Is it possible to do a conversational programation with a mach3 lathe?

Thanks and best regards

Saumur,

Mach3 lathe does have some conversational programming in the form of what they call wizards.  There are several different ones and if you can think up new conversational programming you would like, make a suggestion and maybe someone will make them.  Users with some basic programming skills can build their own. 

I have done a couple of wizards to generate ID grooves, end groove, parabola, and some other tapers.

Arnie

I do not understand what you mean by conversational programation.

Zarzul mentions wizards - so I assume you mean short programs to do small turning jobs.

Yes - I had a lathe, CNC ready - but coukd not, as I used to on my manual lathe, sit down and do anything.

I thought about the jobs I did on my lathe.

1. I turn down a piece of bar to a smaller radius for a certain lemgth.
2. I make axles for my railway which means turning 30 mm bar down to 25mm (to fit the wheel) and 17 mm (to fit the bearing).

Both were the same job - so I wrote a Visual Basic Script - which took 20 thous (1/2mm) cuts down to the right diameter for a given length. This is macro M201, the metric version is M301.

I put additional user DRO's on a page of the Turn Screens - Start radius, First Radius, First Length, Second radius and Second length
which the program can access.

I can now fill in the DRO's and call M201 and the machine goes ahead and cuts it. I have done a similar one to round the end of a bar - given the diameter. M202 or M302.

These Macros - as well as being used on their own, can be called up in GCode programs.

If that IS NOT what you mean, then YES - Mach 3 can also have a conversation - The Vis Basic command is "Speak" - but you do need a conversational prigram in the computer already.

 

Maybe Saumur is meaning something similar to the NewFangled Solutions Addons for Mill which let you walk through wizard type pages and at the end you have the code for a complete part. Dont think this will happen with Mach but maybe someone will follow Brians lead and do one for the lathe and sell it as an addition like the NewFangled ones, any takers???

Hood

"Yes - I had a lathe, CNC ready - but coukd not, as I used to on my manual lathe, sit down and do anything."
I use version 1.84 still on my lathe. It has a nice selection of wizards in it, which work well and are easy to use. As for conversational programming, well, it's kinda what I have been asking for over the last two years, to be able to machine a part to a non standard profile, basically from  a DXF profile or similar. You can import a DXF profile but it has no real method of roughing it out unless you draw all the roughing offset lines and save them all on different layers. Those familiar with the Fanuc machines will know this as a G71 roughing, along with a G73 reentrant cycle. As I always say, I will help pay for these to be written if needed. One day....!

Yes - but where , then do you get into the realms of full scale CAD - CAM.

I do not mind posting my Macros as I write them, which can rough down, and then finish, such as axles and things on the lathe, given various parameters to start with. I would like one for the mill to cut out letters from plastic sheet - which is my next project.

We could perhaps - and someone will tell me there already is - a part of this forum where we can lodge small macro's for other people to use if they wish - it would be a great help getting started - and something for prople to build on.

I have used a Fanuc based lathe for years, and never needed anything more than the G71 roughing, G73 reentrant and G70 finish cycles, never used CAM for the lathe. I am using CAM for my Mach3 lathe now as a necessity, but it's somewhat slow to use and has more crash potential than the Fanuc cycles. Crashes on mills are usually nothing much, snap a mill off, etc, but it's a very scary thing on a lathe, heard of whole toolchanger turrets being broken off the ways and thrown into the door, etc. Nasty.
CAM seems to be written for mostly mill work, and is often neglected in functionality for the lathe, even though it would seem to be simple for the CAM software writers, it's only 2D after all!

I am interested in this. I have just used Solidworks to do a part, but when I look at the GCode, I can remove big chunks of it and get the same result. This was for the mill, and the lathe is even simpler to program manually.

When you say you have used Fanuc roughing - how does it work - i.e. what does it do. It must clearly have a start radius and a finish radius for the workpiece, and, I assume you can specify the depth of cut - but how does it follow the profile i.e. how do you tell the machine what the finished profile is?

Given all that I can write a macro for roughing. I have one or too now, but they are limited to simple bar stock. If I knew how the profiles were described that would help.

Here is one for the axles I mentioned above. It roughs a bar down to a size, and puts a finished diameter on - two different diameters - for making railway axles.
It is in inches - although it only makes a difference to the depth of cut - set at 20 thou. I could have put a larger depth of cut, or even another variable in to specify the depth of cut (which would satisfy both imperial and metric users.)

The macro - named M301 - requires several user DROs - which I have put on the manual page of Mach3 Turn. It can be called from within a GCode program or just run as a standalone by entering M301 manually. X0 is the centreline of the lathe, Z0 is the business end of the workpiece.User DRO's are persistant, and return when the computer is restarted - so check each time before you use. Download to your Macro folder.

Please try it. BE CAREFUL, HOWEVER -  This particular version has not been tested. I am in the process of putting new limits on my lathe, and this version is on my office computer. I write them here, and then transfer them to my workshop computer, where any last minute bugs are ironed out.

Here's some code to machine a part. Rapid to the clearance of thw workpiece. You call out the G71, first line is the roughing depth of cut. Second G71 line, P60 is the first line of the part profile, Q160 is the last and the U and the W are how much material to leave on the part to be finished later, and the feedrate is the F of course. Then, just write the G code of the profile start to finish. It will rough down to this profile, leaving the stock there you called out for, and then return to the start rapid in point when done. Then rapid away, call out a toolchange to the finishing tool, rapid in again and use G70 to call that same section of G code to finish, all in one line. Rapid away again and you're done. So, no need to use any CAM at all, the G71 will do it for you and the G70 finishes it using the same piece of called out code. If you think about it, it's really only like a pocket clearance program for a mill, but you don't clear one corner of it out, the rapid in point.
%
:2008
N10 G20 G95 G97 G42 M03 S750
N20 T0101
N30 G00 X3.3 Z.05 M08
N40 G71 U.06
N50 G71 P60 Q160 U.01 W.005 F.005
N60 G00 X0
N70 G01 Z0
N80 X1.485 R.08
N90 Z-1.48 R.08
N100 X1.813 R.08
N110 Z-2.2638 R.08
N120 X2.249 C.02
N130 Z-2.39
N140 X3 C.02
N150 Z-2.55
N160 X3.3
N170 G00 X4 Z4 M09
N180 T0 M01
N190 T0202
N200 G00 X3.3 Z.05 M08
N210 G70 P60 Q160 F.003
N220 G00 X4 Z5 M09
N230 M30
%

That's great - about the biggest jump forward I've taken for a long time.

Are you saying that G70 and G71 are implemented in Mach 3.  I take it you start the job with the tool set to the bar stock diameter.

It beats my effort into a cocked hat.