Mitsubishi have a 3 flute ball nose tools with all 3 flutes to center (some of the other Japanese manufacturers do too IIRC). http://www.mitsubishicarbide.com/application/files/2614/4643/8971/b059g.pdf Most 3 flutes have 1 tooth to center and 2 that are relieved. For 4 flutes they are generally 2 to center and 2 relived. I asked Mitsubishi to consider making a 6 flute ball with 3 to center and 3 relieved (still waiting, haha). The zero SFM is only a problem with ball cutters. For bull nose (and square) tools tilting the tool gives the effect of a much larger radius on the bottom of the tool. This is called Sturtz milling or P-Milling. Figure 13 in the image below shows it quite well. While the image shows the tool being tilted if you machine a slope in a 3-axis setup then you are getting the same effect

Easy picks would be the Makino or Yasda. From spending some time in Europe though I would suggest Kern. http://www.kern-microtechnik.com/en/home/ Ridiculously accurate machine and a small foot print. Maybe look at the Evo or Pyramid Nano (interesting looking machine too). If you're not doing micro work now then get ready for calculation times to go through the roof due to having to use very small tolerances as well as actual program size going up. It's funny but the smaller the part you are cutting the bigger the actual size of the NC program

^ This. +1000000 (plus a lot more zeros) Buying cheap is generally a false economy whether it is tools or software or machines, you might initially save some expenditure but you will lose out in the long term on what revenue you could have generated with the higher initial investment. Cheap actually has more potential risk attached to it in terms of costing your business money then buying expensive. The biggest mistake I see so many shops make is trying to save money rather than looking at ways to make more money.

Each 3+2 position has 2 possible solutions so your post might have some A-axis restrictions so that it will only choose the A- option. Not sure if MachSim has the same possibility to set axis limits but that if it does then that would be one way to ensure that the simulation matches the output.

I am wary of tooling suppliers showing +0 -(something) tolerances for their cutting tools. The reason being that ground carbide rod is typically supplied to h6 tolerance which is +0 -(something) tolerance. In my opinion that means that to ensure that the edge is correctly ground (and is not left as the same diameter as the shank and potentially not sharp) then the maximum cutting diameter needs to be less than the minimum shank diameter. So realistically the tool should have a -/- tolerance. For example a 1/2" tool will have a tolerance (h6) on the shank of 0.5-0.4996 (if my math is correct to 4 decimal places). So the cutting portion needs to have maximum diameter of less than 0.4996. Seco, among others, list the diameter tolerance of their tools as e8 which is -/- tolerance. A bit more realistic as far as I'm concerned.

I think what a lot of people don't realize about Vericut is that it is essentially a second post processor that needs to be set up correctly. Yes, it does read the posted NC code but how does Vericut know what the G and M codes are? It has to be told what they mean so it can interpret them into internal Vericut commands. So the information flow is: internal CAM data > post > NC code > vericut control/machine definition (vericut post) > internal Vericut code I've seen some potentially serious collisions not caught by Vericut because it wasn't configured correctly. So of course time is spent configuring it correctly rather than correcting the original post. Of course, I will say that it has other options like stock compare and an understanding of the machine kinematics better than most CAM systems (and some companies insist on third party verification of NC code which is BS in my opinion) but effectively it is a band-aid over lacking functionality in CAM software.

I would also say to try to PowerSHAPE, they appear to have a nice mix of solid, surface and triangle mesh (stl) tools. I found some videos on this page that look interesting http://www.delcam.tv/ps2014/LZ/EN/whats-new-r2.html

I remembered reading something about this and Delcam being involved in this a while back. Googling gave me the following links, maybe its's more what you're looking for? http://www.delcamconsulting.com/adaptive-manufacturing/adaptive-machining.asp http://www.delcam.com/news/press_article.asp?releaseId=1664#.UupYx7tdXh4 http://www.delcam.com/languages/de/news/press_article.asp?releaseId=1459

