gears in drawing

I am making some gears and I would like to know what is the best way to show
the teeth in a drawing doc. It looks funny if I leave the teeth showing and
it is very time consuming to hide all the teeth lines.
thoughts?

Nathan

 

Yes this is what I was looking for but I would have to section the shaft and
my superiors say that a shaft shouldn't be sectioned. Or should I do a
broken out section view where the teeth are on the shaft?

 

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?)

 

Yes
yes
and yes.
I guess it is a more of general question. I know that I will be draing
gears, a shaft with gears cut into it. I am just looking at how is the best
way to show the teeth using a soild model. I don't want the 2D guy giving me
crap because my 3D model drawing doesn't look like his 2D

 

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.

---------------

(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.