1. Tool definitions                 Author - Derek Mackenzie

This note is intended for use with Dolphin PartMaster CAD/CAM software, but most of the data and some of the comments may have general use.

The attached file gives all of my current tool parameters. All dimensions are metric – just multiply by 25.4 to get imperial equivalents. The original is available in excel format – E-mail me if you want a copy (see Contact Us page).

This is used on a modified Hobbymat lathe, but the basic tool definitions should apply to any lathe.

Tools 1, 2, 4, 8, 9, 10, 12, 14 and 15 all appear to be industry standard holders that in theory should be interchangeable – but see note below.

Tools 8, 9, 10 and 15 are tools 1, 2, 4 and 14 just turned through 90 degrees for axial turning – it is a pity that the Dolphin software can’t just turn the tool as required, but requires separate drawings for each orientation. Note the instructions for drawing a tool further down the page – things have to be done in the right order or strange results ensue. Drawings for each of these tools are available – E-mail me if you want a copy.

Tool 3 is a standard parting blade – I made my own 4-way toolpost to take 3 standard tools with the parting blade on the fourth side – again drawings are available.

Each tool acts as an end stop for the tool next to it; the tools then have spacers super-glued to their ends so that the tool tip is always the same X distance from the toolpost centre.

When you are turning an object that requires several tools, it is essential that the software knows exactly where the tool is – even a few thou out could produce noticeable errors on the transition from one tool to another.

This is done by defining turret offsets in the tool definition – the values given here can be used as a starting point – but will almost certainly require changing as I failed to drill the mounting bolt hole quite in the centre of my 4-way toolpost! Turret offsets might not have been activated in your post-processor (they weren’t in mine) – just E-mail Dolphin with a request for a modified post-processor.

It would be an advantage to have enough 4-way toolposts to keep most of your tools permanently mounted – say one for axial tools and another for radial tools.

If you going to do both axial and radial turning on a single piece of material it is essential that all tools are offset from the same place – I have used the tip of tool 1 as the master position.

I defined a turning operation to move all tools to a given position so that I could check that I have got the offsets right – mount a piece of bar in the chuck, single step the program until the tool is at the given position then measure the distance from the bar with a feeler gauge (I do one pass for the X-axis, then another for the Z) – the values can then be corrected in the tool definition (it can be a problem working out whether you should add or subtract – I get it right about 90% of the time) or you could superglue shims to the side of the tool. I have tools from several manufacturers and they vary a bit. Tool height can be checked by milling half way through a piece of rod, mounting in the chuck with the cutaway at the bottom, then move each tool under the rod and check clearance with the feeler gauge – they should all be the same (if not add shims to the bottom of the lower ones) – the clearance should be zero if you cut away exactly half the rod.

Tools 5, 6, 11, 13 and 16 are home made – tool 6 uses a junior hacksaw blade cut into small pieces to cut a 0.45mm groove.

Industry standard holders should be marked with a code such as SCLCR-1010-E06 for tools 4 and 10 – this breaks down as follows:-

S – ?
C – insert shape –	C = 80 degree diamond
	D = 55 degree diamond
	R = round (button)
	S = square
	T = triangular
	V = 35 degree diamond
	W = 80 degree almost triangular
L – holder style – I don’t know what this means!
C – insert clearance angle -	B – 5 degrees
	C – 7 degrees
	N – 0 degrees
	P – 11 degrees
R – hand -	R = right hand
	L = left hand
	N = neutral
10 – tool depth – in this case 10mm
10 – tool width – in this case 10mm
E06 - ?

Note:- these are European codes – they may not apply in USA

I have bought replacement indexable tool bits from various suppliers at various prices – the finish of the bits varies but they appear to be of a standard design

Bits can be bought with different tip radii – if you use anything other than 0.4mm radius then the following must be changed in the attached tables –

Tip radius

Z offset

X offset

Incidentally I find the different axes on lathes and mills confusing – in each case the rotating bit is the Z axis, but the lathe X axis is what you would expect to be the Y axis on a mill – I am using the same control software and box for both my lathe and my mill so I wrote a program to swap the axes on Dolphin output CNC files (I later found that it could have been done in the post processor) and the lathe control software required a different version that changed the way arcs were machined.

2. Pausing cutting for manual operations               Author - Derek Mackenzie

If you need to tap or cut a thread with a die in the middle of turning an object, you will find that Dolphin do not provide an indeterminate suspension of operations – you can do a delay for a fixed period, but the last thing you want is for the lathe to spring back into life whilst you are in the middle of a manual operation that took longer than expected. I got round this by setting up a tool called “Pause for manual operation” – the tool 7 missing from the attached list – this just homes the tool and waits for the continue command – just do whatever you need, and then hit continue.

3. Travelling steady for small diameter rods     Author - Derek Mackenzie

If you are turning small diameter pieces of any length – say less than ¼” diameter with a length diameter ratio > 6 (e.g. 1/8” diameter x ¾”) you will find that the material will bend away from the tool bit, probably snag, then break – the solution is a travelling steady bolted to the lathe saddle (not the cross-slide) with different inserts for different material diameters. Again a sample drawing is available.

In this way you can keep the material overhang to a minimum, but it is best to then machine in a single pass so that the full material diameter is supported in the insert – this will require a different approach to building up tool paths.

Note that the pausing cutting for manual operations (above) does not work if you need to use the travelling steady mentioned above, as it has just homed the tool and taken the steady too far to the right (I am assuming that home is the right hand end of the original bar material, and in my case 40mm my side of the lathe centreline). In this case I use tool 7, then add a comment in the file about what operation to do, then a comment about single stepping the next instruction, then instruct the lathe to move left to a position where the steady is clear of the required operation, then continue as normal.