I would look at using a 5/8" (or 16mm) tool for that. The problem with a 20mm tool would be that it is too close to the slot width so to keep the engagement angle down (and heat) you would have to reduce your step over. But too small a step over and then the heat becomes an issue because on hi-temp alloys it's best to keep a good chip thickness (which I'm sure you know already). Also I've found that it is best to keep this type of toolpath to a maximum depth of 1.5 x tool diameter so 16mm just fits with that (little bit over I know). 5%-10% stepover, I'd start at 5% and see what the cycle time vs. tool life analysis comes out at. Mitsubishi, Jabro or Hanita (in that order) are the tools for this in my opinion. And as high pressure a coolant flow as you can get on it, seriously the higher the better.

I think you're making this harder than it needs to be to be honest. Just probe either side of the boss at the A0 position (the left hand picture on your screenshot) along the X axis at the same Y and Z positions. These 2 X-axis values should be equal if the boss was situated in the right place, so just halve the difference and use that to trig out the angular adjustment required using a macro. Hope that helps.

OK, so to expand on what I wrote earlier. To use the EasySet macro in a program you'll have to deal with all the positioning moves yourself. So try something like this (I've assumed that you've positioned on the bottom left hand corner of a square block): === (Jog Probe to .25 above corner you wish to probe) #1 = 0.5 (X PROBE POSITION RELATIVE TO START POSITION) #2 = 0.5 ( Y PROBE POSITION RELATIVE TO START POSITION) #3 = 0.1 (Z DEPTH FOR XY PROBING) #4 = 0.0 (Z VALUE FOR PROBED SURFACE) #5 = 1 (WORK OFFSET, 1 = G54, ETC) #6 = 0.1 (CLEARANCE VALUE BEFORE PROBING XY EDGE) (***PROBE Z FIRST USING XY POSITIONS***) #10 = #5021 + #1 (TARGET X POSITION) #11 = #5022 + #2 (TARGET Y POSITION) G91 G31 X#1 Y#2 F100 (MOVE XY USING SKIP SIGNAL) IF[[#5021 NE #10] OR [#5022 NE #11]] GOTO 10 (DIDN'T GET TO TARGET POSITION, SKIP SIGNAL TRIGGERED - COLLISION) G170 Z#4 S#5 (PROBE Z SURFACE) (***PROBE X EDGE***) #10 = #5021 - #1 - #6 (TARGET X POSITION) #11 = #5022 (TARGET Y POSITION) G91 G31 X-[#1 + #6] Y0.0 F100 (MOVE TO POSITION IN X) IF[[#5021 NE #10] OR [#5022 NE #11]] GOTO 10 (DIDN'T GET TO TARGET POSITION, SKIP SIGNAL TRIGGERED - COLLISION) (MOVE TO DEPTH IN Z) #12 = #5023 - 0.25 - #3 (TARGET Z, ASSUMING WE ARE ACTUALLY 0.25 ABOVE THE PART) G91 G31 Z-[#3 + 0.25] F100 IF[#5023 NE #12 ] GOTO 10 (DIDN'T GET TO TARGET POSITION, SKIP SIGNAL TRIGGERED - COLLISION) G170 X0 S#5 (PROBE X EDGE) (***PROBE Y EDGE***) #12 = #5023 + 0.25 + #3 (TARGET Z CLEARANCE PLANE) G91 G31 Z[#3 + 0.25] F100 IF[#5023 NE #12] GOTO 10 (DIDN'T GET TO TARGET POSITION, SKIP SIGNAL TRIGGERED - COLLISION) (MOVE TO PROBE Y POSITION) #10 = #5021 + #1 + #6 (TARGET X POSITION) #11 = #5022 - #2 - #6 (TARGET Y POSITION) G91 G31 X[#1 + #6] Y-[#2 + #6] F100 IF[[#5021 NE #10] OR [#5022 NE #11]] GOTO 10 (DIDN'T GET TO TARGET POSITION, SKIP SIGNAL TRIGGERED - COLLISION) (MOVE TO DEPTH IN Z) #12 = #5023 - 0.25 - #3 (TARGET Z, ASSUMING WE ARE ACTUALLY 0.25 ABOVE THE PART) G91 G31 Z-[#3 + 0.25] F100 IF[#5023 NE #12 ] GOTO 10 (DIDN'T GET TO TARGET POSITION, SKIP SIGNAL TRIGGERED - COLLISION) G170 Y0 S#5 (PROBE Y EDGE) (***MOVE BACK TO WHERE WE STARTED***) #12 = #5023 + 0.25 + #3 (TARGET Z CLEARANCE PLANE) G91 G31 Z[#3 + 0.25] F100 IF[#5023 NE #12] GOTO 10 (DIDN'T GET TO TARGET POSITION, SKIP SIGNAL TRIGGERED - COLLISION) #10 = #5021 - #1 (TARGET X POSITION) #11 = #5022 + #6 (TARGET Y POSITION) G91 G31 X-[#1] Y#6 F100 IF[[#5021 NE #10] OR [#5022 NE #11]] GOTO 10 (DIDN'T GET TO TARGET POSITION, SKIP SIGNAL TRIGGERED - COLLISION) M30 N10 #3000 = 1 (PROBE COLLISION DETECTED IN MOVE) M30 === Couple of points: 1. I"ve not taken into account turning the probe ON/OFF. Check your probe documentation on how to do this in code (M75/76/78/79?). I wrote this from memory so haven't run it on a machine. 2. I'd look at using the XY values to dictate which corner of the block we're probing X+Y+ = bottom left X-Y+ = bottom right X+Y- = top left X-Y- = top right You'll have to check my syntax above to make sure the moves will be correct regardless of negative or positive value. 3. I'd also look at wrapping it all up in a custom macro call. EG. G555 C0.1 D0.1 W1 X0.1 Y0.1 Z0.0 Where C is XY clearance, D is Z depth for XY probing and W is work offset to set (XYZ should be self explanatory). You'd need to change the variables I've used above though. Good luck.

