How many on here use a Taig / Peatol Lathe or Mill?

[alan2525]

Since I'm a Taig Lathe owner, I just wondered how many other fellow Taig owners are on here and what kinds of work they've made with them? I've seen a few pictures with a glimpse of that familiar black anodised extruded headstock!

Also if you have a Taig Mill is it a manual or a cnc conversion?

I should be picking up my Taig Mill soon and it'd be great to find out what other peoples experience has been like with them!

Alan

 

[shred]

I've got a Taig lathe (plus an old 6" Atlas and being-rebuilt Sheldon lathes). My mill is a CNC-modified Taig which I often drive around in manual mode for simple cuts.

All the milled parts on the Small Sterling Fan and my other engines to date (Tall Vertical, Tiny, Brassy Babe) were done on the Taig, though most of the turning for the fan was done on a larger lathe since I wanted to see how it did.

 

[joe d]

Hi Alan

As you will have gathered from my answer in another thread, I too have Taig equipment, both a lathe and a mill. The mill is manual, I've not yet felt the bite of the CNC bug. (but, maybe one day...). I've had the lathe for two years, so far it has done everything I've asked of it, got the mill a little less than a year ago, and am happy with it as well.

There are obvious limitations of scale, but since my primary idea was/is model building this has not been problematical.

One future project is to add a lead screw on the lathe, I've seen two different versions of this and I like what I've seen! Some nice elf brought me a 4" rotary table for the mill at christmas, it's a good fit on this size of mill. If you're going the CNC route, you could add a stepper on a rotab and have another axis to play with :big:

Cheers, Joe

 

[gilessim]

I also have a Taig lathe that I bought on ebay a few years ago ( I paid about 100 euros here in Italy!) it was apparently unused and came with a whole bunch of bits including a 4 jaw, I later bought the Mill attachment and a collet set, I made a Stuart 10H basically just using the Taig, an old drill press and some files!. I later got a bigger chinese lathe and a small mill but I still use the Taig a lot for tiny stuff, thay are incredibly accurate!

one day I might just invest in their CNC mill, that looks fun! but not just yet!

Giles

 

[raym 11]

The Taig mill is a very stable ,accurate machine. I use mine only for very small work since I now have a 'full size' mill. I machined all the mill work on my Silver Angel with the Taig.
I see a ER-16 adapter advertised for ~$100, that would make it a better machine if it
doesn't reduce the head room.

Cons:
not enough 'z' axis head room.

needs variable drive

note: mine is an older model (R&D )

Ray

 

[alan2525]

If you're going the CNC route, you could add a stepper on a rotab and have another axis to play with :big:

Cheers, Joe

When you setup a cnc mill, I'm not sure how you'd actually set the datum or home position for the machine if it has a 4th axis or a trunnion table without the machine doing something daft and trying to mill chunks out of itself!

On my roland machine in 2.5D the drawing is drawn on a sheet which represents the machine table and then the spindle home position is simply set to the lower left corner, I assume Mach3 software for a mill conversion is basically the same.

Or would you need to use an edge finder or some such to locate the tip of the tool on the edge of the workpiece to set the datum each time?

 

[alan2525]

I've got a Taig lathe (plus an old 6" Atlas and being-rebuilt Sheldon lathes). My mill is a CNC-modified Taig which I often drive around in manual mode for simple cuts.

All the milled parts on the Small Sterling Fan and my other engines to date (Tall Vertical, Tiny, Brassy Babe) were done on the Taig, though most of the turning for the fan was done on a larger lathe since I wanted to see how it did.

How easy is it to use the cnc converted Taig in manual mode?

If I for example set up a fly cutter in the machine and wanted to take a few thou of a piece of square aluminium stock, would I be able to simply use the cnc control to set the travel on the relevant axis to take the cut, in effect using the cnc feature like a glorified power feed?

 

[John S]

Yes Alan for 'manual' jobs such as this you use what is known as MDI, which stands for Manual Data Input

Using Mach3 as an example you go the the MDI screen and type in
G01 X50 F250

Which in clearspeak means G01, do a linear move, X50, go 50 units in the + direction along the table at a feed rate of F250, ie 250 units per minute.

If you have a couple of jobs to do say a box cutout you can teach it.

Press Teach on the MDI screen then type in line by line with an enter after each line

G01 X30 F250
Y20
X0
Y0

Then end teach.

