21 Replies Latest reply on Aug 10, 2010 8:16 AM by Alan Stoldt

    How do you fully define a sketch?

    Kris Carlson

      Following a suggestion by Joe Kelchner, ("I suggest breaking down each thing to it's absolute minimum and then model it in a two dimensional sketch and get that to work like it should and then use that as a layout sketch"), I am creating a complete 2D sketch of my new project before doing any 3D work.

       

      On the other hand, Jerry Steiger and told me my sketches should be fully defined (https://forum.solidworks.com/message/164513#164513). Attached is a sketch that is underdefined--select for instance the simple inner ellipse in White-SCF-Dura-Ambient (this is the white matter in the spinal cord). Why is it underdefined? How do you diagnose underdefinition? How do you fix it?

       

      Taking a blind stab at defining the sketch further, when I try to fix its center to the origin (which I thought was already done when I created it), it becomes over-defined.

       

      My texts do not really address fully defining a sketch and I had thought it was a good thing to be underdefined because clearly I get error messages when a sketch is overdefined and sometimes have to wade thru many options to fix the overdefinition. Here is what my best text, Planchard's A Command Guide for SolidWorks 2009, says, which seems ambiguous. I know I was naive in thinking an underdefined sketch is good--I just want a set of best practices for fully defining a sketch. Thank you.

       

      "...it is not necessary to fully dimension or define sketches before you use them to create features. You should fully define sketches before you consider the part finished for manufacturing." (p. 4-17).

       

      btw all suggestions I have received on this forum have been very helpful--I really appreciate them.

        • Re: How do you fully define a sketch?
          Alan Stoldt

          Kris,

           

          I think given the nature of your sketch, that anyone would have to spend some time to fully define it.

           

          If you go under TOOLS -> DIMENSIONS, while editing one of your sketches, you will see this option:

           

          FULLY DEFINE SKETCH

           

          fully.JPG

           

          I was able to use it in both sketches to fully define your sketches, but am not sure that for your application it is required or advisable.

            • Re: How do you fully define a sketch?
              Kris Carlson

              This was helpful because I didn't know SW could define a sketch automatically. But it leaves me, as so often in my life, doing something without a clear idea of what it is I'm doing. Accordingly see my challenge to Jerry Steiger next.

              • Re: How do you fully define a sketch?

                Sometimes I use this command to see where it need to be constrained. Then I undo and see if Ican define it formy design intent. this does work. I was going to mention the same thing but just reply instead. Another thing I do sometimesif it is under defined in sketch mode is I try to grab a line or point and try to pull it apart to find out where it is not fully defined. good luck KC

              • Re: How do you fully define a sketch?
                Jerry Steiger

                Alan,

                 

                I don't remember the details of how the original model was made, but I think my remark about fully defining sketches may have made sense for how the elliptical bodies were built. You really needed to have identical sketches for multiple bodies. Working with your new sketch method, fully defining the sketches is not nearly as important. As Alan pointed out, fully defining the spline shapes is probably not necessary and can eat up a lot of time for no great increase in usefulness. It also often makes it difficult to modify later.

                 

                The inner ellipse on Sketch 1 just needed one of the two points to be coincident to the horizontal construction line to become fully defined. Similar coincident relations for a point on the vertical and horizontal construction lines for the two other ellipses and the addition of vertical and horizontal dimensions will fully define them as well.

                 

                I would only add dimensions that you felt were critical on the spline based "wings". To really tie it down you would need to dimension x and y for each point plus angles and strengths for the tangencies. Not much fun and probably not very useful.

                 

                Jerry Steiger

                  • Re: How do you fully define a sketch?
                    Alan Stoldt

                    Jerry,

                     

                    My thoughts were basically that this is more of an artistic endeavor than say a machined component.

