Order of Operations

I think some orders of operation are almost always fixed, like rough all over before finishing might be one example. Others depend on the particular part like the form tapping example that you gave.

Best, Steve

Steve:

You're right, some operations ARE always fixed. You have to drill a hole before reaming or tapping it. But roughing all features before finishing any, is not universally set in stone. If someone were milling a series of very thin walled pockets, one pocket might be finished to size (and then possibly filled with a fusible alloy or an aluminum plug), before finishing an adjacent pocket sharing a thin wall.

Yeah. I always like to drill first, and then tap. Just a personal preference, I guess.

A lot of how you process work depends on whether you're doing onesy-twosies, or low volume jobbing, or higher volume production. For the lower numbers, setup costs are major. Having a set, automatic, everybody knows how to do it kind of processing scheme for standard part features can save a lot of time. In shops that do one and two piece special stuff, processing often depends on what you have on hand to hold the work and to cut it. Higher volumes, though, can justify extra costs for tooling, fixturing, and for planning and perfecting processes.

Families of similar parts are important, too. The process may be just right for family member A; but barely capable for member B. But limping through B might still be cheaper and faster than doing two complete programs and setups.

Obviously, the examples of bulges from form taps are quality issues (or hand-finishing requirements) that need care and attention. But maybe you could save hours of reworking a job just by switching drill sizes and using a cutting tap, even if forming is what you'd prefer.

There are too many variables. That's why, even in an age of CNC machines smarter than most of my inlaws, the skill and judgement of good machinists are what make the difference between success and failure.

KG

good point. Say yu had 3 pockets with thin walls. You might machine rough/finish the outer ones and then do the middle one last, then you only have to deal with the thin ribs on one pocket instead of three. or you might rough/finish each pocket in z levels 3 pockets at a time. Or in electrodes, you might finish a pocket, then rough the pocket out. so when your cutting the pocket its in solid graphite, then removing the inner later without hurting the walls...

Vinny:

Also an excellent idea.

I always try to machine parts so that if ther is any filing/beburring to do it is easy to get to! Is much better when the parts come out finished - why should I do it when the machine can :)

Reuben:

That's a good point. On vertical outer perimeter sharp corners I tend to program a .005-.010 radius edge break to keep the tool in contact with the work (unless the print, or function, NEEDS it to be dead sharp). If allowed, a small chamfer made with a spot drill or 45 degree carbide chamfer tool used on the upper edges/pocket-walls can make deburring less painful. There are many brands of abrasive nylon brush systems that can be used to CNC deburr while the part is sill in the machine. Top surfaces, large holes, and small features below the surface can all sometimes be gotten to. One example follows.

One drawback to abrasive deburring on the machine, is that fine abrasives can sometimes get into the coolant, so an extra and finer filter may be recommended if you do a lot of that sort of thing.

One of my guys has decided that he wants to learn how to program using our CAD/CAM (Edgecam). After a few days of working his way thru it, he made the comment, "Damn, you really have to think about every friggin' detail before you start!" He's been at it for less than a week and has written 3 or 4 good programs. I think he'll be alright.

"Damn, you really have to think about every friggin' detail before you start!"

Alphonso:

Isn't THAT the truth. I think that's one of the major differences between manual machining and CNC machining. You have to visualize the complete machining process from start to finish, so you don't paint yourself into to a corner.