I ended up doing a bunch of moving prep, and visited with my son in the hospital on Sunday. I'll put some time aside this coming weekend (either Saturday the 30th, or Sunday the 31st), to do a live session. Is there one of those days which works better for you Zeke? I'm thinking around 1:00-2:00 PM, on either of those days...

Glad you got value out of my courses. I was the guy teaching those classes, and Derek was hosting the website. We officially shut down about a year ago, but I've rehosted many of my old class videos on YouTube for free. There is a link in my signature...

I think some Model Prep review, and putting a couple 5-Axis Paths on this part, would be a good exercise for this weekend on YouTube. I will see how much I can cover in a couple hours. I know Advanced Drill is another requested topic, but playing with this part is just too fun Zeke...

Create a Surface from the Circular Face. Untrim the Surface. Now > create an Arc on one edge, using Create Curve - One Edge. That Arc will be Planar to the corner...

DROB, You're on the right track, with adding logic to test for conditions like "is this a new operation" (NCI 1000). However, it is important to know that "Depth Cuts" and "Multi-passes" each output a Null-Tool Change block to the NCI File. I suspect that is why you'd be getting the extra TWP calls, between cuts. I think you'd need to modify the logic to detect "has the op_id$ really changed, or is this really still the same operation, but a new cut?") Most CNC Software derived 5-Axis Posts, started life as a "completely vector based, old-school approach" for repositioning between cuts. In other words; the original 5-Axis Post was designed to calculate "safe" approach and retract moves, based on the kinematic setup of the machine (defined by variables in the Post itself), and based on the "Misc. Integer and Real Number values", which are passed on each operation. Take this with a grain of salt, as it may only describe "historical behavior" of the Post, and may not actually apply to your specific version! At the Operation Level, we've got 1-10 Integers, and 1-10 Decimal Numbers, that are available to the Post Developer, to "trigger" output from the Post Processor. One of the features of the original Generic Fanuc 5X Mill Post, is the "Vector approach and retract", typically done with MR1. If you look at Miscellaneous Real Number 1 (mr1$ variable), this is typically used for the Approach and Retract vectors. There is a function inside the old Generic Fanuc 5X Mill Post, which lets you define a "box" to use for Approaching and Retracting from the part. This can be "a linear offset from the User Defined Stock", or it can be hard-coded positions in the Post Processor. The purpose is to allow you to program 3+2 cuts, using different Tool Planes (think, cutting on Front, then immediately cutting on Back), and the Post will take care of all the "intermediate position vectors", to both move the tool "around the boundary", but also to reposition your rotaries. Depending on how the logic gets called, and the Operations in your Mastercam File are Programmed, the MI/MR values can be used to tweak the Post output, and also to perform the vector approach/retract moves for repositioning between different Toolplanes. Note: the Vector App/Ret logic basically works between any operation, so you can apply this to 5X App/Ret moves "between operations" as well. But again, this also depends on the particular Post you are using, and what particular Post Blocks are getting called.

EDIT: It seems to be related to your 3rd Position Plane. I took the wireframe, and performed a "Translate Plane to Plane" from '3rd Position', back to 'System Top View'. With your original geometry, now moved and reoriented to the Top Plane, the function works as expected. I also tried making a new Plane, using one of the Arcs, of the original geometry. No-Go. Mastercam 2022 doesn't like using that geometry in 3D Space, for some reason. I tried a couple of different "new Plane orientations", with different directions for the XY axes, but still No-Go. Yes, there is something really wonky going on with using Line-Perp, using a Non-System Plane, in 2022.

No, you haven't missed anything. These seems "broken" in 2022. I exported the geometry as STEP and Parasolid, and this is working as expected, in Mastercam 2021. Normally, for Perpendicular line creation, we use the following steps: Open the Line-Perp function (default is set to "point" mode) Click on the entity you want to construct a line perpendicular to Click on the Anchor Point, where you expect the line to "start" (Mastercam now "locks on" to this anchor point) You can now move your cursor to one-side, or the-other-side, of the line, and "Stretch out" a Perpendicular line, from that anchor point (If you've got a "line length locked" on the function panel, then you only get to swap-sides, as you move your cursor to one side of the line, or the other) This works perfectly in 2021, but in 2022, the "anchor point" never gets 'locked in'. It seems to "still float", which prevents you from accurately placing the line.

"Foundations of Mechanical Accuracy", by Wayne R. Moore. Gives you the history of measurement, and how the Moore Company built the most accurate machines in the world, from 1940-1975. Their Jig Bore and Jig Mill machines are still sought-after, for machining parts to millionths of an inch accuracy. There are lots of pictures, and the story that Wayne weaves into the pages is quite compelling. (At least, it was for me.) If you want to grow your knowledge of how to measure and make precision parts; this is the book to do it. "CNC Programming using Fanuc Macro B", by S.K. Sinha. Another book that gives you great insight into how any Fanuc-controlled machine functions "under the hood", and shows you how to become a true master of writing NC Code in your programs. Each book, is worth far more than its own weight in gold. The information contained in each one is priceless. However, it only becomes so if you actually learn what they are teaching. That motivation has to come from you. If you want your work-life to get better, and to earn a higher salary; then you've got to invest in your own education. It won't all be fun. It won't all be enjoyable, but the harder you push yourself to learn; the bigger the rewards you will reap in life.