                    • Re: How do you fully define a sketch?
                      Kris Carlson

                      Jerry,

                       

                      Your note is very helpful; now I start to see what is involved in fully defining a sketch and as Alan suggested, reinforced by your comments about not needing to define the splines and how tedious that would be, I am starting to get an idea of why and when to fully define or not. Early on and before establishing a hierarchy of driving dimensions, I see one would not fully define. If I were actually sending a CAD file to a manufacturer, I'd probably be remiss to not fully define all key aspects.

                       

                      Alan, this is not an artistic endeavor; the CAD file goes into a finite element program, COMSOL, where the distribution of an electric field on the spinal cord is simulated. Then it goes to a neural circuit program where we try to figure out the effect on pain management in the lower back and legs of different electrode designs and parameters.

                       

                      So Jerry, to save me the time of comparing what SW's Fully Define function does by comparing before and after sketches to figure out what 'fully define' means, can you boil it down--generalize it from the examples you gave? Because I still don't get how to know what will fully define a sketch. Obviously it's imposing necessary and sufficient constraints that the dimensions cannot be changed, stopping short of over-redundancy. But how do you know what will define the sketch, of ellipses and whatever?

                       

                      Thank you!

                       

                      Kris

                        • Re: How do you fully define a sketch?
                          Jerry Steiger

                          Kris,

                           

                          A good part of it is just experience, or training. You understand the basics. Just think about what it takes to completely define an ellipse. You need a major and minor radius, a center point, and an angle. You had the center point and the major and minor radii. Putting one of the "end" points coincident with a vertical or horizontal line gives you the angle.

                           

                          When faced with a sketch that seems like it should be fully constrained but isn't, I often try dragging points to see what moves.

                           

                          I tend to stay away from the automatic constraint generator. I like my constraints better than the ones that SW comes up with.

                           

                          Jerry Steiger

                      • Re: How do you fully define a sketch?
                        John Sutherland

                        "my best text, Planchard's ....."

                         

                        I sent my Planchard books to the paper recycling.

                          • Re: How do you fully define a sketch?
                            Kris Carlson

                            John,

                             

                            I've read some of your comments and respect your knowledge. For me as a raw CAD and SW beginner, the Commands Guide was really very good. One of the things that is really annoying about SW is you can search Help for an exact function name but you may not get an answer or it may not be ranked at the top. That is very inept imho. So a commands guide has been a invaluable complement to Help.

                             

                            But you've piqued my interest and I'm wondering what you might point me toward now that I'm a few months into it. Another book that is more advanced and I think really elegant is Matt Lombard's Surfacing and Complex Shape Modeling. But it's focus is only that.

                             

                            Kris

                              • Re: How do you fully define a sketch?
                                Alan Stoldt

                                Kris,

                                 

                                I meant no offense in the use of artistic, so I do apologize.

                                 

                                Another option is the FIX option. Irregardless of anything else, the line/spline/arc, what have you stays exactly where it is at the time it is fixed. This is a down and dirty option, and can sometimes come back and cause problems futher on. In my opinion, not the best option either.

                                 

                                I would say that if your Spinal model was going to be driven with changing vales from a Design Table, then at that point you probably would need to fully define dimensionally your sketch.

                                 

                                The (4) four spurs radiating outward appear to be equal and opposite.

                                 

                                Fully set Horizontal and Verticle relationships for all ellipses in Sketch 1. Dimension the centerlines to difine the outer ellipse. Dimension the major and minior on the middle ellipse. Extend angle construction line to bounding box and dimension Angle and add coincident relationship to the line it touches. Convert Bounding Box to Contruction lines and dimension.

                                 

                                Remove the Spur from Sketch1 and remove the On edge Relationship for it in Sketch3. Trim the ellipse back to the spline on the upper left spur.

                                 

                                SplineTrim.JPG

                                Delete the other three spurs and fully defined what is left, then use the Mirror command twice to create the Left Top and Bottom, then mirror the Right Top and Bottom.

                                You can now use both sktches as required.

                                 

                                Since Sketch1 has 3 ellipses nested, Ii chose the inner and outer ones for the extrude.

