My job is to prepare and set up the machine, write and proof-run the program, deburr the workpieces and give them to the customer. So my process is, write the program, run it and improve it after each iteration until it runs perfectly with as little need for deburring as possible. Those improvements and fine-tunings happen at the machine. Sharp chamfer? Need some radius. Chatter? Have to change feeds/speeds. Taper? Need to compensate for. Saying that edits at the machine are not needed is IMO pure fantasy in a job-shop environment where you have to deal with crappy machines with crooked turrets and misaligned tailstocks and use the sparse tools and inserts that are available. However, if I someday get promoted to a programmer-only position, my opinions may change

Here's an example (comments removed): T909 G55 G96S220M3 G0Z5M8 G0X70Z-82.85 G1X33.2F0.2 U2W1 G0Z-30.85 G1X23.2 U2W1 G0Z-27.486 X22.828 G1G42X20.Z-28.9F.2 Z-29.4 G2X20.876Z-30.5R1.6 X23.2Z-31.R1.6 G1X29.517 G3X29.659Z-31.029R.1 G1X29.941Z-31.171 G3X30.Z-31.241R.1F0.08 G1U0.2W-1F0.2 G1G40X32.828Z-29.827 G0Z-79.986 G1G42X30.Z-81.4 G2X30.876Z-82.5R1.6 X33.2Z-83.R1.6 G1X66.987 G3X67.18Z-83.074R.1F0.08 G1X69.813Z-87.987F0.2 G1U0.5W-1 G0G40X300Z10M9 M1 Using incremental values ensures that the lead out is always the same, if/when a need arises to edit the code, less margin for error or too long a lead-out. And it is also easier to spot (the line "G1G40X32.828Z-29.827" is mastercam-generated lead-out)

No problem. It's just more convenient when modifying programs at the machine. I always use U2W1 or similar as a lead-out when typing programs by hand and would like Matercam to honor this tradition.

This is the mplmaster template, with only small modifications...

Lathe

I'd like my post to output the lead out movement as an incremental move (U/W). Can the lead-out movement be recognized somehow inside the post?

I can think of two ways. Add an invisible character (eg ALT+255) as a line in your manual entry. Your control or DNC file transfer may or may not filter it out. Or, modify your post so that certain strings represent an empty line in the code. For example, if you used the word "SPACE" as an empty string, the post would look like this in the pcomment2 section: if gcode$ = 1006, #Manual entry - as code [ if scomm$ = "SPACE", " ", e$ else, scomm$, e$ ]

Does this version finally have the modern Windows 7 style file open and save dialogs that show desktop, favorites etc in the left pane? I really, really miss those.

What if you change default active spindle to "right"? Does the spindle direction change and everything else stay the same?

I hope in some future version "Quick verify" option in backplot would work in Lathe just like it does in Mill. That is, the insert would leave gray trails. "Use a stock" would be a response to my wishes. But hey... it works in Mill even when you don't define stock!!!

I thought virtual Y axis means controlling X and C so that you enter X as X and Y as C and the control converts them to polar coordinates X and C.

SAR will only affect that when the spindle is turned on, it will move after the spindle has arrived at full speed. Disabling SAR is useful when turning long shafts etc that tend to resonate, you can command S on short G1 intervals without ruining the surface finish..

I think Mastercam re-tessellates the geometric shapes after saving. When saving while wireframed, it is faster, but turning back to shaded there is a slight delay. And vice versa. Do you notice the same?

If it was 32bit, it would say * 32 in the list of active processes inside task manager.

I can give you an example after the weekend, but the code is Fanuc-specific.

Yes, you need to change the lead-in and lead-out angles to get that sort of thread start/end on the control. Can you use live tooling to mill it? Mastercam has multiaxis toolpaths for this if you have the 3D model...

It's not possible to turn a custom profile with Mastercam "by default". It can be done, but requires heavy post-processor modifications especially done for this kind of thread turning. I do it by hand using controlled threading G32 with Mastercam to get the threading cycle start points for a grooving tool. It's just easiest to buy the appropriate insert or grind it. Oh and btw, welcome to the forum

It was really well hidden I must have gone through those menu items gazillion times.

There should definitely be a shortcut for "Invert selection"..

Do you mean "Repaired NCI?" I get those every now and then. What does it actually mean and why is the operation locked? It doesn't fortunately seem to affect the operation parameters.

I always define the second Q parameter larger than the first so that the first cuts take more until the minimum depth of cut is reached. Q100/Q500 works quite well and saves a lot of time as well in larger threads... the manufacturer (Sandvik does this) may have labeled the recommended number of passes in the box of inserts.

If you know the starting points of the lines and their angles, you need a ray-ray intersection macro. The angles must be converted to direction vectors first. The math: http://stackoverflow.com/questions/2931573/determining-if-two-rays-intersect Example: First point p1=(X10,Y10), angle=240 Second point p2=(X5,-Y10), angle=90 240 degrees direction vector d1=(cos(240),sin(240))=(X-0.5,Y-0.866) 90 degrees direction vector d2=(cos(90),sin(90))=(X0,Y1) The first ray p1+x1*d1 The second ray is p2+x2*d2 The intersection is where p1+x1*d1=p2+x2*d2 p1.x+x1*d1.x=p2.x*x2+d2.x p1.y+x1*d1.y=p2.y*x2+d2.y you will finally get => x1=((p2.y-p1.y)*d2.x-(p2.x-p1.x)*d2.y)/(d2.x*d1.y-d2.y*d1.x)=10 x2=((p2.y-p1.y)*d1.x-(p2.x-p1.x)*d1.y)/(d2.x*d1.y-d2.y*d1.x)=11.34 When you plug these x1 and x2 into the first and second ray formulas, you will get the intersection point at (X5,Y1.34). Of course, the macro should check that they intersect at all (x1 and x2 positive) and they are not parallel (division by zero). Happy writing

Fanuc indeed does not support specifying angles in linear interpolation, as far as I know, like Siemens does (our controls support chamfer and radius, but naturally they are options...like everything else in Fanuc...) You have to use trigonometry, and in this case, the TAN macro B function. It's nothing but elementary school math

Dunno about A-axis, but I'm assuming you meant C-axis. (A in some cases refer to a live tool aligned with X-axis) Are you trying to do face contouring? You should check if the control supports G12.1 and G13.1. With it, you can enter Y-coordinates using the C register and what's best, G41 and G42 works in that mode!

Everyone has a preference Indeed, adding a line in the lead-in is a way to circumvent the undercutting problem G42 G0 G54 X26. Z2. G1 Z0. X30. G3 X40. Z-5. K-5. G1 Z-20. G40 X44. Also, adding a line in the lead-out is needed to avoid overcutting when G40 is read. G42 G0 G54 X26. Z2. G1 Z0. X30. G3 X40. Z-5. K-5. G1 Z-20. X44. <- added line G40 X46.828 Z-18.586 In our Fanuc controls, its possible to define a vector using I and K to continue the "imaginary" profile to avoid overcutting. I don't know of any post that does it, but it could be implemented easily with misc variables.. G42 G0 G54 X26. Z2. G1 Z0. X30. G3 X40. Z-5. K-5. G1 Z-20. G40 X44. I1 <- prevent Z overcut