Yes, a Global Formula, entered in the 1st column, is probably the best way to handle this. That way your Mastercam File units are correct. Are you positive the feed is exactly a factor of 10 different? Could it be in Metric mode, rather than inch? 25mm per minute instead of inches per minute, would be .984" of travel, in 1 minute. Not that I doubt you, just wanted to be sure that multiplying the Feed value by "10" in a Global Formula, is the correct fix.

I wonder if this could in some way, have to do with the Display List? There is a separate "part of the database", which tracks visibility of entities. I wonder if the wireframe and/or surface, could be "visible on the screen", but somehow not registered correctly in the Display List, so the system doesn't "see" the correct projection?

Advanced Drill was new in 2021. It has been improved for 2022. Yes, you should use the checkbox to force a rapid move down to the last drill peck depth, and then it will feed to the next depth, and repeat. Say what you will, but we had to do this for the last 15 years by building Custom Drill Cycles, which wouldn't even show any of the pecks, or any other start/end moves, so this is a huge improvement. 2021 needed some improvements, which they have made, and I'm sure there is still room for additional improvements in the next couple of versions. Advanced Drill has been a huge addition. Especially for users who don't use pecks because we've got Coolant Thru-Spindle to flush the chips. Now I can approach a hole with the drill spinning CCW at 500 RPM, feed to the start depth slowly, stop the spindle, turn on the spindle CW at the start RPM, ramp the RPM up in stages while enabling the CTS pressure to build, then drill my hole to depth. Finally I get control over the retraction process steps as well.

No worries Jeff. 2D Pocket is probably your best option for uniform passes, if you want to control entry points. The issue with Horizontal Area is you can't tell it to "enter the cut from the outside". It is always going to ramp down onto the floor, unfortunately.

I'm pretty sure Horizontal Area is designed to "ramp" down onto the part, using one, or more, depth cuts. You really can't tell it to "start off the part". Your best bet, if you require the control, is to use a 2D HST Path. Of course, this requires creating a bunch of extra 2D boundaries, so you have "cut geometry", "avoidance geometry", and "air geometry". The "air" geometry signals to the path, where the tool can "approach from the outside". You do have to use the "from outside" cutting strategy.

G93 was the "original" method of synchronizing "linear motion" with "rotary motion". You XYZ axes move in linear motion, with respect to time. "Inches per minute" or "millimeters per minute". Your ABC rotary axes move using different units entirely. "Degrees per minute". (Same units, in Inch or Metric mode). "Inverse Time", means that we specify "the inverse of the amount of time it takes to complete each move. When using G93, every line of G-Code must have a unique F value, that tells the machine "how long it takes to complete the move". Because we specify the "feed rates" on our machines in terms of "1 minute", that becomes the Numerator of the equation. (1 / x) The Denominator is the "Time" component, which is simply the 3D Distance divided by the velocity. 1 / Time, where [Time = 3D Distance / Velocity] For example, in Inch units, say we are making a 4" long move. We want that movement to happen at 25 IPM. 4 / 25 = 0.16, so that is our "Time" component of the equation. 1 / 0.16 = F6.25 Now, we can vary either the "3D Distance" or we can vary "the velocity" component. (How fast do we want to complete the move?) If we programmed the same 4" cut, at 210 IPM, then we have 4 / 210 = 0.0190476, and our equation is: 1 / 0.0190476 = F52.5 What if we changed the "amount of distance"? Let's change that same equation from a 4" move, to a 0.020" Move. With the same "25 IPM" velocity: 0.02 / 25 = 0.0008 1 / 0.0008 = F1250. Now, if we want 120 IPM velocity: 0.02 / 120 = 0.00016666 1 / 0.000166666 = F6000. One thing you should notice based on the equation above, higher "F" values equal "shorter or quicker" moves. (Remember, it is a combination of distance divided by velocity) Lower "F" values indicate "slower or longer" moves. It is not uncommon to see "very low" or "very high" Inverse Time Feed Values. You should be careful to check and be certain that you aren't hitting the "Inverse Time Feed Limit". This is typically "F9999.999" in many Post Processors, when some machines are actually equipped with larger Inverse Time F Registers. (Newer Haas Machines, for example, use F40000. as the max.)

I think Ron is spot-on here. The only other solution for paths which do not accept a negative stock value, is to create "offset surfaces", or in some other way physically manipulate the Geometry you are going to cut.