                                 

                                2D_sc_Profile_Work.JPG

                                The extrudes aren't merged, but that can be accomplished easily enough.

                                  • Re: How do you fully define a sketch?
                                    Kris Carlson

                                    I was not offended at all; and sorry I didn't preface with a clearer description of the project. I went thru your very nice model and understand most of what you did. Besides being more precise in your sequence of steps than I have learned to be, you add defining dimensions more often, so I guess between you, Jerry and John I am starting to get what it means to 'fully' or I might say 'adequately' define a sketch. It does import into COMSOL, btw, so the geometry seen by COMSOL is continuous and without flaw. Here is what I don't understand; I'd be grateful for any further quick answers.

                                     

                                     

                                    Fully set Horizontal and Verticle relationships for all ellipses in Sketch 1.

                                    --Aha--good, I see how that will prevent misalignments and small gaps with mates.

                                     

                                    Dimension the centerlines to difine the outer ellipse.

                                    --Centerlines? Or the axes as you say next?

                                     

                                    Delete the other three spurs and fully defined what is left

                                    --How?

                                     

                                    --And finally I thought I've tried extruding right through a 3D object, as I guess you did with the spurs through the cylinder, but ran into problems. You can do this without doing the cuts?

                                     

                                    The extrudes aren't merged, but that can be accomplished easily enough.

                                    --Actually they should not be merged, or what could be, optionally, is what is interpreted as two pieces of the spur--the part outside of the elliptical cylinder and the part overlapping it, which I guess is interpreted as two parts since you didn't do a cut--no big deal to take care of in COMSOL.

                                      • Re: How do you fully define a sketch?
                                        Jerry Steiger

                                        Kris,

                                         

                                        Since Alan hasn't answered yet, I will jump in. I think when he said centerlines he meant the semimajor and semiminor axes.

                                         

                                        How you define the splines is up to you. What are the important features? Are the angles where the spline meets the ellipse critical? How about the width at the ellipse? Is the horizontal or vertical location of the tip important? Whatever matters, come up with a dimension that controls it. Whatever doesn't matter, you can ignore, whether or not the spline is fully defined (black instead of blue).

                                         

                                        Alan probably had the spline extend into the ellipse because that is the safest way to guarantee that SW can join the two together. If the ellipse has different material properties than the wing, then you will want to keep them separate bodies. In that case you could convert edges from the ellipse to form the inside edge of the wing. If your geometry gets less regular (lofts instead of extrudes) you could run into issues where the two pieces overlap or leave voids between them. In that case, you might want to build the wing so it clearly overlaps the roughly elliptical body, then use a surface offset 0 from the elliptical body to cut off the wing so that they exactly match.

                                         

                                        SW is happy to build two bodies to that they overlap. It's up to the user to decide if they should be joined into a single body or left in the strange state of coexisting in the same space, even though classical physics doesn't allow that.

                                         

                                        If you want the spur or wing to penetrate inside the ellipse, but have different properties, then you could use the surface of the ellipse to split the spur into two bodies. You could use the surface of the inner body to cut away part of the elliptical body, so you end up with just one bit of something occupying any one space at a time. You can do the same type of thing with the Combine feature, but you need to make copies of the various pieces as the feature "eats" the tool parts.

                                         

                                        Jerry Steiger

                                          • Re: How do you fully define a sketch?
                                            Kris Carlson

                                            OK, I'm getting the idea of defining the sketches, thanks to everyone's observations.

                                             

                                            "then use a surface offset 0 from the elliptical body to cut off the wing so that they exactly match." No idea what that means! I did just look up 'offset surface' in Help, but not sure how to use it to do a cut.

                                             

                                            Hmm, very enlightening on overlapping bodies. I guess I've been assuming that SW knows if I make two parts match, like the outside dimension of one part and the inside of a part surrounding it, it will let them mate nicely. But your comment is the 2nd time I've heard I may need to overlap them and cut away the overlap. Seems a little strange. When you say 'use the surface of the inner body to cut away part of the elliptical body,' you mean use the converted edge of the inner body to Trim Entities the elliptical body?

