Does your boss have draft. If not, use the tangent point on the wall, and do a contour 3d using the tip as the compensation point, then use a - radius stock to leave vertically to get it to the right height. As you found as well, pencil should work. Otherwise, you could use the project toolpath in the MW suite and accomplish the same thing.

LOL, I knew you were going to ask this. I have a calculator that gives me this information. I do not have the formulas right handy at the moment. When I get a minute I will see if I can create something that can be shared to calculate this. Or I will at least dig up the book I have should have this in it. May be online, worst case I could derive it.

What I mean is how many cutting points/flutes are in contact with the material at one time. It is not reference to how many flutes there are in the cutter, yet that is part of the calculation, but so is width of cut, depth of cut and helix angle of the cutter. It's a decent indicator of how much cutting force you are going to have.

Zeke, Feel free to reach out for some optimized parameters. I know you guys run Widia and Kennametal endmills. I'm happy to compare notes on some parameters and see how conservative you actually are right now.

Most people don't maximize the productivity they can get out of the tools they buy. Granted it's about finding a good balance of productivity and economy from tool life. At least 4 out of 5 applications I run into out there, I can get more productivity without sacrificing any tooling cost per part, often with a more expensive tool. I know what I threw out there would fly without trouble using our tools. Hope I haven't steered anyone down the wrong path due to not knowing the complete setup.

You are way too slow for that radial engagement. Not that I want to help a competitor sell tools... I would do as follows. If this is in a 50 Taper with a good setup, run full depth by all means. If this is a 40 taper, you have too many points of contact for full depth. But if you back it down to 1.625" depth or less, but not less than 1", you will find success. Keep the 5% stepover for now. I'd run 1000SFM, .0112fpt. This takes into account chip thinning and speed factor based on the light radial. 5093 RPM, 341 IPM. Feel free to back off the feed a little bit if the machine can't keep up, but I would go no slower on the feed than about 200. If it burns up try to maintain the chipload, but reduce the surface footage. Air blast would be better than coolant, but coolant would be ok if you can't get the chips away from the cutter. I'd prefer dry if you don't have a chip evacuation issue. A little heat will help you as long as you aren't re-cutting chips. I would consider the above parameters middle of the road for our tools. The fact that you have chatter is likely a function of machine stiffness. Your original parameters show 6 points of contact, which IMHO for almost any 40 taper is way way too much. 3-4 points is better and should work on even on a medium quality machine Nothing wrong with 4 or 5xd in steel. Many people do it everyday. But quality holders, setups and machines become very important very fast. As I mentioned earlier, I likely wouldn't be doing that in a 40 taper with a 3/4" tool. If you needed to, I would use a tool with a tapered core and maybe drop a flute or two to keep the contact points / force down. My favorite 5xd tool is the Kennametal Harvi II long. Never had trouble getting it to work. I've run it in anything from alloy steel to Inconel with very good results. One notable success was in Inconel 718, similar depths to what you are doing now, in a 40 taper, taking about .010 stepover. We had a little springing, but that was from the setup as we were cutting on a weak trunnion table. Husker

Programs in Siemens macro language IMHO can be less than half the size and complication of Fanuc and do the same function almost instantaneously. No long processing time.... I wish Fanuc would give us the same power without having to go to integrator school...

Something is funky with your chaining. It works great for me from outside. Select the face you want to cut as the machining region. You can do that by either selecting the face, or the outer boundary of the face you want to cut, think in terms of the actual area you want to cut including any islands. when you select a face, the island won't be included, but you don't need them to be. Then select all the avoidance geo. The areas you don't want to cut, they can be inside of or outside of you machining boundary. You can use solid faces or wireframe. No need for a containment boundary outside. The select from outside for the machining region strategy. if you preview you should have blue indicating air cut area, outside of the red hashed cut area, with blank zones where you want to avoid.

