detailing symmetrical parts

A couple of questions on detailing symmetrical parts or parts with
symmetrical elements.

What is the prefered method for showing that two similiar elements are
equally spaced across a centreline - I remember back in college we were
taught to have a dimn between the two elements then two dimns from the
centreline to each element with an equality sign - is this still acceptable?

Or should I ignore the major dimn between the elements and just create two
dimns each side of the centreline - these would then need individual
tolerences half that of the general tolerence.


Wildfire 2

Also, if I have created a half view [of a completely symmetrical part], how
do I create a dimn between two elements each side of the symmetry line
[obviously I cant see the other element to pick it] - say two holes? Or, as
above should everything be dimensioned to the symmetryline? If this is so,
what do I hook onto at the symmetryline as everything on the symmetryline -
axis, reference plane - is not displayed - have I missed something.



Cheers, Sean


--


~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
Sean Kerslake
Dept. Design & Technology
Loughborough University
Loughborough
LE11 3TU

01509 228317

 

:
: A couple of questions on detailing symmetrical parts or parts with
: symmetrical elements.
:
: What is the prefered method for showing that two similiar elements are
: equally spaced across a centreline - I remember back in college we were
: taught to have a dimn between the two elements then two dimns from the
: centreline to each element with an equality sign - is this still acceptable?
:
The preferred method is to adhere to a widely accepted standard ~ ISO, ANSI, DIN,
one of those. Get it off the shelf, dust it off and take a look at it. Raise the
kids right, maybe they'll follow it later, when they get out in the real world.

The standard I'm familiar with is ANSI. It's minimalist: minimum number of
views/dimensions to completely and unambiguously describe a part so that it can be
made and made in only one way. Another aspect of its minimalism is assumptions: if
the line looks straight, vertical, horizontal, parallel, perpendicular, tangent,
then it is. A dimension is need only to clarify when the apparent is NOT the case,
as in, when a line looks parallel to another but needs an angular dimension to
clarify that it is not parallel; or when a line looks perpendicular but needs a
dimension to clarify that is drafted (and natually, the amount of the deviation
from perpendicularity).

You will have noticed in Pro/e's sketcher that you can see all these symbols ~ for
perpendicularity, parallel, tangency, coincidence, etc. But, when you show
dimensions in detailing, none of these symbols and characteristics of the geometry
show. The same is true for symmetry: draw a center line on each of the datums,
create a rectangle, dragging it from the upper left to the lower right quadrants
and you automatically get symmetry and notion of such on the sketch. Add a circle
in the upper left quadrant, near the corner, mirror it to the right side (more
symmetry notation) and mirror these to the bottom (symmetry notation again, now in
both directions). Two dimensions control the rectangle size, two control the
circle placement. Then extrude a solid feature a certain thickness, five dimenions
in all. Make a print of this with two views (Top, Front), show all the dimensions
and those same five dimensions show on the print. Can you make this part correctly
with those dimensions? You most certainly can and it follows the ANSI rules. There
are no centerlines showing, no overt dimensions from an edge to a centerline and
from centerline to hole. Yet, all the assumptions normally made about ANSI
dimensioned drawings tells you that there is no other way to make that part.
Furthermore, Pro/e sketcher assumptions are perfectly compatible with ANSI
detailing assumptions. It also tells you that the only reason to add centerlines
and to dimension from centerlines to a hole is if the symmetrical-looking pattern
is NOT symmetrical, in fact. GD&T is a similar kind of amending or clarification
of assumptions, in as much as the assumptions require the absolute, the ideal
condition. GD&T says how much deviation from perfectly square, perfectly round,
perfectly flat, etc. is allowed.

The last point is what is the most appropriate use of symmetry. I'm not sure if
this is covered by the standards, but I've seen it most often used in two
circumstances: in castings where the dimensioning of a pattern of features,
irrespective of its location, is a critical characteristic of the part and, where
there is no ready, machined surface from which to make or measure the pattern
location to the same degree of precision as the pattern's internal spacing; the
other is in just the opposite type of fitted block where outside boundaries are as
much a critical characteristic. The centrality of the features was preserved by
removing equal amounts of opposite fitted sides.

David Janes

 

....

Yes, it will. It will show the sketcher reference dimension exactly as it
was created in the sketcher, with a 'REF' postfix. If you prefer to have a
refernece dimension in brackets, you'll have to modify it.

 

: ...
: > That being said, the users of the drawings (especially tooling and
: > fixtures) may like to see the overall dim and the dims between the
: > elements, even if they are shown as reference. This would reinforce the
: > idea that the feature is symmetric.
: >
: > I don't remember if Pro-E will show sketcher reference dims on drawings
: > (I don't think so).
:
: Yes, it will. It will show the sketcher reference dimension exactly as it
: was created in the sketcher, with a 'REF' postfix. If you prefer to have a
: refernece dimension in brackets, you'll have to modify it.
:
Or change the config option, parenthesize_ref_dim, to YES. The dimension will show
this way in sketches and drawings.

David Janes