Nothing like cheaping out on control options, or not using what you might have under the hood. It's even worse when you have an option installed where the MTB spec'd it as standard, that should be implemented as it would save on maintenance, and they don't have anything configured nor know how to configure it......

At least in a mill configuration, this depends on how your parameters are setup. You can have it either way if you want. Interestingly enough when parameter are set such that 359 - 0 is a 1 degree move (shortest distance), a reference return isn't necessarily going to follow those rules, be wary.... I wouldn't imagine the rules would change on a T control.

I don't remember the settings, but IIRC there is a parameter to use the offset register's instead of the mazatrol tool data with comp. I also recall, although it be fuzzy that you can continue to use mazatrol tool data for the length, and only grab offset register for side comp.

You will likely need a custom post and linked sim. Does your post output code properly adjusting C for y position?

I have been trained to figure about 6-8 minutes planned tool life with inserted ceramic milling tools (round negative inserts) if you are running them at the optimum conditions. Plan for using redundant spares if you need more than that and just divide up the time equally between them and change them every part. Have spares ready outside the machine to swap it. Roughing with ceramics is by far the fastest way to plow nickel based material off your part. Through spindle air isn't a requirement, but is highly highly highly recommended. It just helps to make sure the chips get away from the cutting zone and off of the workpiece. You will chip / damage the paint in the enclosure, and any you won't be able to see through any plastic windows shortly after you start cutting. IT WILL BE LOUD, especially if you are getting the level of productivity what warrants the use of them. But generally speaking ceramic inserts are on par or likely cheaper than the carbide inserts that might survive, but will smoke carbide on cost per cube removed, and time getting it done. Let us not forget in a job shop environment where the next job is waiting, cash is king, and you need a balance of roughing cycle time / cost per cube removed, that you make sure to bias toward getting it roughed out as fast as possible while still falling within the tooling allowance quoted for the job or within the machine rate. If you are running negative rounds, and keep the depth of cut below a 45 degree engagement angle, in theory you should be able to get about 8 indexes per side. But mind you they are typically infinitely indexable. I use a marker to mark the insert where it was to help gage the amount of rotation. For the solid ceramic end mills, I have never worked with them, but have spec'd them and the customer backed out because they didn't want to run their spindle full tilt for a few minutes of roughing, and we couldn't quite go fast enough for confidently applying 3/8 tool. I ended up using a Harvi III 6 flute (coated carbide) at about 175 base surface foot with an dynamic mill toolpath. 20% or 40% stepover I believe, don't be afraid to take some radial engagment, it will help with life, just try not to take more than 40%, back off on the width as the depth gets deeper. If you go to fast, or have rigidity issues, it will just start peeling the edges off the endmill, gets knarly fast. A 25 sfm change can make a huge difference. I didn't ramp but the final .025" for the entry for the pockets as I had a flat bottom drill to poke the start with. I highly recommend drilling over ramping with carbide. Kennametal GOdrills work great in 718 and 625 Inconel. (any material actually) 85 sfm, feed with nickel based starting book values, through coolant for sure. We were drilling 8mm holes 8xd deep with great success. If drilling through, pay attention to the exits, you will want to slow the feed on exit by about 40%, not as important if you have through coolant, but is still a good idea to prevent chipping the drill corners, as you won't get far once you do. When processing that part, I drilled then removed the material below the hole so as to not have to exit the material anywhere. Customer couldn't believe the difference in tool life. It was consistent for once!!!!

A sample file would tell us a ton as to why you are getting the output you are. Short answer as we don't have anything much to go by: Use 5x drill path not planar drill toolpaths. Which if you are up to date and have a multi-axis license is all under one toolpath now. If you are creating a toolpath for each hole, combine them all under one and it should act better than it is now. Past that it would be a post issue likely.

