"Sean Kerslake" wrote in message news:cbrae6$2r7$ snipped-for-privacy@sun-cc204.lut.ac.uk... : : 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