The Home Machinist!

If I go conventional milling two of the side are cut going in the negative dial direction which does not allow to overshoot the target and reverse to offset the backlask.
Working always in the positive dial direction forces to climb mill on two of the sides, not desirable. Now that I think of it the mill may climb back to pich up the backslash and render the dial reading correct at least in theory.

So what is the proper procedure to mill a pocket to size counting only on the dials. I can measure the pocket for correct size but location need the ability to measured from an outside reference.

I was sinking a square pocket 0.45 x 045; 075 deep into a 0.75 dia piston.
I drilled down the four corner with a 0.098 drill, and milled a round hole in the center 7/16 and cleaned up with 3/16 end mill. I had to pull out and locate each corner working from corner to center. Lots of motions, not very efficient. I was still climb milling away from the corner.

_________________
Mauro Gaetano
in Austin TX

Mauro,
I faced that situation regularly when I was actively machining. What you do is use the dials in both directions, but you can't trust the numbers when you reverse. To help you understand what I mean, lets talk about a cross symbol +.
I let each of the ends of the cross represent the surface being machined, and I record my readings on a piece of paper, or even on the vise or table of the machine, using a wax pencil. The bottom one (6:00) and the right one (3:00), I use the dial, as the left and top side of the part are generally my reference points, so the dial reads in the positive direction. I can determine where to stop simply by calculating the position, reflecting the size of the end mill, or if it's a critical dimension, I measure, then determine the desired dial setting. In either case, the dial setting is written at the respective end of the cross.

The other two positions (9:00 and 12:00) are different. Both of them are now in the opposite direction, so you can't rely on calculations. However, they are (generally) easily measured, so I rough each, leaving material to be removed when I know where I am. I do that by reversing the handle, so I am now reading the dial in the opposite direction, with backlash eliminated. All that is left is to determine where you are in regards to the dial. What I do is either measure from the ends, or from the opposite face, which I will have already generated, so it can be used as a reference point. If you have left material for a final pass on those sides, remember to allow for the amount you left when measuring from the opposite face. Record the calculations at the respective ends of the cross. You can now rely on your dials in both directions, for backlash has been addressed. I'm sure you realize that the dial readings may not make sense in reverse, due to the amount of backlash in the screw/nut assembly, but the readings should repeat reliably.

I generally leave a few thou for a finish cut on all sides. You can then climb mill, approaching each corner without hesitation.

When cutting pockets, there's almost always a small amount of hesitation when changing directions. That often results in a minor chatter pattern in the corner, along wiht minor undercutting. You can avoid that by ever so slightly backing off the stationary handle as you approach the mark on the dial. All that is required is to unload the screw, moving the slide only a thou or two. I hope this makes sense---it works very well when you understand what to do, and when to do it.

Harold

_________________
Wise people talk because they have something to say. Fools talk because they have to say something.

Thanks, why did I not think of that.

To paraprase your instructions ...
Work the 12:00 and 3:00 sides trusting the dials with allowance for the actual mill dia. Stopping at 1:30 and 4:30. I am milling conventional and in the positive direction.
Now I have two sides to reference a measure.
Reverse the handle until the backlash is remove. Move less than full travel to leave a smaller pocket than nominal, using the dial as differential move neglecting the absolute reading. Still conventional milling.
Same for the forth side.

Now climb mill all around trusting the dial in the positive direction, measuring and adjusting in the negative direction.

_________________
Mauro Gaetano
in Austin TX

Assuming you have used the left side and top side as your reference (picked up with an edge finder), you would machine the 3:00 and 6:00 sides by direct dial reading, compensating for cutter radius. When I speak of the top side, I am making reference to the 12:00 side of the part. From your description, you would have referenced the 6:00 side, but that causes you to read the dial in reverse. Not a problem, but it can be confusing if you are not very comfortable with working dials backwards.

Correct.

Direction of travel in making the cut can be climb or conventional, considering you are machining a slot initially. Once you have opened the window, however, climb milling can be troublesome if you have a loose machine, or it is light duty. I did my finish passes by climb milling, but I would remove only a few thou, so it wasn't troublesome. Let that be the guide for your selection in the direction you prefer to feed.

The bottom line is, once you've established the relationship of the dial to the cut, you can trust the dials in either direction, because what you've done is account for the amount of backlash at that particular place on the screw. If your screw can be trusted to a thou, it will repeat within a thou.


That would be correct for both semi-finishing and finishing, assuming your machine is robust and does not yield problems with climb milling. Climb milling almost always yields a better surface.

If you have recorded the proper stopping points for each side of the window, your final pass can be one smooth movement for all four sides. There won't be any witness marks in the cut. Keep the markings where they are visible wihtout taking your eyes off the cut. That's why I often make the + on the vise, or the table, near the cut.

Harold

_________________
Wise people talk because they have something to say. Fools talk because they have to say something.

How does the finish become enhanced by climb milling?

It is the mechanical fact that the tooling pulls into the work slightly slicing off the stock, and when the cutting action stops, springs away just slightly so as not to 'rub' the bit against the stock? Is this basically what is happening, or is my understanding of the mechanics here way off?

_________________
Big Dave

Be Alert! The world needs more Lerts.

My understanding is that the contributor is that the edge enters the work at depth of cut, then thins as it exits, ejecting the chip behind the path to avoid recutting. Conventional milling starts by sliding over the surface trying to get under a bit so it can cut (pushing away till it does, causing some flex), then tosses the chip right into it's path where they often pile up and get back into the cut to gall/mark the fresh surface.

_________________
Russ
Master Floor Sweeper

I'm not sure I understand the mechanics of why climb milling yields a better finish, but, to me, it's obvious that when conventional milling, any chip that gets re-cut does so by being wedged on the already machined surface, yielding damage. In climb milling, that isn't possible.

Harold

_________________
Wise people talk because they have something to say. Fools talk because they have to say something.