By this time it will have gone 30 units to the right, 20 units up, 30 units to the left then 20 units down to end up where it started. That program because that's what it is has been saved under the name teach.
Find it and load it up and you can cut as many as you want.

I have simplified this because I haven't taking switching the spindle on or bringing the Z down for a cut but that is the basis of CNC, it's just point to point.

John S the 3rd.

 

[alan2525]

Yes Alan for 'manual' jobs such as this you use what is known as MDI, which stands for Manual Data Input

Using Mach3 as an example you go the the MDI screen and type in
G01 X50 F250

Which in clearspeak means G01, do a linear move, X50, go 50 units in the + direction along the table at a feed rate of F250, ie 250 units per minute.

If you have a couple of jobs to do say a box cutout you can teach it.

Press Teach on the MDI screen then type in line by line with an enter after each line

G01 X30 F250
Y20
X0
Y0

Then end teach.

By this time it will have gone 30 units to the right, 20 units up, 30 units to the left then 20 units down to end up where it started. That program because that's what it is has been saved under the name teach.
Find it and load it up and you can cut as many as you want.

I have simplified this because I haven't taking switching the spindle on or bringing the Z down for a cut but that is the basis of CNC, it's just point to point.

John S the 3rd.

John,

Thanks for that. It's good to get a few pointers in the basic concepts to put it straight in my mind! I was wondering how much functionality i'd get with the mill if i converted, for doing those little straightforward manual jobs.

At the moment I use a Roland Desktop machine EGX300 and Techsoft 2D Design, in that software I basically import a DXF file and then use different colours for each tool. The tools are defined in the software and have various parameters for feedrate, cutting depth, clearance etc. I'm using 2.5D to cutout parts, drill holes, slots etc. It's basically like plotting but with a slot drill rather than a pen, in Mach 3 I assume it also supports a similar concept and generate the required G codes automatically from a dxf?

I imagine I'll be using 2.5 D for most of the parts I'm likely to make.

 

[John S]

2 - 1/2D is fine for 90% of everyday parts that are made today. People think they need to go straight into 3D but the truth is the learning curve on 3D is very steep and probably puts a lot of people off.

3D is needed for advanced projects like moulds and complex shapes but is really more for the advanced user, first you need a 3D model in CAD to start so ask yourself can I draw this? if the answer is no then learn to walk before running, you loose no experience moving up a ladder.

A quick explanation between 2D and 2 - 1/2 D.

2D is just like a flat drawing on a piece of paper, it has no thickness so it has no Z moves. Some machines like the Protrack mills based on a Bridgeport use 2D as they only have controls on the X and Y. They rely on the operator to feed the tool in manually then start the program. These are very quick for doing semi auto jobs and are cost effective in industry compared to a full 3D machine.
A typical job would be milling a pocket out to a depth of say 10mm in 2mm stages, the same program being run 5 times.

2 - 1/2D is the same as 2D but the computer controls the Z so it could do the above program without operator intervention. 2 - 1/2 D is where the machine can't move all three axis at the same time in an interpolated move. Interpolated means simultaneously moving through 2 or more curves.

Now this is where I'm going to throw a spanner in the works and get you all confused :'(

With modern controllers the difference between 2 - 1/2D and 3D is away from the machine and in the CAM side !!

Take out simple rectangular pocket 30 x 20 above, now if we get the cam package to do this 5 times going 1 unit deeper each pass it would be 2 - 1/2D because the Z move would be a move of it's own whilst the X and Y were parked.

Now if our CAM package is intelligent has has an option on it for ramping where the tool is fed into the work on a gradual ramp then because it's being fed in whilst the X and Y are moving this is actually 3D.

A simplified description but the focus is that modern controllers can do 3D but the decision to do 2 - 1/2D or 3D is made off the machine in CAM.

 

[alan2525]

John S III

Thanks again!

With my current setup the machine is capable of 3D Machining but only in lightweight materials like wood, plastic and modelling wax. I made some domes, little tank turret hatches and the tub of an F1 car using a jig and double sided milling, creating the 3D model shouldn't be a problem it's just what software to use to communicate with the machine. I wanted to upgrade to a desktop mill for working in large components from Brass and Aluminium.

Whats the support for 3D machining like in Mach 3? Would you just import as an STL file and the software calculates the toolpaths? I used Artcam with my machine to work on some 3D relief designs, the actual 3d model from these was just created from a bitmap image though. I've also seen packages like PowerMill which look impressive and undoubtedly come with an impressive price too!

