Anthony's Advice on Cost-effective Part Design

(Reproduced with permission from an Anthony post to alt.machines.cnc)

On a thread earlier in the week, I happened to remember a couple of old posts about drawings and design for manufacturing that may be worthy of a repost for any Engineers who happen to be newer to the group.

If you follow some of these thoughts, your parts will be *much* cheaper to produce.

1. Remember the KISS rule: (Keep It Simple Stupid), Sure...fancy pants looks good, get all the oogles and awes, but they generally don't WORK well. Simple is cheaper to make, cheaper to repair, MTBF (mean time between failures) is longer, and easier to operate.

2. Understand what you are designing, from all facets, not just the part, but how that part interacts with it's environment. Understand the entire process, not just one little snippet.

3. Do NOT TOLERANCE ANYTHING that doesn't absolutely have to have a tolerance. Use a general border tolerance, like ISO 2768. Tolerance fits, and other critical features, and ONLY those things. A General Note tolerance for bolt hole locations and other common features is perfectly acceptable and preferred by many in the machining trade, and it UNCLUTTERS the drawing. Remember, typically, you do NOT need a +/-0.002" tolerance on a bolt hole location. Tolerances cost money, pure and simple. The more tolerances, the more the part costs. The tighter the tolerances, the more it costs. Even if you give +/- 3mm for tolerances, but you tolerance every feature on the drawing, your part will COST MORE. Job shop guy scanning a drawing for quote sees 100 toleranced dims on a drawing...he jacks the price up, it's a fact of life.

4. Learn the practical application and practical meaning of GD&T tolerancing as it applies to making parts. A true position tolerance is generally NOT needed on everything on a drawing. True position is NOT a "catch-all" tolerancing method, as so many seem to think. Again, refer to item #3 above. Use the proper GD&T tolerance for only those features that absolutely require it.

5. Most do this, but take into account when you design a part, what stock raw material sizes are readily available. Your goal as an Engineer in search of cheaper parts is to reduce the amount of machining needed to produce your part as much as possible. If it can be made from 1"x4" saw- cut bar stock, it will be MUCH cheaper than a part where a custom sawed 1-3/16"x 4-1/8" piece of material is required. DEFINE what overall size of material is needed to produce the part on the drawing.

6. While taking #5 into account, make SURE you either give or allow the machinist to make whatever qualified surfaces are needed to actually produce the part within tolerances on his machines.

7. Take into account what sized, lengths and shaped cutting tools are commonly available, and those that the machinist probably has readily available on-hand.

8. While you are thinking about #7, and designing your part, think about how many different tools it will take to produce your part. The more tools, the more it costs. Consider tool changes to be set-ups, for that is what they truely are. Consider putting a tool list on the drawing, of what you had in mind when you drew the part. This little tid-bit of information can give the guy quoting your parts a) a handy reference b) Allows him to better follow what you had in mind when you drew the part. Consider including a drawing of the geometry of any special tool needed to make your part right on the drawing.

9. On the same subject, the larger diameter/radius tools you allow the machinist to use on your part, the cheaper it will be. Generally, larger tools can be fed much faster, decreasing machining time considerably. Decreased machining time directly == less cost.

10. Think about what operations are needed to produce the part. How many times does the machinist have to re-fixture it to cut your features? Is the machinist going to have to make a fixture to hold the part, or can it be held in a plain and readily available vice, collet or chuck? The more set-ups there are involved in making a part, the more it will cost. The more special fixtures he has to make, the more it costs. Even soft jaws. You can even call the shop you are using and ASK what sized soft jaws he has on-hand, if the diameter isn't truely critical.

11. Do you *really* need that slick finish? 90% of the time...NO. So why specify it? Slick finishes cost $$$$. Spec a more than reasonable Max Ra, and let it be. 99% of the shops out there will send you a good looking part, at no extra charge, because it reflects on their business visually. Most shops, if you specify a fine finish, will GRIND the part. GRINDING is EXPENSIVE.

12. When you design your part features, make sure you do not forget the following items: a. Max R for inside corners. Square corners means EDM, if it can't be broached, or in the case of lathes, extremely short-lasting sharp- cornered tools. Any of which is expensive. b. Large enough undercuts for ground meeting faces that the machinists doesn't have to dress the corner of the wheel and re-pick up on the part a half a dozen times. c. Min/Max chamfer sizes - can be a note.

13. Reduce Grinding and EDM work to the absolute minimum. Allow hard turning if possible.

14. Pick out a good, feature-defined datum from which to dimension. A large hole, or the corner of a square part. You want something, if possible, accessible from any orientation that the machinist must fixture the part to machine another feature. If he can use the same datum for all set-ups, the parts will be cheaper, as the probability of something going awry are greatly reduced. Diminsioning from a theoretical point in space, or an arc where the center lies off of the part WILL cost you money, guaranteed.

15. Keep dimensions readable, traceable to the feature and uncluttered. If two dimension lines show up close together, either put a note on one dimension that clarifies to what feature it refers, or see 16 below.

16. Define smaller features in a scaled bubble view. Use auxillary views, section views and cut-away views to show features in a more clear manner if they might at all be questionable.

17. Dimension logically. I cannot stress this enough. Keep dimensions of a feature in one view, if possible. A machinist having to hunt all over the drawing for dimensions to a feature causes errors, frustration, and added expense. Try to apply dimensions in a logical flow of the most probable machining sequence of the part. If it is a round part with milling, put all the diameter information in one or two views, if it doesn't get cluttered or unreadable, and all the milling information in another view or two. The machinists won't be distracted by dimensions for features he isn't machining. Many times it is possible to lay out the dimensions in a manner that flows with the manufacturing progression of the part.

18. Put your direct contact information on the print, if allowed by company policy. If there are any questions, the machinist can call and clarify.

19. You can learn a great deal from the machinsts on how to make parts less expensive, if you LISTEN.

Remember: The more information you can convey quickly, clearly, and logically to the machinist on a drawing, the cheaper your parts will be.

-- Anthony