Mach3 Professional Turn


Please consider this as a quick “get started” guide and not as reference manual.
N.B. References to tooltable are not yet operational.

All the following assumes a lathe with a FRONT toolpost, quick change toolholders, chuck to the operator’s left, operator stood in front of the machine.

Z goes positive as it moves AWAY from the chuck
X goes positive as it moves TOWARDS the operator

X0 - is always on the centreline of the work.
Z0 - can be anywhere, but is usually the point on the stock where the finished job is parted off. This is usually far enough in front of the chuck so the parting tool and holder don't hit the chuck jaws.

If the job has a boring or internal threading operation only, Z0 could well be inside the chuck!! It could also be inside the chuck if only part of the outside is being turned. i.e. If the job is 50mm long and only 20mm needs working on you could chuck the job with only 30mm sticking out.


SETTING UP LATHE SPECIFIC PARAMETERS

Decide whether you want to use Radius or Diameter mode. This is set in Config/Ports and Pins/Turn Options. N.B. ensure you do not run Radius mode Gcode in Diameter mode or vice versa. There is no G or M code to change this – it is a machine setting. 

The only things that change in Radius/Diameter post processors are X linear moves.  G2/G3 arc moves are just as in Radius Mode!!


SETTING UP TOOTABLE AND TOOL OFFSETS

(Assumes you are using individual quick change holders for each tool and indexable tips)

Make sure all tools are correctly set for centre height.

Decide on tool numbers for each tool, start at 1 with most commonly used tool and go to least used. Write the number on each holder with a permanent marker. It's also a good idea to initially note the following measurements on paper, keep the paper record safe for future reference! 

Tool 1 is going to be our "master tool" and all others compared against it.

Go to Manual screen 

Set a slow jog rate and a suitable spindle speed using the relevant arrows.   

Make sure Jog is enabled 

Jog tool forwards and right far enough to allow loading stock and clear tool1.

Insert some scrap stock about 25mm dia. and 40mm long.

Insert tool1, start spindle 

Take a facing cut, zero Z axis DRO  

Then take a cut along the stock and zero X axis DRO 

Switch off spindle 

Do NOT touch Zero DRO buttons again until all tool offsets have been determined and noted down!

Jog clear of stock.

Insert tool 2, jog slowly in until it just touches the face of your newly turned stock, note down Z reading (it may, or may not, be a negative number) move and just touch outside diameter make a note of X axis reading. 

Repeat this for all tools.

For threading tools align the point, by eye with the corner of the stock, for left hand tools and parting tools, hold a flat piece of metal across the end face and line up against the edge of that - ensure the edge of the tip is exactly in line with Z face.

For internal tools again line up tip with a flat piece of metal held against the outside of the stock to ensure tip is exactly in line with X outside diameter. 

If you use drills or reamers from a toolpost holder or chuck  insert centre drill in holder and get Z reading as normal, then touch off side of drill against stock, note X reading then subtract RADIUS of drill. That is the X offset. Do not try and centre drill on stock ;)

Open tooltable  

Enter all values and tool descriptions, make sure to save it.

Another good check is remove stock and stand a block of wood on bed, align corner with tool tip, make sure correct tool number is entered and jog away some distance in X & Z then in MDI type G1 X0, Z0 then press return key and see if tool goes to the corner of wood - if it does, great. Try this using other tools making sure to enter their tool number. If the block is still on the bed - this should increase confidence greatly <G>. 

Once you've done this procedure try not to remove the tool from its holder. You'll have to reset its table entries if you do.

You will probably have to tweak these values very slightly in use, some will cut under or oversized and tip wear will creep in. This can even be done “mid-job”. 

Pause job using Feed Hold 

Stop spindle and coolant and measure work diameter, compare to what last line completed says for X. (Z can be done in a similar way if you have a reference to measure to, a shoulder on the job maybe.)

Select Tool Adjust  

And increase or decrease values as necessary

Restart spindle, coolant and press 

Don’t forget -  a .001 adjustment on tool will remove or add .002 to work diameter!!

If your machine doesn't have a fixed tool change position, to save time, set this just far enough away from the stock to enable you to change to the longest tool you are going to use on that job - Always go further than the distance it takes for the tool to accelerate to its set federate!


SETTING UP A JOB

Insert tool1 (see Setting up tooltables)

Open Mach3, select Auto  

Make sure Jog is enabled and fast jog tool far enough right and forward to allow stock to be loaded. Make sure enough is sticking out so job can be completed, if possible, without removing again.

Set slow jog to controllable speed.

It's normal to take a small facing cut and clean up cut along the diameter to enable the touch off to be done accurately. 
For ultimate accuracy, the zeroing can be done as the cuts are made!!

Touch tool against end of stock, then ZERO Z Axis

Touch tool against diameter of stock, then ZERO X Axis

Jog away a little and enter G1 X0 Z0 in MDI, tool should go to front corner of stock.

DO NOT MOVE TOOL if it is correct.

You can now enter work offsets – in Radius Mode measure diameter of stock then half it. In Diameter Mode note the actual value.

Enter this value in X part zeroing DRO then press return, Z work offset is normally length of finished job. Enter this value in Z part Zeroing DRO 

Press  Part Zero 

for example - your finished job is 20mm diameter, 30mm long. Your stock is 25mm diameter and 40mm is clear of the chuck.

In Radius Mode your DRO's should read X12.5 Z30
In Diameter Mode your DRO’s should read X25 Z30
NB - Z value NOT 40 !! You have set Z0 10mm in front of the chuck in this case. 

If everything looks good load your Gcode using 

Press CYCLE 

This will take you to the Cycle Screen

Check display and indicators if all look OK then, recheck, and only then ..

Press 

Your job should run.

There are a few things to think about. Always try and make sure your part Z0 is clear of the chuck. Initially – if using CAM, it's a good thing to draw your part slightly long (chucking piece) if you are parting off, make sure left hand side of parting tool and holder will clear chuck jaws. You can dispense with this “chucking piece” when you get more confident.

It’s always a good idea to dry run new Gcode with no stock just to make sure everything is as you expect and hover over the stop button just in case !

Don’t Forget - NO loose clothing and ALWAYS wear eye protection and be safe!!!

Steve Blackmore - Oct 04