Really it all depends on the workholding.... Most typical processes that will effectively cut inconel will do it if you can hold it properly for the op.... Using a drill will certainly be an issue given they are less than 1xd. The .098" diameter hole might be ok to drill. I suggest a Kennametal GOdrill for that, assuming it is well supported, such as on a sacrificial support plate. Reduce feed to 40% of normal feed on exit to prevent blowing the corners off the drill. The .221" hole, I think i'd go with a helical/circle milling solution. Using the .098 to pre dill might help extend tool life of the end mill, but would possibly not be overall cost effective. I think an 1/8" Endmill would be about perfect. Preferably something with a 1/4" shank and stub length. 3 degree ramp angle, 65 sfm, .0002" chip load. .005" finish pass on the wall.

@Elvincncthat code is interesting. The only thing that I see as an issue with it is that you wouldn't be able to run it in AICC as IIRC you can't have macro code when in lookahead mode on a Fanuc. Stupid I know, but that is how it is... Otherwise that is a great way to be able to adjust the program output for tool variation without having to go back to the CAM system or without having the 3axis comp option on the machine control.

After thinking about this more today, what I think it really boils down to is the ability to at least turn it on and off. I also think it would be nice for many people to be able to use it on swarf, but maybe only in one way mode, or if in zig/zag would give you the ability to flip when going in the conventional direction. It would make it such that you don't need to use vector based comp. The machine can and will compensate on it's normal to the tool axis and toolpath direction, which in the case of a cylindrical tool would be the same as the contact point normal vector. What I would like to know, is that if you have G41.2, do you automatically have G41.6 (type 2 vector based comp) on a Fanuc? Maybe this is something James or Ron can chime in on. But I think at some point here we need to get some good use case info in place. I know for me personally, I had two use major cases. One for where I wanted to run regrind endmills and was using 5x curve, as well as standard contour paths without G68.2, And one where I was doing rotary surfacing where I had the need to run an 80mm ball with reground blades. This is where I would have needed vector based comp, but at the time I didn't have the time to modify my post to transform the surface contact point data to match the machine kinematics. Not even on a test basis. Therefore I was never able to test vector based comp on the machine. I used to program everything from the center of the radius, so it wouldn't have been a problem to just update offsets and let it fly. I had a large pile of dull blades and a big need for using them. So my solution ended up being to have .25mm different increment programs, and run them when I was running abrasive laminate materials. Not a big deal. But comp also would have been useful for making size adjustments that don't effect other features, without having to change work offsets in relation to center of rotation. In this case we were not using TCP for the table rotary axis, but we were using it for the two head rotaries, so there was that complication as well.

I think I start to stand with Aaron on this one a little. It's not so easy.... I suppose having a switch would be easy, but I am starting to understand why left/right is irrelevant on a surface based path. Technically speaking if you are comping to a surface normal vector as you would with "true" 5axis comp then left/right doesn't have any bearing whatsoever because the resulting comp vector will dictate the direction. but if you aren't feeding the machine the comp vector than the "side" becomes relevant assuming a wear offset. Fascinating subject. I think we need to start breaking this down into sub sets. Specific comp types for specific toolpath types and shapes, on a specific control. I would say if we want to get serious about helping develop new practices or standards moving forward we will need to start making sure we are all talking apples to apples. Basically speaking, as I understand it, there are two types of comp: Side Comp (in a plane normal to the tool axis) - This would typically be done on a Fanuc with G41.2/G42.2. This would typically be applicable for say a curve 5x, or a swarf path, but less likely to be used with morph or parallel. I can see zig/zag cuts with swarf being a challenge if were to just set G41.2 and roll on. I think you would want it to flip the comp direction at the link between slice. Surface Comp (in the direction of the surface normal for use with ball nose or bull nose on free form surface) - This would be used with say Morph, Parallel, and so on and would be more for use ball nose cutters. This is where Left/Right wouldn't really be applicable here as the vector would control the direction. I don't have any experience with this type of comp, so please, those that do, chime in.

