Hints and tips of the trade.

In the machining world, we sometimes have to improvise in order to complete a job. For this topic we'll look at some of the things that machinists do to accomplish a task at hand. Perhaps these tips can help you out when you find yourself in a bind.

Finding the axial centerline on a lathe...

There are two ways of finding the axial centerline on a lathe.

If the tool you're setting up is static (non-rotating), use a Deltronic pin in the tool holder position and clamp an indicator into the spindle collet. A 0.0001 resolution indicator is best for this application. Bring down the Deltronic pin in 'X' and roughly center it to the spindle. Using the indicator clamped in the spindle, gently swing the indicator around the Deltronic pin until the indicator shows little or no movement on the dial. The 'X' axis value for this tool position can now be set in the controller.

If you're setting up a 'live' tool, clamp a Deltronic pin in the lathe spindle collet and the indicator (0.0001 resolution) into the live tooling position. Bring down the indicator to the Deltronic pin and sweep the pin by turning the live tool holder. Once you've found centerline by fine tuning in (in tenths) 'X', set the 'X' value in the controller.

*Be sure you enter the correct 'X' axis value for the tool position and turret you're finding center for. Multi-turrent/ multi-spindle CNC lathes have several repetitive axes (X1, X2, X3) and different work offset locations (G53, G54, etc.). Setting the wrong 'X' value location can result in 'crashing' the machine tool.

Finding the radial centerline on a lathe...

*This is critical when setting up a multi-axis lathe.

Setting the radial axis (diameter) is easily accomplished by inserting an indicator (0.0001 is the indicator resolution I like to use) into the tool holder in the turret position you want to locate.

Assuming the lathe spindle is within normal working tolerance, chuck a precision mandrel into the spindle collet. I've found a mandrel that is at least 8 inches long, with a diameter of 1 inch, works perfectly. It is also useful in aligning the sub-spindle on dual spindle lathes.

Bring down the indicator in 'X' towards the mandrel until it gently rests on the apex of the mandrel diameter. Zero out the indicator and indicate the opposite side of the mandrel. Determine the difference between the two sides. You will need to adjust the turret to reflect half of the value of the runout. Make minute adjustments to the radial alignment by 'dialing in' or 'clocking' the turret axis (can be designated differently depending upon the make and model of the machine tool).

Once you've made sure that the turret is perfectly perpendicular to the spindle, set the new axis value in the controller. Its always a good practice to write down all axis values prior to editing them.

2nd op collets.

One of the primary concerns of machining is the ability to quickly and accurately make parts. Every effort should be made to reduce cycle times and set-ups. To that end, we will discuss the machining of what is referred to as '2nd op collets'. A 2nd op collet is nothing more than a specially created bushing that allows for the quick set-up of the second operation of a part. The concept is that, if possible, the 2nd op collet is made to the same diameter of the bar stock used in the first operation. This does away with the need to change out the primary collet of the collet chuck. The 2nd op collet should be machined before the set-up of the first operation. The 2nd op collet should have a flange larger than the part diameter so it will not get pushed back into the lathe collet chuck and it should have a step inside of the 2nd op collet to position the part at the appropriate position for machining.

Yes, it does add time to the initial machining of the part, but in the long run it will shorten the machine cycle time considerably. Subsequent set-ups of this part will now be done in minutes with only the 'Z' having to be touched off after the first operation. Be sure to mark the new 2nd op collet with the part number and store it away in a tooling kit for that part. If you find yourself constantly making parts that have the same diameters, you may want to consider making a set of 2nd op collets that may be used on several different jobs.

How to bore your lathe jaws correctly.

Boring the jaws on a lathe is just as important as machining the part. Two things to consider before you bore the jaws. One, size/shape of the area that the newly bored jaws will grasp… and two, how tightly you’ll need to hold the part while machining.

If the part is very small, and the thickness is less than one inch that you want to clamp on, you’ll need to consider boring the jaws with a taper in the Z axis. This will allow the part to be ‘sucked’ in to the jaws instead of squeezing out. If the part is larger and has some weight, you may need to bore the jaws slightly undersized. Typically you would bore the jaws about .003 to .005 under the diameter of the OD of your part blank. The theory behind this approach is that if you bore the jaws to size, you will only have three points of contact with the material. Boring undersized, you’ll obtain six points of contact, thus exerting greater clamping pressure onto the material.

CNC lathe machine warm up cycle.

This is a sample warm-up cycle for a Haas lathe.

%
O12345 (WARM UP PROGRAM)
(Haas SL-10)
(16 SEPT 2005)
G20
G00 T101
G97 S700 M03
G50 S2000
G96 S700
T202
T303
T404
T505
T606
T707
T808
T909
T1010
T1111
T1212
T101
S1200
T505
T202
T606
T303
T707
S600
T404
T808
T505
T909
T606
T1010
T101
T1111
T303
T1212
S1600
T202
T303
T404
T505
T606
T707
T808
T909
T1010
T1111
T1212
T101
S200
T505
T202
T606
T303
T707
S1800
T404
T808
T505
T909
T606
T1010
T101
T1111
T303
T1212
M99
%

As always, make sure the lathe turret is clear of the chuck before running this program.

CNC milling machine warm up cycle.

Here's a quick CNC mill warm up cycle to use when first turning it on.

%
O90000 (MACHINE WARM-UP)
(HAAS VF-2)
(11 MARCH 2005)
N100
S2500 M03
G01 X0 Y0 F20.
G01 X-10. Y-6.
G01 X10. Y-6.
S3500 M03
G01 X10. Y6.
G01 X-10. Y6.
S3000 M03
G01 X0 Y0
G01 X-10. Y-6. F10.
G01 X10. Y6.
G01 X-10. Y-6.
G01 X10. Y6.
S4000 M03
G01 X0 Y0 F20
G01 X-10. Y-6.
G01 X10. Y-6.
S3500 M03
G01 X10. Y6.
G01 X-10. Y6.
G01 X0 Y0
G01 X-10. Y-6. F10.
G01 X10. Y6.
S2500 M03
G01 X10. Y-6.
G01 X-10. Y6.
G01 X0 Y0
N200
M30
%

I usually would run this without a tool loaded in the spindle. Safety first!

Finding the centerline.

This works well with manual lathes. No need to go out and buy some fancy, expensive gadget with a level bubble on it to make your life easy. A lot of times a manual lathe machinist is loading tools and setting up for new jobs. This requires centering turning tools that may have a different centerline than the previous tool loaded in the same holder. An easy way to dial in your centerline quickly is to use a scale. Place the scale gently between the cutter and the OD of the stock you're setting up to cut. Check it visually for perpendicularity to the stock. The scale should form roughly a 90 degree angle to the stock. Fine tuning the tool height is then easily accomplished by taking a skin cut across the face of the stock and measuring the 'tit' left behind. Adjust the tool height as necessary.

Using the controller to measure a part.

I've been there and I'm betting many of you machinists have too. How do you measure a part while its still in the machine? You cannot take it out or you'll lose your location, resulting in the part being out of concentricity, parallel, true position, or worse... scrapping the part out all together. Here's a simple technique that is applicable to CNC mills as well as CNC lathes. Using your indicator (I always use one that reads in tenths), attach it to the front of the turret in the lathe or the spindle of the mill. Position the indicator up to one of the linear surfaces you want to measure... ID or OD. Zero out your indicator and write down the Z value displayed on the controller. Now, jog the indicator to the 2nd position you want to know the Z value... writing the value beneath the first. Subtracting one from the other, you'll find the value between the two. Simple, yet effective.