                                             

                                            In sketches I've had mixed results with Trim Entities. I try all the settings--Power Trim etc--what is "inside" and what is "outside"?--and click and drag away... and sometimes it works. I'm hoping Lombard's Bible will tell me how to use that tool consistently.

                                             

                                            Thanks again for the generous help, Jerry.

                                              • Re: How do you fully define a sketch?
                                                John Sutherland

                                                "I guess I've been assuming that SW knows if I make two parts match, like the outside dimension of one part and the inside of a part surrounding it, it will let them mate nicely."

                                                 

                                                Wrong assumption.  You seem to be thinking of nesting/spooning.

                                                 

                                                Coincidence of shape has nothing to do with mating.  SolidWorks bodies happily penetrate each other like a ghost walking through a closed door.  Mates are very simple rules for assembling bodies relative to each other; e.g. parallel, perpendicular, tangent, colinear, coincident.

                                                • Re: How do you fully define a sketch?
                                                  Jerry Steiger

                                                  Kris,

                                                   

                                                  There is a feature called Cut with Surface (I think; SW if crashing on me right now, so I can't check it). So when you have more complicated shapes, it can be a good way to make sure that two parts or bodies match up nicely in an area. You don't need it with your extruded bodies/parts, but it would probably be useful if you were trying to model the exact shape of your neural pieces in all of their three dimensional organically shaped glory. So long as you stick to your extruded shapes, you can use converted edges to do the cutting.

                                                   

                                                  I don't remember if you mentioned how you have learned enough to get this far. Have you worked through the SW Tutorials? They will help you get a better grasp of the fundamentals. If you are going to be doing very much modeling, and depending on howyou learn best, you might want to sign up for classes at your VAR or a college or community college. A local users group is also a good place to pick up good tips and tricks.

                                                   

                                                  I'm afraid I can't help much on trimming. I think I learned SW before they added some of the options. I use the default setting, whatever it is called. You click on the sections you want removed. My sketches are usually simple enough that I can click on the stuff I want to remove faster than I can figure out how to use one of the other options.

                                                   

                                                  Matt's Bible is a great reference book. It is not not set up like a course or a tutorial, though, so it is a bit tough on the person just learning the software. I think it is money well spent, for beginner or experienced user.

                                                   

                                                  Jerry Steiger

                                                • Re: How do you fully define a sketch?
                                                  Alan Stoldt

                                                  Jerry,

                                                   

                                                  Thank you. Been away from work and computers for around 9 days. Still trying to figure out if it is good to be back yet.

                                                   

                                                  Delete the other three spurs and fully defined what is left

                                                  --How?

                                                  Kris,

                                                   

                                                  What I meant was iin regards to the four spurs. I eliminated three of them and concentrated on getting the one remaining fully constrained. After that one bit was fully constrainded (or defined), I was ablt to mirrow it once horizontalilly, and then mirror both those once vertically. This results in all four remining fully defined, but only doing the work once.

                                            • Re: How do you fully define a sketch?
                                              Greg Hynd

                                              Matt Lombards solidworks 2010 bible is a good book. Seems to cover everything!!

                                              • Re: How do you fully define a sketch?
                                                John Sutherland

                                                Kris,

                                                 

                                                Flattery will get you everwhere.  I have Matt's Bible and I keep it at hand.

                                                 

                                                Here are my personal notes on sketching compiled from my interpretation of others' writing, and from my experience which will be different to others' experience.  There may be errors which I have not yet discovered.

                                                 

                                                 

                                                Sketches

                                                 

                                                You should plan the assembly before the individual parts, and explicitly specify the plane on which to sketch the base/first part profile, in order to avoid any need to reorient the part when it is inserted into the assembly.  Your assembly should follow the SW convention of Y axis vertical.

                                                 

                                                Sketches may be placed on a default plane, on any other plane, and on the planar face of a part.