Depends on what type of toolpaths you are trying to comp..... There are multiple types of comp that can be used. For full 5x surfacing type paths you would need the 3D comp option, and you would have to provide the machine with a comp vector on every line of code. I have never implemented this type of comp. I have had the need to in the past, but settled with just having a few different versions of the posted code to get by. I had some different technical issues in my way. One of which was that the MW paths did not port the info I needed at the time (surface contact point, and surface normal vector). Certain considerations also need to be made around cutter size and comp amount with concave geometry, making sure you don't comp yourself into an opposing surface, which get far more complicated when we start thinking in a 3D multi-axis situation instead of a 2D contour. For 2D Contour and curve5x type operations with G41.2/G42.2 in a Head/Head machine, really it isn't that hard to implement. The control figures out the comp vector and life is good. Though, sometimes you will get errors due to lookahead which have to do with the control not being able to figure out a comp vector on small point to point moves, but mostly it works just fine. I am sure there are ways of fixing this, but I never had the time to figure out mathematically what the control was having trouble with. You end up basically just replacing G41 with G41.2 and move on. The best method IMHO here is have your post output G68.2 for any planar work and use G41/G42, your contouring code will be more concise using arcs and lines, and you won't have issues with the machine potentially alarming out regardless of comp value. For curve5x type paths, you could implement it to use G41.2, and for the most part, it would work without issue. Edit: I will add that this is assuming mainly just for wear type comp applications. I haven't been in a situation to test full radius comp with G41.2 in a curve5x type path. I personally make it my practice to never use full Radius comp with I have a CAM system at my disposal. If I will need to make significant edits at the machine or when building a macro of some type, I will consider full radius comp, as it can simplify the code and math required to get it running, especially around rolling corners or adding chamfers. Ohhhhh, I could go on for days on this subject, wish I had a need to dig into this further and could do some testing. I'd love to be able to provide people with some good hard and clear data / guidelines on 5ax comp methods and practices. It truly opens up tons of options and improves operability at the machine for production and prototype type 5ax work. It also affords shops the ability to better lock down their programs on their most expensive and critical equipment and hopefully prevent more crashes and programming errors down the line. I'd much rather be changing a comp value than reposting and running a "proven" Mastercam file. We all know mistakes can be made. Now if you use CAV, like Vericut or Camplete, well, that would take some time to rerun your "comp" program through it, so you would be saving time by just using comp.

Well you could use a misc integer/real. But how to change things on the CAMplete side to take that info and do something with it. I have no idea. I am not a camplete user. With a normal mp.dll post. Not a problem.

Well.... given the data you are given in the NCI, I suppose with some math's it could pretty easily be any of the above. Now, interfacing a method of selecting the comp method with CAMplete, no idea how that would be done.

On a table/table, yes, definately, and almost regardless of parameters settings... Now that said, on a Head/Head. Different ballgame. I used to very confidently turn on G43.4 on my initial XY approach, then approach in z. The only caveat was that I had it set in the parameters to activate G43.4 at the end of the move. So it would go to the right position, but it would be fastest axis path for each axis. Not interpolating a straight line from A>B whiles moving the rotaries. Complicated subject. As James said, there are Plusses and Minuses to everything. The key to all of this is to know without a doubt as a programmer what the machine behavior will be between toolpaths, and toolchanges. As well as in cases where the operator stops, jogs, hits reset, etc. in the middle of a program.

It can get you in trouble really fast. Hence why I don't use it a lot of the time. But if you do it properly, it pays off in spades. The problem is, most people like to just start sketching, which is a no no in true top down. The other thing with top down methods is if you don't have a robust integrated pdm / teamcenter system, multiuser on the same assembly or part is a total nightmare. Top down enables people to work on things in teams. Of course you need a robust CAD software to do this well. NX, Creo, Catia, are first to come to mind for that at an enterprise level. Solidworks isn't bad, but I think has some limitations if not implemented properly. All CAD systems require a certain level of rules / standards and strict adherence to them is the only thing that make it work long term without major timeline setbacks.

Yeah, I had a misc int for it in the past. But given some issues with it on the machine I ended up not supporting it further in the future, I found it best to create a repeatable process and change cutters when they went out of spec. But we were cutting wood so tool life wasn't an issue. Typically speaking in half years or more.... It wasn't a problem for me to use comp, but it snagged the operators too many times, as sometimes it wouldn't take a 0 value. Due to some parameter/toolpath issue I couldn't figure out, I for some reason couldn't convince them that a .001mm value wasn't going to effect things enough to worry about it.... Some vector/lookahead error on point to point cuts.