The 2d HST toolpaths do fine for finishing with a decent pattern similar to pocket, just use area mill instead of dynamic under pattern. What am I missing?

Another thing to toss into this... Sometimes when they say .020r Max. They may have an obscure spec called on the drawing by reference that would also allow a 45 degree chamfer that would meet the radius where they become tangent. If you see a bunch of code specs in the title block, and you are making parts for the end customer. It always pays to get a copy of thsoe specs so you can interpret the meaning of .020 MAX. At one company I worked for, we had a lot of 50 degree max callouts on faced shoulders. They were modeled at 90 or vertical. Most of our plants would just use a shoulder mill and be done with it, and then would complain they had to deburr the edge or weren't getting very good too life. I got clarification from engineering and used a 45 degree cutter which greatly reduced my tool cost, performance, time in cut, as well as eliminated the burr! Notes like that on drawings are game changers sometimes.

Is that using template setups / matercam interface and loading stuff that way, or building setups and whatnot in vericut manually? I have personally never used the mastercam interface except oobserving when working with customers that have it... We don't have a license for the interface. I used to use vericut all the time, but completely standalone. If I was in a hurry I would build it out in mastercam, send it to the customer I was working with and have them use the interface to build me a template, then I would work the vericut file from there. That was my shortcut to get tools and fixtures located. I thought their training was actually pretty good. Though I wouldn't say I'm an average student as far as picking up new software.

They are also throwing in free training every year with each maintenance seat. Something I don't think they did before.

I do believe you would be looking for nano smoothing. G5.1 Q3, probably not as easy to setup and configure as the HH cycle 32

Short Answer: No Long Answer: What I had done was more to compensate for lack of high quality surface models. At the time I did some modeling of the features I was cutting to create more accurate surfaces to drive with that would have better continuity overall, but by no means perfect, as the shapes were out of my league to model perfectly with the time I had. Those efforts helped immensely, but as I was using a tool that was larger than the minimum curvature (very very very very small ripples in places) this fault caused me to have some "extra" points here and there. You know, those pesky zigs and zags, or that extra point between two points that you don't understand why the toolpath generated it, and lack of a filter won't allow us to remove it? Those were what I was removing. I must stress that I didn't correct any point to point data. I was just evaluating the motion of the toolpath and deleting any points that exceeded a certain vector difference over a moving average based on a number of points in front and behind of where we were. I had played around with filtering posture changes as well, but given that I was using a guide curve with the tool path, it wasn't really needed on that job, filtering the translational points in space was more than enough to make a better program. I wish I had before and after pictures of the parts. The before part looked like it had pock marks from ball bearings being dropped all over it, and the after looked nice and smooth without so much as a divot. Mind you this was cutting wood on a large gantry router. I'd say we might have been successful at moving around 120IPM at the fastest with the original program and the filtered program was moving constantly around 300. I had other jobs where the combination of translational and rotational filtering would have helped, but never had time to refine the algorithm to the point where I was going to cut parts with it. Not to mention it was a pain in the butt to get the import NCI function activated in MC after 2017, so I didn't bother. I think that function is back on by default now. AFIAK it never totally disappeared before, but was just left out of the GUI for us to use. As for the functions you highlighted in the pictures above. Yes, combinations of those settings will have a huge effect on the quality/capability of the program to generate a good surface finish, and/or move at decent feedrates. But the most important thing for getting good results is good input geometry. Constant curvature continuity of the base drive surfaces will yield the best results by far if you need to drive posture using the drive surface. Otherwise, if using surfaces without constant curvature continuity, using points or lines from whatever logical distance from or through the surface will yield the smoothest posture control. Smoothing of added tilt collision controls, such as shown above are there to smooth from the normal tilt strategy into the added, and back again. I haven't played with the smoothing feature on the unified toolpath yet, but will at some point to see how and what it does. Maybe there is some hope. Some sort of filter function on the Moduleworks paths would be great......

