17 Replies Latest reply on Nov 10, 2009 6:47 PM by Ryan Laplante

    Why is 3D sketching so hard !?!?!!?

      Why is 3D sketching so hard and why can't I get SolidWorks to do what my brain says it should do? This is supposed to be 3D solid modeling and I want to design as my brain envisions it in 3D. I just seem to so much time on sketching. Is there a good tutorial for just 3D sketching that anyone could recommend? I realize I'm a newbie to SoldWorks but 3D sketching just should not be this hard.


      Thank you,

      Chris

        • Why is 3D sketching so hard !?!?!!?
          Dale Dunn
          I don't know of any tutorials other than what comes with the software. Is there a specific issue you need a nudge on?

          Different people have different results with 3DSketch. I do somewhere between OK and well with it, but it took me a while to get the hang of it.
            • Why is 3D sketching so hard !?!?!!?

              Dale Dunn wrote:

               

              I don't know of any tutorials other than what comes with the software. Is there a specific issue you need a nudge on?



              Different people have different results with 3DSketch. I do somewhere between OK and well with it, but it took me a while to get the hang of it.

              Dale,

              Take a look at this part. Open the 3D sketch that is under the extruded surface labeled "Pull Tab". Can you show me how to fully constrain the sketch and use dimensions so I can adjust the size of sketch later if required?

              Thank you!

              Chris


                • Why is 3D sketching so hard !?!?!!?
                  Dale Dunn

                  Chris Maiden wrote:

                   

                  Dale Dunn wrote:

                   

                  I don't know of any tutorials other than what comes with the software. Is there a specific issue you need a nudge on?







                  Different people have different results with 3DSketch. I do somewhere between OK and well with it, but it took me a while to get the hang of it.

                  Dale,



                  Take a look at this part. Open the 3D sketch that is under the extruded surface labeled "Pull Tab". Can you show me how to fully constrain the sketch and use dimensions so I can adjust the size of sketch later if required?



                  Thank you!



                  Chris

                  Sorry, I'm stuck on 2007. Maybe someone else can jump in and take a look. Maybe I can describe it verbally or reproduce it if you post a screen shot.
              • Why is 3D sketching so hard !?!?!!?
                Tom Nicholson
                yea, It can be a pain in the ass.. I think the only time I've ever used 3d sketching was to make a weldment.. and then it was a bitch to use..

                I guess the best thing to do is learn how the 3d sketch works, how to switch planes on the fly.. I know in the tutorial section, under building models, there's a couple on 3d sketching
                • Why is 3D sketching so hard !?!?!!?
                  Kevin Quigley
                  What is it you are trying to create? 3D sketching has many different uses. For something like a weldment setting up reference planes first would be a good step and using them to drive the sketch. For more freeform stuff try staying in one plane and moving the points after you have the rough shape. Take a look at Matt Lombards Surfacing book - there are some examples in that - or I think Mark Biasotti's surfacing videos cover some 3D sketch use as well.
                  • Why is 3D sketching so hard !?!?!!?
                    Roland Schwarz
                    The best advice I have about 3D sketching is to go carefully and slowly. Constrain as you go. Don't leave too many underconstrained entities out there. Constrain endpoints whenever possible.

                    Use the tab key to switch between X-Y, Y-Z, and Z-X planes.

                    You can sketch on faces and datum planes by selecting a face or plane before drawing.

                    Turn on "Display entity points..." and "Display arc centers..." in your sketch options.

                    Lines can be constrained coincident with, perpendicular (normal) to or parallel to surfaces and datums.
                    • Why is 3D sketching so hard !?!?!!?
                      Charles Culp
                      Chris, I'm trying to edit your part to make it all constrained, but your design is not set up the way I would do it.

                      I can say that in general, what you need to do is create construction lines along the X, Y, and Z directions, connecting your endpoints. Start with one at the origin, and connect it to one of the corners of your part. Then you can dimension where your sketch endpoint is in relation to the origin (or other datum starting point of your choice) by dimensioning those construction lines. Then you need to create more X, Y, and Z construction lines, and constrain to those. You can also use the "parallel" constraint to keep things parallel to planes. Don't forget about the "on plane" and "on surface" constraint. This is great for endpoints.
                        • Why is 3D sketching so hard !?!?!!?

                          Charles Culp wrote:

                           

                          Chris, I'm trying to edit your part to make it all constrained, but your design is not set up the way I would do it.



                          I can say that in general, what you need to do is create construction lines along the X, Y, and Z directions, connecting your endpoints. Start with one at the origin, and connect it to one of the corners of your part. Then you can dimension where your sketch endpoint is in relation to the origin (or other datum starting point of your choice) by dimensioning those construction lines. Then you need to create more X, Y, and Z construction lines, and constrain to those. You can also use the "parallel" constraint to keep things parallel to planes. Don't forget about the "on plane" and "on surface" constraint. This is great for endpoints.

                          Thank you Charles!

                          Please feel free to correct my design in anyway. I will learn so much from your corrections I am most sure. Being a newbie from the AutoCAD world I am learning so much from all of you SolidWorks Gods on these forums!