I think I'll steer clear of a 4th and 5th axis for now though...otherwise I can feel my head starting to explode


Alan

 

[John S]

To do 3D you need a 3D model from some CAD package and STL file from something like Rhino will work fine.
Then this file needs to go into a CAM package like Artcam, Cut 3D from Vectric or a new one called Cambam to generate the G Code.

3D support is good in Mach, in fact Mach support is very good.
There are two forums, one on Yahoo for day to day text based problems and a web based forum at www.machsupport.com for downloads and web based forum, handy for pictures.

5th axis is mind boggling.

Whereas 4th axis is nothing to get frightened about. 4th axis is usually a rotary table mounted on it's end or a stepper driven dividing head.
In 4th axis it's usually running as 3 axis as Y doesn't move and keeps the rotab on centre line.
In fact some people take the Y axis stepper and fit it to the rotab so they still only have 3 usable axis.

Simple lesson on making a dial for a lathe or mill.

What is needed is a dial with say 50 divisions on a 2" circular blank.

First draw the scale out full size in CAD the lengths of lines need to be in the X direction, the number of the lines needs to be in the Y direction.

So we want the main marks to be 1/4" long, the 1/2 marks 3/16" long and the units 1/8" long.

IMPORTANT. The distance from the first mark to the position of the 50th mark which isn't cut is Pi x D or in this case 3.1416 x 2 = 6.2832"
The reason the program has to go to the 50th mark but not cut it is that 50 and 0 are one and the same.

Put numerals on if needed, note rotation ;D and then post process the file as normal but choose a post processor that doesn't use arcs as you can't interpolate in a rotary axis.

You then get a file that spits out loads of short line moves in X and Y, using notepad edit all the Y's for A's and load this up into Mach.

This will then engrave your dial on a 2" blank.

4th axis opens up a whole new ball game for the small engine builder.

Watch these two video's.

[ame]http://uk.youtube.com/watch?v=fps0OR1eF_s[/ame]

[ame]http://uk.youtube.com/watch?v=FkzqwIjjBhs[/ame]

First off the gears are not geometrically correct as I was just using a vee cutter and not the correct shape for the teeth. Secondly ignore the rocking about as the X3 was on a transit stand on it's way to a show and the jacks hadn't been wound down.

.

 

[Alphawolf45]

JohnS
Wow, I never read such a good simple explanation of use of a rotary 4th axis...I have two large cnc mills , niether with a 4th axis and I would had one by now cept I didnt know that programming could be as simple as exchanging Y for A......Very good, thankyoumuch, I have new project to consider now.

 

[alan2525]

It's all beginning to make sense now!

I'll probably join a couple of usergroups regarding Taig CNC and Mach 3 too when I'm nearer to start the cnc conversion. It's been really helpful to get a bit more insight in how the cnc'd mill can be used - I'm certainly liking what I'm seeing!

Alan

 

[Bill S]

I'm in the process of changing the rear cutoff tool holder I had made previously from normal blade with the lathe running in reverse to upside down, and was wondering if it would be advantageous to have positive rake on the parting tool. I did some research and couldn't find anything regarding it. The holders I have used before had no rake. Any thoughts?

Bill

 

[abraxus]

I would love to know where to get this item for
a hundred euros, I actually live near the taig
/peatol salesman's home ( a right turn, then
a left after about three hundred metres,).
When I bought my lathe and mill the cost was
nearly £2,500 and I do not use CNC. My lathe
and mill. Is. used for toolmaking for a locksmiths
business, not really for model making. It has
proved its use and reliability over three years
but I suspect that it would have been a lot
cheaper to have bought a table top lathe and
mill setup from Machine Mart that would have
done the jobs I need doing, despite what is
often written, locks are not generally close
tolerance items "Medeco" being one of only
two that I have come across that may carry that
label, ( both makes are American ), and not sold by
your local locksmith, but by bonded and high end
security institutions. The Medeco are used
by government and Buckingham palace. And
to my knowledge has only been "picked" a
couple of times once each, on both sides of
the Atlantic, the tolerances are just too
close for the average locksmith to deal with.
So much so, that when an American managed to
do it they actually made a movie, the
Scotsman who managed it does not even
advertise his services, relying on word of
mouth from clients, and is a true high security man.
even to the extent that he does not even
tell his family what it is he does for a living !
Worth the price ? For the right skill level user ,
yes !!!
For most of us ? Not really, most table top stuff would be easier
To buy/control, or get extras for ! Just too costly.