As a design engineer with 10 years on Pro/E and the last 15 years on SolidWorks designing machined parts, these would be my comments.....
• Your parts and drawing are
very good. Your parts could be made.
Being self taught, you are to be commended.
• If anything, the greatest drawback is that the parts are over-dimensioned.
A) For instance, the length of the 4 holes. I would have pointed at one hole and said "2X Ø.375 THRU". The exact length of the hole is the part
minus the 2 counterbores. When you give the length of the hole, then it is not clear to the machinist which is more important, the length of the part
or the length of the hole. The hole is therefore, double dimensioned. Obviously, the overall length of the part is far more important, the hole will fall out as a
result of the part length and 2 counterbores.
Rule: Only show the MOST IMPORTANT dimensions. Any dimensions that can be derived by simple math are NOT shown. If you want to give the dimension to save the machinist calculation time, then place the dimension in parenthesis, or follow the dimension with the word "REF". Those dimensions are then understood to be "for reference only" and are not "ruling".
Consider your checkbook monthly statement. If your statement told you your balance was $203.00 and yet the same sheet told you the balance was $203.02, then you'd be in a dither about what the exact balance was. This is exactly what you are doing to the machinist when you double-diemnsion. Capisce ?
B) You needn't give a detail view of both chamfers. There are realistically only 2 places an outside chamfer can be, and both are already shown. I have a BSME degree and a US patent,
but every machinist I ever met was way smarter than me, so give them some credit. Simply point to one corner and say "2X .12 x 45°". I assure you they will find the other corner.
And why is the corner chamfered? To make is easier to handle or fit, so a 3 place dimension (+/-.003") is not required. Notice I knocked it down to a 2 place decimal. This one move just saved you $200 in manufacturing costs.
And why did I make both chamfers identical? Because when you dimension them differently you are calling out for 2 separate machining setups. Use the dimension you
must have on one end, on BOTH ends and save money. Part cost is life or death these days.
Think about the cost. Think about the part as if it were YOUR money being spent.
And chamfers are dimensioned across the
horizontal or vertical, hardly ever across the face. This because a lathe is already setup to give this dimension directly from the machine controls. If you MUST have the .030" face, then you have to give the r
eference dimension for the horizontal or vertical so that the machinist doesn't have to do the trig.
C) Drilled holes do not have the same tolerance as machined holes. Drill bits are typically +.003/-.001" up to 3/8. If you want a drilled hole and will accept the resulting tolerances, then make it clear you what you want and will accept. Again we are concerned with cost. I might say "2X Ø.375 +/-.010 THRU", meaning you use a 3/8 drill bit and I'll accept the hole it generates.
Ø.2188 is a reamed hole. Do you really need a reamed hole? Really?
Holes are always called out in the "full face" view if possible; that is, the view in the lower left corner. Again, the shorthand nomenclature is used.... "2X Ø.375 THRU". The machinist will find the second 3/8 hole.
The purchase of a copy of ANSI Y14.5 would go a long way toward helping you improve your dimensioning.
Hope this helps!
I can measure your part and tell you where you put the features, but does it match your design intent? No reference to features, just imaginary points in space. What should the diameter or depth of the groove to be, for example? I would dimension the edge of the groove from a known end of the part and then dimension the width. Then I would dimension from the OD to the ID of the groove. Sorry to be critical....too many years of inspection experience!