I don't think this can be done. #4111 is the system variable for the last H value executed but it's a read only variable IIRC so you can't make a H value "active" without calling it in code. The other problem that comes to mind with what you're trying to do is that the work offset has to be at least roughly defined before you can use the Renishaw Inspection+ macros directly. What I mean is that this line: G90 G65 P9511 Z0.0 S1 (Measure Z Surface) Will try to probe wherever the current Z0 is (plus a bit of overshoot) and the write the actual probed Z position to G54. But the current Z0 needs to be at least already sensibly defined from where you are positioning the probe before calling the line. That's what the EasySet macros (G170) are designed for. Just position the probe close to the part and it will probe along the specified axis (for a set distance) until contact is made then it will set the specified work offset to where that probed point is. Yes, you have to run it 3 time for X, Y and Z. Having said that, you could write a macro that makes those calls but you'd have to deal with the protecting positioning moves yourself using G31. I don't have time right now to knock something up (maybe later today) but as a starter think about this (some stolen from above): (Jog Probe to .25 above corner you wish to probe) #1= .5 (Distance to move in X&Y to probe Z surface relative to routine start position) #2= -.5 ( Z position to measure X and Y relative to probe routine start position) #3= 1 (Work offset to update) G91 G31 X#1 Y#1 F100. (Protected Position) G91 G31 Z#2 G170 X0 S#3 One thing that you'll have to do is between the 2 G31 moves is check the input for the broken skip signal and abort the macro if it's been triggered (a collision has happened). I assume you know how the skip signal command (G31) works and how you'd check for it's activation? (If not, actually look into one of the Renishaw macros). I'll add more to this later.

So are there any bug fixes and enhancements or not? Or are they solely translation fixes and enhancements? Thanks,

I think you might be out of luck. Machine Simulation only works for mills not lathes (including turn-mills like the GMX).

Here's a good video showing how it works, basically the holder kicks the tool off centre.