Last I had checked they wouldn't output in the old school paths either..... did they at least hook that back up?

These types of things are precisely what keep us employed..... On a more serious note. Most of the things they are doing are purely based in best CAD practices, or basic CAD defaults. We have similar things on the CAM side that we could care less about on the CAD side, and vise versa. There has to be a happy medium somewhere. That said, when I model fixture parts I will model to nominal size (not necessarily center of tolerance), as it makes for a much easier time to make your assemblies go together properly without major mistakes, it also makes drawing creation far faster and at least how my mind works, that is when I start to think about determining final fits and whatnot. Once the drawings are done, I used to sometimes go back and make a new configuration with everything in the middle of the tolerance. A lot of this depends on if you use top down or bottom up assembly modeling techniques. I am typically disorganized and end up with a hodgepodge mixture of both, but mainly bottom up design as I go. I have taken some training on the top down approach, but some habits die hard and usually I'm not doing things complicated enough to where top down becomes a requirement. It would be cool if when create a drawing, you could have the drawing tool automatically kick out an associative model, that has the surfaces which were tolerance color coded based on if it is unilateral, bilateral, or whatnot. Then we would know to check and select tools or comp toolpaths accordingly. I supposed if more people used annotated 3d models as the standard it wouldn't be needed.

You will have to get a little specific with your questions on how to make the changes you want to make, but to say the least, what you want to do isn't that difficult, but you will need to be very careful when you do it as you may end up with unexpected behavior at certain null toolchange sitatuions. There might be swtiches in the post to get it to this already built in. Research that possibility first then report back. It will be under a variable that reads something like safe index, but can't remember exactly if that was the one that controls that behavior.

Stupid rules.... They have a purpose. But when it comes to troubleshooting a problem there you should be able to have exceptions from time to time. Another thing you can do is print from your phone. See if you can set that up.....

Are you working in inch or metric? Working in inch, did you put 6 in the previous tool radius. Dumb I know, but likely it is something stupid like that. Another thought is to close the region and add the closing leg as an air region.

I stand corrected. I am going to go with that the dealer and CNC software need to be contacted to get this all sorted out. Something doesn't seem right for sure. As previously stated it could be any number of things. When on the MT side of the software, it becomes even more of a unwieldy beast than normal, no better than CNC to search for the problem and come up with a solution, it is most certainly a requirement given the current restrictions. I doubt the dealer switches and whatnot really would have any effect on the issues he is facing, unless there is a training issue in play. Best of luck, very interested in seeing how this is resolved. Also, I'd be happy to look at it if you wanted to send me a zip2go? I have a partner license, so I should be able to work with your MT environment.

I don't think he's using MT, I think he's just talking milling paths in lathe... IMHO, most if not all of his issues are post related. +1 for postability

Except the logic he presented forth.... He has good intentions, but.... I'd want the parts to be super simple, mostly just hole poking type work, I mean really simple 2.5d work. Otherwise machines will be sitting all the time while operators fat finger their programs at each setup. I do believe WPCSHIFT is what you are after. Your best bet would be to get a local apps engineer in from your dealer and have them work out a programming sequence with you. With that many machines on your floor, surely you can get them to come in and help.... Likely for free if it can be done remotely, which in reality shouldn't be a problem. But I still say WHY? Are the operators programming the simple stuff at the machine? If so, there are potentially much better ways to operate a shop, then again, we don't know what type of business your shop does, maybe it works pretty well. Based on how many machines you guys have, it seems to do pretty well.

It amazes me to this day how cheap companies are.... I know there are cases where it makes sense to only have mill level one, but gosh, in this day and age, having full 3d capability makes for being able to solve problems with a much bigger tool bag. I have had a multiaxis seat for 6-7 years now and I don't think I could even go back to mill3d.... Once you start using the moduleworks stuff, about all you end up using from the mastercam paths is 2d dynamic, opti, 2d/3d contour and the hole making paths. As far as surfacing, maybe raster, but that's about it... I used to have a mill level 2 license, and the crap I had to go through to get something done was amazing, the cost of moving up to even mill3d would have easily been recouped in programming time alone in less than six months.