                                                 

                                                The simplest definition of a plane is a point on a vector normal to the plane.

                                                 

                                                Dimensions are sizes of elements and distances between elements.
                                                Ordinates are locations of points, relative to the document origin.

                                                 

                                                A profile is a chain of elements.

                                                 

                                                The shape of the profile is defined by Relations which specify the relative orientation of elements.  e.g. parallel, perpendicular, angle, tangent.

                                                 

                                                The size of the profile is defined by the linear dimension (which may be a keypad entry or a function of known parameters) of one element, together with the proportions of the remaining elements to the dimensioned element.

                                                 

                                                The size of the profile may be scaled up or down by varying the one dimensioned element while the shape remains constant.

                                                 

                                                The position of a profile is its location and orientation in document space.

                                                 

                                                Constrained means employing Relations and Dimensions to define the shape and size of a profile so that it cannot be morphed by dragging.

                                                 

                                                Fixed means defining the position of a profile within document space by "nailing" it at two locations being centres of circles or vertices of polygons (thus denying translation or rotation), located by ordinates or by the Fix tool.

                                                 

                                                Fully Defined means constrained and fixed with necessary and sufficient relations and dimensions.

                                                 

                                                Relations may appear to be a free issue but are actually very costly.  Discipline yourself to use only necessary and sufficient relations.  Relations employed for positioning only (e.g. Vertical and Horizontal), should be suppressed after doing their job.  Disciplining yourself to avoid using the Fully Define Sketch tool (a very blunt instrument) will avoid unwanted consequences.

                                                 

                                                When modelling legacy designs, it seems easier to define sketches by multiple dimensions to infer proportion, rather than strain your brain to write equations.  This may lead to unwanted consequences.

                                                 

                                                New designs should aim for a single dimension per shape, and optionally extras for positioning.

                                                 

                                                While any fool can start a sketch (Command Manager>tab Sketch>tool 2D Sketch), she cannot exit the sketch to do something else until it is Fully Defined.  The document can however be saved in spite of the torrent of messages.

                                                 

                                                A simple profile such as a rectangle can easily be shaped by relations between elements.  A complex profile can benefit from a simple skeleton/scaffold Construction framework which is itself Fully Defined, and to which all profile elements can be related.

                                                 

                                                An example skeleton is a polygon, morphed as required, so that the vertices are the intersections of known and unvarying infinite lines, and the centres of significant arcs.  Default sketch polygons come with relations which must be deleted in order to morph them.

                                                 

                                                Fully defining a polygon of n sides requires n+(n-4) constraints (angles or lengths), plus two points constrained by ordinate dimensions to the origin, or by the Fix tool.  The last necessary constraint will turn the whole polygon black.  The first redundant constraint will turn it yellow.

                                                 

                                                Add shape elements and Relate (orientation and dimension) them to the framework by geometric relations and trig functions and linked dimensions and numeric dimensions.  Ensure each element has sufficient Relations to code it black before proceeding (define as you go, using if necessary the Fully Define Sketch tool on the selected entity).

                                                 

                                                Points are reference in space and not elements of a solid.

                                                 

                                                Trimming dangling entities may be necessary to make the sketch fully defined.  Mouseover highlights what will be removed.
                                                Avoid using end points of lines for other things.
                                                Avoid equality relations of length/radius where elements are filleted.
                                                Avoid using dimensions to infer relations.
                                                Add Virtual Sharps in way of fillets to retain identity of intersections.
                                                Apply fillets last.

                                                 

                                                The framework is the evidence trail for auditors.  Ensure that it is not trimmed out of the sketch, perhaps by Saving As and trimming in the new version of the document.

                                                 

                                                While sketch elements can be freely dragged on the plane, and their ordinates read in the Property Manager, the ordinates are not fixed until the position of the profile is explicitly fixed.

                                                 

                                                3D sketches are lines to guide sweeping and lofting of 2D profiles.