              I have questions regarding this topic:

                               

                              1. Where is the limit? 10, 50 or 100 sketch entities?

                              2. Is it a technical issue or it's just the human limit of the user?

                               

                              I assume this one is over the limit:

                               

                              Type Name                             Count Converted

                              100  Arc                                   531       531

                              110  Line                                  879       879

                              116  Point                                   15        15

                              124  Transformation matrix             9         9

                              314  Color definition                       1         1

                              402  Associativity instance              9         9

                              _________________________________________________________________

                               

                              Curve/Sketch feature(s)                1425

                              --------------------------------------------

                               

                              But I have another one, which is much smaller, but it's pretty large also:

                               

                              Type Name                             Count Converted

                              100  Arc                                      91        91

                              110  Line                                   101       101

                              124  Transformation matrix             2         2

                              314  Color definition                       1         1

                              402  Associativity instance              2         2

                              _________________________________________________________________

                               

                              Curve/Sketch feature(s)                192

                              --------------------------------------------

                               

                               

                              The sketches came from the same type of problem: Both time I had an existing pretty complex yet sheet-shaped part without any documentation which I had to remodel. The simpliest way I found to deal with it was to scan the parts in the best possible quality than use "sketch picture" to create the sketch from it.

                              This way I had to find out the relations to set up the proper geometry, and this worked me best when sketching all contours in the same sketch. A bit of a relief is that in such cases there is a smaller chance that later I have to modify the sketch from roots.

                               

                              At the beginning I could rarely work for even 5 minutes without getting the whole sketch red and yellow, but I've learned a lot from it.

                              After a while I've understood that the system interprets definitions a bit differently than me, but it's still consistent most of the time (in a weird way), and now it's quite rare for me to get a yellow screen, and when it occurs, normally I can solve the problem fast.

                               

                              Best regards