Solid Thinking: Better Sketching is the Foundation of a Better SolidWorks Design16 Nov, 2004 By: Greg Jankowski Cadalyst
Define a procedure and communicate it well to all users in your organization
Sketches are the building blocks of your designs -- a better sketch equates to better a design. But good sketching isn't as simple as it might sound, and your organization should put some thought into how it can best incorporate sketching into its design process. As with any best practice, the key here is to define how this approach benefits your company and communicate the practice and the reason for it to all users.
So why is creating a good sketch so important? A well-defined sketch will help capture design intent, the means by which a designer can build and document his or her design intentions into the model. An example would be a hole that should always be located in the center radius profile (figure 1).
Figure 1. An example of a design sketch (before).
The basics of good sketching are determining the extent or scope of the sketch; sketch order (sketch, constrain, and dimension); design intent; exercising your sketch; and geometrically and dimensionally constraining the sketch.
Sketch the Geometry
The first step is to determine how much detail should go into a sketch. The sketch shown in figure 1 has the profiles and the holes in the same sketch. A better practice would be to break this sketch into a couple of features. This makes the features easier to modify, and the hole wizard could be used to add more intelligence to the hole (for example, thread or counter bore). A sketch that has too many features is much more difficult to constrain because it has so many geometric and dimensional constraints. Having three features in this part would also better describe the intent of each of these features. One rule of thumb is to use functional grouping. In this case, I would separate the profile from the holes.
Typically, cosmetic fillets should be added as a separate feature at the end of the design. This example uses fillets that are part of the design intent. Therefore, they were included in the sketch. The two tangent fillets between the large arc were included because that was easier than trying to create the intersecting lines and add a fillet later.
You should create a sketch in a definite order. First create the sketch entities (figure 2). Note the holes were removed and the main feature was renamed MTG PLATE PROFILE. Also note the two sketch relations (tangent) that were created automatically. SolidWorks displays an indicator during sketching that a relation is created. You can override this automatic relation during the sketch by holding down the Ctrl key while creating the sketch entity.
Figure 2. Create the sketch entities.
Figure 2. Create the sketch entities.
Create the Geometric Relationships
The next step is to add the rest of the geometric relationships using the Add Relation function. Too often this is overlooked. One of the attributes of a good sketch is the ability to change the sketch and have it update as intended. The original sketch was underconstrained both geometrically and dimensionally. This is bad for a good number of reasons. The original geometry was not given enough information to fully solve the sketch. This is not precise and cannot be easily modified.
Another advantage of using geometric constraints is that fewer dimensions are required to fully constrain the sketch. SolidWorks displays underconstrained geometry as blue, fully constrained as black, and overconstrained as red. Use this graphical indicator to determine which items need additional constraints.
Now our sketch is fully constrained geometrically (figure 3). Note the use of construction geometry (center lines). Any sketch entity can be made a construction element within the sketch. The PropertyManager has an optional check box, For Construction, that you can check to denote the entity is for construction or reference use only.
Figure 3. The sketch is now fully constrained geometrically.
Exercise the Sketch
After the sketch is constrained, exercise it to ensure the intent is correct. Drag the sketch elements to a different position and resize to see if the sketch behaves as expected. This does not take long, and should be done before you add dimensions to the sketch. Once dimensions are added to the sketch, it will be harder to determine where you need additional geometric constraints. By taking this simple step, your sketches will behave better and modify more consistently.
Another method you can use to exercise your sketch is to create the sketch in a different size and location than you will use for the desired finished sketch. This is done so that as the sketch is modified, you can see if the sketch changes in the manner you expected. If not, additional geometry constrints may be required.
Dimension the Sketch
Once the geometric constraints are complete and you have exercised the design to see if it matches your design intent, dimensions can be added to the sketch. Once all the dimensions have been added our sketch is fully constrained all sketch entities will be colored black (figure 4). One of the advantages of the geometric relations is that the R.360 dimension is only shown once on the sketch.
Figure 4. Dimensions have been added to the sketch, which is now fully constrained and final.
This sketch has been made so it can be reused to create the detail drawing. Notes, tolerances, or annotations can be added to the sketch so it can be reused to create the drawing view. Some additional dimensions are required for the detail view that was not required to fully constrain the sketch, and those display in gray in the figure. These are driven dimensions, which mean they are driven from other constraints and driving dimensions. A driving dimension is shown in black and can be marked for drawing reuse (figure 5). Use the drawing function Insert Model Items to import these dimensions and annotations into a drawing.
Figure 5. Mark a dimension for drawing reuse.
Finish the Design
To finish the design, we need to add the two sets of holes (figure 6). Note the use of good names for each feature.
Figure 6. The final part design.
Good sketches are the foundation of a good design. Good sketching concepts are not difficult or time-consuming to implement, and they will result in better, easier-to-modify sketches. Always remember to define, communicate, and reinforce this important practice to the other users in your organization.
About the Author: Greg Jankowski
Autodesk Technical Evangelist Lynn Allen guides you through a different AutoCAD feature in every edition of her popular "Circles and Lines" tutorial series. For even more AutoCAD how-to, check out Lynn's quick tips in the Cadalyst Video Gallery. Subscribe to Cadalyst's free Tips & Tools Weekly e-newsletter and we'll notify you every time a new video tip is published. All exclusively from Cadalyst!