Many Many Things. But I guess the two most complicated things I ever did were: Filtering points and postures of full 5ax NCI files, so I could import them back in and post them. This resulted in a lot of time saved. Roughly 30-40% improvement. Drastically better surface finish. This was done via VBA. Excel was just a vehicle to graphically see areas where changes were made. The other was to make end to end size compensation on some rotary surfacing ops. I wrote a routine that could rotate G1 and G0 points about any point in space. Never got around to adding further functionality, but it wouldn't have been too hard to at least give it that ability to do drill cycles and G2/G3 moves as well. I just didn't need it, so I never bothered. It was far faster to write that routine than it would have been to correct the geometry issues on the machine or in CAM as everything was an organic surface. Never figured out if I could have used WSEC or coordinate rotation to correct the issue as we were running G43.4, but for H/H and were rotating an added table that was not compensated, which is where the error was... Worked like a charm. I could compensate out .002" or so over 15" in about 30 seconds, with just a few clicks. Generate the new program and run it. I had excel on the machine control computer so I didn't have to go back to the desk.

That sounds like a good top notch insert application. .031"wide x .050"deep capability NG2031R KCU25 I'm guessing 3/4" shank?

If Sandvik is going to take an active role managing MC, they will push very hard to become the best in the industry at MT. It will take time, and lots of moving pieces would need to come together and mesh (finally), but maybe that's what the product needs in order to become widely accepted in industry. From my dealings with it, it's close, but customers don't have enough dealings with it to understand how to get up and running with it efficiently yet. Too much reliance on CNC to provide post support, CNC likely isn't getting the feedback they need to make the proper post/environment improvements. Maybe Sandvik can help bridge between builders and CNC to help solidify the post processor development and software capability development activities. One can hope anyway. I'm going to try to stay positive about this, but at the same time, I'm sad that they have agreed to sell out. I'm sure it was too much money to say no to. Curious if the family will stay at the helm long term, or if they will bow out completely.

I don't know if those options are available on the 18i series controls. If they are, that would be the way to go. IIRC, and correct me if I am wrong, but Nano Smoothing 2 is supposed to compensate/smooth posture differences as well. It is Nano smoothing 1 that doesn't look at the rotary motion. FWIW, smooth TCP is probably the option that would help the most, short of reprogramming with a much finer/smoother input toolpath. Given the age of the control, I think the key will be creating a very smooth base toolpath. Focus on smoothing the rotary motion. The linear movement will be where it is, but generally the smoother the rotary is the smoother the linear motion will be as well. IMHO, it is almost always best to isolate the jerky motion down to one linear axis at a time. For me that used to be Z as I used to to wrapped spiral cut parts with a cylindrical or elliptical pattern surface.

That is the culprit 99% of the time....

I was thinking about this a bit more and have decided to elaborate. A ball bar can be a very handy tool for detecting mechanical problems on routers, but you have to toss aside the usual test routines sometimes to get the problems to show up in the plots. Turning up the test feed to run at feeds that you normally cut at are important here, especially on tack drive machines. It can be very useful for detecting bad teeth, loose motors and such that don’t move unless under stress. Having had a ballbar for a while now I wish I had had more time/opportunity to play with it and develop more tests and procedures for evaluating machines. Especially in regards to evaluating kinematic/geometry errors on multi axis machines.

Depends on what you are doing, 99.99999999% of the time this statement is true.