                          Chris




                          • Why is 3D sketching so hard !?!?!!?

                            Charles Culp wrote:

                             

                            Chris, I'm trying to edit your part to make it all constrained, but your design is not set up the way I would do it.



                            I can say that in general, what you need to do is create construction lines along the X, Y, and Z directions, connecting your endpoints. Start with one at the origin, and connect it to one of the corners of your part. Then you can dimension where your sketch endpoint is in relation to the origin (or other datum starting point of your choice) by dimensioning those construction lines. Then you need to create more X, Y, and Z construction lines, and constrain to those. You can also use the "parallel" constraint to keep things parallel to planes. Don't forget about the "on plane" and "on surface" constraint. This is great for endpoints.

                            Charles,

                            I added the construction lines and dimensions as you suggested and learned a lot doing it. I still have to dimensions i can't get to work. Could you take a look at it and see what I've left off and or constrained incorrectly?


                            Thank you sir!


                            Chris
                            • Why is 3D sketching so hard !?!?!!?
                              Charles,

                              I have applied your advice to parts in my current project and I'm slowly but surely understanding 3D sketching. Brfore I had not understood the relationship of using construction lines to constrain and adjust location and size of a sketch from the orgin. I'm still having trouble getting a sketch fully constrained but I'm sure eventually I'll get there. I have also used the SketchXpert to analyze, understand and correct all the constrain errors I get.

                              Once again thanks for your help and patience with this SolidWorks Newbie


                              Chris


                              Charles Culp wrote:

                               

                              Chris, I'm trying to edit your part to make it all constrained, but your design is not set up the way I would do it.



                              I can say that in general, what you need to do is create construction lines along the X, Y, and Z directions, connecting your endpoints. Start with one at the origin, and connect it to one of the corners of your part. Then you can dimension where your sketch endpoint is in relation to the origin (or other datum starting point of your choice) by dimensioning those construction lines. Then you need to create more X, Y, and Z construction lines, and constrain to those. You can also use the "parallel" constraint to keep things parallel to planes. Don't forget about the "on plane" and "on surface" constraint. This is great for endpoints.

                                • Why is 3D sketching so hard !?!?!!?
                                  Klyde Keeler
                                  I'm new to SW but Yes, I can't seem to catch on either... back in the day, turn of the century, I used Vellum. They had a wonderful 3-D drafting tool.... if anyone in a position to help is reading maybe they could check it out. I don't know what their current product is like.

                                  So in a related thought am I the only one that thinks the ISO and Trimetric views are weird. I'm and engineer with a machining background and Z is North and South except sometimes like when you are working on fixturing for a horizonatal mill but that is the exception.

                                  I thought this was the strangest thing in the training class but when I asked they all looked at me like I was nuts so I just dropped it. But I really have trouble convincing myself to create a model contrary to the way I envision it, will manufacture it, import it into a CAM package, use it and so forth.... I bet there is a way to reconfige something or set a temp axis or something but I would appreciate the oppurtunity to understand what "everyone else" is thinking. I am just getting too old?
                              • Why is 3D sketching so hard !?!?!!?
                                Charles Culp
                                Klyde,

                                One trick I have heard is to set up solidworks with the "4 views" approach. Window>Viewport>4 view. Then make sure three of the views are set to XY, YZ, and ZX. Then you can drag lines in the appropriate planes automatically, and things won't "go flying everywhere".

                                You can modify your axis/coordinate system. Here is a thread discussing that: http://forum.solidworks.com/fo...atid=10&threadid=9084

                                Can you give a more specific example of what you don't "get" with 3D sketching?
                                  • Why is 3D sketching so hard !?!?!!?
                                    Charles,

                                    Your original posting on the methods for 3D sketching seem to be the best. It's still taking me a while to apply them but I feel I have a far better understanding than when I first asked. I still can not get fully defines sketches but I can get "dimension adjusted" sketches now.

                                    Thank you!

                                    Chris

                                      • Re: Why is 3D sketching so hard !?!?!!?
                                        Ryan Laplante

                                        This is how I make 3d sketches that can be used for extruded paths and other complicated shapes.

                                         

                                        I design tubular legs for furniture and have come across a very solid way to create and update 3d sketches - using solid geometry.

                                         

                                        Starting on the right plane draw your part in side profile or at least just block it out from one solid angle this can be whatever view suits you.

                                         

                                        Using the sketch on the right plane 3d sketch out construction geometry lines which will control the planes that your 3d sketch needs to follow.

                                         

                                        Insert all relative planes into sketch - these are all sketch driven so they can be used and changed in configurations.

                                         

                                        Using your recently created drawing view of the object - block out the large shapes and extrude them up to the relative planes.

                                         

                                        Now for the fun part - start a 3d sketch and convert the edges of your solid geometry into a 3d sketch - you can always add fillets because its always co-planar.  Then insert a plane normal to curve and draw your extrude shape.

                                         

                                        Take the part I have attached and roll it back to the first sketch and then roll it forward one step at a time, you can modify the 3d sketches controlling the planes and affect the entire profile of the path extrude, which will automatically update.