gears in drawing

Back in the old days, only one or two teeth were shown, with minor and pitch diameters shown in phantom lines. If this is what you're after, make a configuration of the part with your tooth pattern reduced to two teeth, then show that in your drawing view, with the relevant circles sketched o nthe drawing view. Instead of changing the pattern, you could also add an extrusion to consume them.

Is that what you're after?

Nathan

Perhaps you should ask the initial question again, being more specific about what you are trying to do. Your reply suggests that your view is looking at 90 degrees to the direction Dale (and for that matter I) thought you were. Please clarify this, also Is the shaft integral with the gear? Are the teeth cut into the shaft? (ie does the PCD of the teeth lie within the diameter of the shaft?)

A broken out section is usually the way this situation is resolved.

Broken Out Sections, in SolidWorks, suffer greatly through relying on a solid edge at the desired section depth. There almost never is such an edge.

TIP: use a split line to create one.

------------------------ WARNING: The following is a long ramble which does not directly seek to answer your question, more to put you in a position where you don't feel the need to ask it. Alternatively, to put you in a stronger position when the inevitable conflict arises with "rule-bound 2D dinosaur-brained" protagonists.

You may prefer to move on now!

The "rule" about not sectioning shafts, like any rule, works best if those applying it understand the underlying purpose. This helps individuals to decide which rules to apply when the underlying CAD data is 3D rather than

2D.

In most cases 2D vs 3D "turf wars" evaporate if this is done.

As I understand it, the purpose of this rule is to help the person interpreting the drawing to pick out any essentially cylindrical bodies which pass through the items we are sectioning. If we section shafts, bolts etc, the drawing gets hard to interpret if they are plentiful, which is often the case.

Hence a fuller statement would be "do not axially section essentially cylindrical bodies" where a fuller definition of "essentially cylindrical " would be "items comprising largely cylindrical entities, along with other features which can be depicted in an external view" The latter qualification picks up such enhancements as polygonal portions (eg bolt heads, square locating bosses per carriage bolts), external threads, and "sticking-out" bits generally.

Another convention is that (dashed) hidden detail should not be used in sectional views, once again because the interpretation of a mixture of hatching and dashed lines is problematic for the human brain.

Personally I happily break this rule if the hidden detail lines are well away from any hatching, say if the hidden detail represents a hole along the axis of a shaft which is not being sectioned.

If a shaft includes complex features like oilways which run out to the interface with the surrounding (sectioned) housing, the "hidden detail" rule (to my mind) trumps the rule about cylindrical bodies not being sectioned, and the shaft in this case should be sectioned, unless it is not appropriate -- in this view, for the target audience-- to show the oilways at all. If these features are local rather than full length, (say a woodruff keyway, spline or gear teeth), it is usually preferable to make the sectioning local (ie the broken out section you allude to).

My limited understanding is that most of the "rules" which should be abolished or re-written when moving from 2D to 3D are those whose purpose was to make it easy for the drafter in a 2D environment.

2D drafters were fairly near the bottom of the pecking order, hence such rules are infrequent. There were, however, *practices* which were common in the 2D world which can be confused with rules, and these should be scrutinised with extreme prejudice when moving to 3D.

An example: It was common practice in 2D machine design and drafting to try to convey as much as possible with each sectional view. In most cases this was simply a reflection of the laboriousness (for humans) of producing multiple views and sheets. In 3D the opposite is true. It is very difficult to, say, "fudge" by depicting fasteners which do not quite lie in the section plane as though they did. Much easier to place a dedicated sectional view for each item we want to depict. Fresh sheets with (simple) new views are not a problem for a computer; they are good and fast at menial laborious repetitive tasks, provided these can be specified easily and unambiguously. In this they differ markedly from (most) humans.

BUT we need to make sure we don't lose sight of whose benefit we are drawing for (strictly speaking, this is NOT our boss, and definitely not us). Remember that the person interpreting orthographic drawing views does not know or care that we are working from a solid model. If there is merit in showing multiple items in one sectional view, perhaps because their relative positioning is important for the person who has to interpret the drawing, we need to take it on the chin and find a way to make it happen.

Someone might jump in here and say "Surely it's just a question of joggling the section line ?", to which I would reply that I'm talking about section planes which are joggled in two mutually perpendicular directions, a "fudge" which was common in 2D drafting but very difficult in 3D. The easiest way in 3D is to create a part or assembly configuration and use several Cut-Extrude operations in that configuration to physically cut away the model so it looks something like the top face of an array of adjacent stacks of dominoes of randomly different heights. Then "Area Hatch" can be used in a drawing view looking square on at that stepped surface.

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(To amplify what I said at the top of this post): Broken Out Sections, in SolidWorks, suffer greatly through relying on a solid edge at the desired section depth. There almost never is such an edge. TIP: use a split line to create one.

The only other way is to specify a depth as a distance, but SldWks forgot to tell us where that depth is measured from. This is a bit of an insult to our intelligence, I feel, but it demonstrates well. By inference, (please jump in here if you know better) the datum for that depth is the nearest vertex of the 3D 'bounding box" of the part, although last time I checked there was a 6mm discrepancy. ( ! ) In practice, using either method (other than the Split Line workaround), there are no grounds for confidence that the depth will not change capriciously. Occasionally, a configuration of the part, using Cut-Extrude similar to the method above, is also the best way to tackle a broken-out section.

Broken out sections need to be able to derive their depth from a plane or a sketch point in the part model. This may have been fixed in 2004 - I don't know either way.