Guiding lines for part modelling

             From simple drafts and blueprints to parts and drawings, the design procedure becomes faster and simple with so many aiding tools that not all of them are known to the CAD users. Even the experienced CAD users are not familiar with a large percentage of commands that their CAD software contains. This is the reason that I am personally against changing from one CAD to another and I believe that is best to find one that suits your needs, applications and budget, buy it and learn to use it to a very good level. The design procedure in the modern parametric CADs, the visualization of the parts, the configuration files, the section tabs and the libraries help and guide the designer. These tools can also help anyone with a relative background to learn a lot about designing. At this point is interesting to separate the designing procedure in two related but also different functions. The first is to create parts and their assembly (part modeling) according to the given specifications and the second is documentation of the above in a readable format (part drawing). This separation is less distinctive from the old days due to the more holistic approach of current CAD. But not so many people approach the CAD programs in order to produce a complete solution. In the past I worked with design and development managers which produced CAD models and assemblies that supposed to be ready for drafting according to the standard procedure. Unfortunately for me, the parts needed more time in order to be documented in drawing format than to create them. There were many reasons for this, like no datum references, depended features, non-standard features, awkward shapes and others. The biggest problem was that the parts were not in a modifiable state. I use the term “modifiable state” in order to characterize how easily a part’s dimensions can be modified. I believe that “The problem” when creating and building parametric parts is to use a large number of reference features. This is clear in very complicated features were the modification of one feature changes or crashes many others (or crashes the entire model). This problem becomes dramatically huge when creating advance surfacing features, were a change of few microns of a dimension or the modification of a chamfer/radius can crash the model. This traumatic (but educational) experience helped me realize the importance of having some guiding lines from the early stages of part modeling. Making the part modifiable is essential. The life cycle of a product enables a lot of modifications and revisions and although this seems like an easy thing to do, in reality it takes a lot of time. Some may ask “Ok, are there any parts that will work without any modifications from the initial design?” These parts if they work from the prototype phase, in the future may be modified into different size in order to suit to another relative application.

 
     These guiding lines apply for the part modeling; remember the essential is to build the correct CAD model. Actually this is the first guiding line.
Prefer removing material from the initial shape instead of adding to it. Consider yourself as a machine tool operator who creates the part from raw material.
Prepare a standard raw material availability list. Avoid parts with overall dimensions, not of available sizes.
Select the initial feature position in reference to the datum planes considering the shape complexity.
Prefer sketching the features with the initial datum planes as datum. For parts that require the development of more complex processing techniques/set-up choose datum which you know exactly how it will react in modifications. As a rule, select or build your datum that the machine tool operator will use.
Use relations between sketch dimensions and features (basic in many CADs). The application of relations simplifies the modification. For example when placing four c-bore holes in each corner of a rectangular plate that are symmetrical (or centered) to the center lines of the rectangle (choose them as datum), you follow the sequence below: Initially, you place one c-bore in reference with the datum (creation of two dimensions) and afterwards you make the pattern of the hole (another two dimension creation). Now if you make relations between the driving hole dimensions and the dimensions of the pattern  you will have two position dimensions in total. In the same example if you want each one of the four holes to have equal distance from the two adjacent sides of the rectangular plate, you can accomplish this by changing only one dimension. In this rectangular plate, L and W are the length and width of the plate and A is the distance of each hole from the adjacent sides. Next step is to place the driving hole and create the pattern. Create an equality relation between the position dimensions of the first holes d1=d2=A. Create a second relation for the pattern dimensions d3=L-2d1 and d4=W-2d1. With this way when you modify the overall dimensions of the plate, the hole pattern is also modified.

Another example is the placement of two threads, each one on the face of a thin wall created by a shell command on a box. The wall thickness and the external dimensions of the box will have to be modified, but this will also change the placement of the threads. If W and B are the external and the internal dimensions of the box, then the center distance between the threads will be d1= (W+B)/2 (see figure below). The relation tool usually supports many standard arithmetic, trigonometric, logical and part related functions.

Avoid sketches with complex geometry, break them down to more simple ones. Large sketches are difficult to edit and modify.
Use datum balls for very complex feature if it is difficult for them to be dimensioned from the initial datum planes.                     
Remember that the parts and drawings (“the archive”) are something alive.