This page is designed to increase the accuracy and general cleanliness of your cylindrical part modeling. In order to understand what goes into a parametrically-modeled part, it's often necessary to use simplicity as a goal. There are always multiple ways of modeling the same feature(s) but oftentimes they will overcomplicate your part and reduce the level to which it can be edited in the future. (although that may not be your goal, so hey)
The general rules I try to follow involve the following ideas:
· Avoid chain-dimensioning features. Instead try to dimension parts from a single feature (or edge) on the model. This will help reduce the issue of stacked tolerances which can lead to inaccuracies on your model. This also applies to making multiple sketch planes; measure the planes and/or cutting depths from a single point, instead of measuring the planes to each other and/or the distance between cut sections (respectively).
· Avoid associating nearby features as much as possible. I know you're thinking, hey that's the point of a parametric modeler! That's true, and it can be handy to form associations with nearby parts, but remember this is only possible if you keep the reference line intact. If you delete the line, any sketches using it for reference will no longer work! (you then have to go back and re-draw features)
The alternative to this is to make the part feature associated with nothing, and therefore when you remove or change earlier nearby features, the later feature will still work.
Obviously this varies from situation to situation. There are times when you won't be making any changes whatsoever to the nearby features, but rather just altering their size, etc. If that's the case then ignore this[above] and go nuts with the parametric associations.
Here's the most important rule. All features that are contiguous with the basic cylindrical shape of the part can be made on the same sketch plane. This means you can reduce the number of features by combining different parts of the profile together. These modeling programs are set up to allow you to add secondary cuts, chamfers/fillets, lofts, and other operations onto the base part feature....however, just because there's a "fillet feature" command doesn't mean you should use that instead of simply integrating the fillet into the 2d sketch.
This may seem like a trivial issue but I see it many times in industry and it makes me shake my head each time. The complexity of the part features is directly related to how many features you use to create it. It won't make much difference for a simple part like a hollow tube, but for a complex part such as those found in a pneumatics system, which can have hundreds of features, can make the model much more difficult to understand. The other advantage of this is the ease of editing: you need only edit one single sketch instead of editing one sketch then a part feature, then another sketch and part feature, etc etc since all the parts are related to one-another. The filesize will be smaller, too.
Here's an example part. Click on the assembly view below and try to guess which of the models is a single revolution, and which is made up of many smaller features.
The two parts are identical in every way! Except for how they were modeled....
As you can see, the right part was created using a series of extrusions, some adding to the part and some subtracting from it, as well as a lofted feature and a fillet on the end. The left part was made using a single 2d sketch located on a bisecting plane for the cylinder's long axis, onto which the entire part profile can be created (which makes parts such as the angled surface extremely easy). And thus the entire profile of the part is modeled in one fell swoop, and the only things you have to add are features not contiguous with the long axis (such as porting through the side of the part, or something).
I've noticed that this practice is very foreign to many newcomers to parametric software. I remember back in 2002 when I was learning Inventor, I did the same thing (and my models were horribly overcomplicated as a result). However, after time, the commands and features become second-nature and you're able to visualize combining multiple operations together to reduce complexity. It has many benefits.
The only time I specifically avoid this is if I made a model designed to additionally demonstrate the production method. For instance, a part machined on a lathe often requires more than one tool to be used for cutting into it. Sometimes it can be useful to show the operations made by one tool, then the operations made by the next tool, then the next, etc. For instance, you can start with the outer profile of the part, then show the small grooves made into it (using a grooving tool) then the angled thread relief (using a single-point cutter) then a bore drilled down the middle of the pat (using a drill bit). This isn't often used, since the machinist should be able to recognize those things, but sometimes it aids the design process.