It's been so long I don't honestly remember. But what I do remember is when using 5x Curve. Filter setting, and tool axis control have more importance on the smoothness of the path than the curve following method itself. Of course the curve following method will influence the "resolution" of the tool axis control and overall motion of the machine, but the "smoothness" of the tool axis control is more dictated by the method of which you pick. Way too many ways to skin the cat once you get into 5x Curve to take a guess on what you should/could be doing.... Post up or send me an example of what you are trying to do, and I will see what I can do to make it "smooth". I'm sure Ron or James would love to pitch in as well. More generic the better as all can learn if we make it public. When I think of making a smooth 5x toolpath, my brain immediately starts thinking in terms of physics and calculus. Determine the outcome desired, then balance that with the cutting velocity required, then you can think in terms of acceleration in XYZ, and then in the case of acceleration of the rotary axes, which IMHO will slow things down more than accel/decel issues in straight XYZ, as they affect the XYZ motion directly NO MATTER WHAT, further from center ->> the worse it gets. This is where options like the smooth TCP / posture control function on a Fanuc control actually smooth out the angular displacement issues between points which cause great acceleration changes in the rotary and translational axes. If you don't have those options, you have to do that at the toolpath level, which can be done with time, patience, and knowing how to recognize and eliminate the trouble spots. This is typically the way to get the absolutely fastest path anyway, so for long run stuff you may as well start to develop your process on doing it. Food for thought: if you have a generic non-tcp post, posted from centerline(s) of rotation, you can edit the post to actually calculate and output acceleration values for each axis at each point and you can theoretically use that code to look for your hot spots mathematically, and then subsequently know where you will have areas on the machine that will greatly slow it down. I haven't done it yet, but I think there is a function on the post side of things that you can use to draw geometry on a level in mastercam. You could in theory use that to draw a visual representation of the toolpath that met certain criterial for acceleration, so you could visually pinpoint the trouble spots. Many times it is just a matter of tweaking a few vectors, or deleting a point here and there. I have written filters in excel that filter the NCI, I then import NCI and post the paths. Sometimes resulting in 50% or greater reduction in cycle time, with vastly improved surface finish due to constant cutting velocity. blabber blabber blabber, I could go on forever. I'll stop now, before I dig a big hole where I need to explain myself.

Fixed. IMHO, unless your taps are free, and there is no other choice, just don't. Use a marginless free cutting carbide drill such as the Kennametal GOdrill and then threadmill with a quality threadmill that is as short as possible, either solid or inserted work fine. Don't expect to be in a hurry. Unless you get lucky and the solid carbide taps you have happen to come with speed recommendations and geometry tailored exactly for your parts and material. It just won't be cost effective in a production setting. Also, drill and threadmill life will depend greatly on the grade and heat treat of the Inconel you are cutting. If it is 718 and is in the 50rc range, just run, run far away and don't look back, you will go through a few drills before you dial in the feeds ad speeds such that you can make a hole, but to tap it .... you can mill that stuff all day long with ceramic (in 8 minute increments...) but holemaking the hard stuff is a different art all together. Ron was spot on with the tool cost info. I typically figure when using conventional carbide cutting methods in inco materials, for it to take 10x the time and 10x the tool cost of 4140 for the same parts. In a typical job shop environment, cutting whatever you come across, other than stainless and super alloys, I typically figure a single cat 40 spindle to use roughly on average 15k in tooling per year, total spend. Cutting Inco, depending on what you need to do for the parts you are cutting, you can expect to spend 30k or more per month on that same spindle in consumables... Course there are lots of considerations into that number, but if you are keeping the spindle turning in Inco, expect to be turning inserts and changing tools all day long. An optical offline presetter and spare tool assemblies are absolutely paramount to productivity. Having a machine that you can swap tools in while it's running is also highly desirable. Don't let any of this scare you away from the job, just know what to expect.

I do believe there is the ability to set a password for the ability to change NE8 and NE9. What series Fanuc control do you have? I don't recall if the 16i/18i had this ability or not, but IIRC the 31i series do. I personally do not know a way around that password.

For sure, I like using 180 degree flat bottom drills for pre-drilling pockets, especially in titanium and steel. They have about a .045" point to flat distance which is very quick to helix out. Typically I will do a helix bore after the drill operation, stock model, then dynamic or optirough, give more control to reduce the amount of entry motion. IIRC you can get optirough to do it for you without much dinking around, but have certainly had trouble making it as optimized as I wanted it.