Oh, I'm in 100% agreement. You're doing it right, because you took the time to set it up that way, and now your company is reaping the benefits of your knowledge on how to do it right.

Let me qualify that John > when you are physically setting up your part "free standing" on the table, not using dedicated work holding. Lol, you're just spoiled, because most of your parts fit in dedicated fixtures/vises on the machine, and you know where all those surfaces are located. You're not taking a giant part, sitting on 1-2-3 or 2-4-6 blocks, and tapping it into location, then running an indicator across the part to be sure the part surfaces are parallel to the axis travel. I mean, feel free to correct me if I'm wrong here, but there is a big difference between the type of part I see the OP cutting, and what you're doing with your Horizontals...

Yo Pete! No wrong way to machine a part, given your constraints. If your company is willing to invest in the options on the machine, then there are certainly newer options for making your life easier, all it takes is making the investment in a proper Post Processor, and purchasing the functions on the Control. But it does also take consistent practice in calibrating the Probing System itself, then going through and calibrating the COR (Machine Rotary Zero Point) Values. WSEC is a God Send for machining Castings! If you are doing a bunch of that work, it may also be worth investing in Verisurf, so you can make measurements of the Castings "on the machine", and feed that measurement data back into the Verisurf model for a "best fit". This can be used to adjust your "main work offset" location on the part, to be able to "fit the features within the as-cast material". Used in combination with WSEC, this can not only make the setup of these complex parts "easy", it can help you to rescue castings where they are on the edge of not being workable by "best fitting" the finished part surface locations to the casting, and then correcting for the misalignments on the machine using the WSEC functionality.

Fanuc Controls are like a "lego set". Some manufacturers (like Matsuura) will setup a "standard package", and will refuse to sell the machine with less options than the standard package. I'm a big fan of doing this. Other machine tool builders will offer a stripped-down, bare-bones control as the base option, and let the customer dictate (pick-and-choose) what options they want to pay for. This keeps the cost of the machine/control combination low, but often results in certain features being missing when it comes to making the most of your machine and control combination. The other thing which factors into this is the Post Processor, for formatting your G-Code output. You can automate "code output" from Mastercam to your machine, but you're relying on a "perfect setup", to know where the part sits on the machine, relative to the Center of Rotation. If you have good setup skills and discipline, you can get away with a lot by doing things "manually", which is what you are currently after. The modern way of addressing this on a CNC Control, like the Fanuc 31i-B5, is to use "Dynamic Codes". This is where a Calibration Routine is run, most often by using a Gauge Sphere in combination with a Spindle Probe, and the results are used to calculate and set "Center of Rotation" Parameters. As James has mentioned, these would be Parameters #19700-19705 on the 31i, for a 5-Axis machine. For a 4-Axis, only the #19700-#19702 would be needed. If you're using Dynamic Codes, where the COR is set and maintained (calibration is performed at regular intervals), you can also take advantage of Tilted Work Planes (G68.2), where there is essentially "1-line of G-Code", which takes care of the rotation, and optionally the "offset" of the XYZ location, to the Feature Coordinate System on the part. The most powerful function for "error correction and alignment" on the Fanuc 31i-B5 is called "Workpiece Setting Error Correction" (WSEC), and this function allows you to perform "true 6-degrees of freedom" error correction for parts which aren't 100% aligned to the machine's axes, and aren't sitting "perfectly" in space relative to the machine's center-of-rotation. It is more commonly used on 5-Axis machines, and might not be the greatest option for a 4-Axis Horizontal Boring Mill, because to correct for these alignment errors typically requires at least 2 rotary axes, but I would certainly look into getting Tilted Work Plane, as this will save you time, money, and aggravation. However, to take advantage of those codes, you'll need to purchase the options on the machine, have someone from Fanuc or the Machine Tool Builder come out and install, configure, and test those options, and you'll need a Post Processor which has been setup to output the correctly formatted G68.2 NC Code output. That will involve at least two purchases, likely a modified Post Processor, and the money to the MTB for upgrading your control functions/options. Plus the training on how to use all those options. I've certainly seen plenty of shops who still use the "old school" methods of calculating new Work Offset Positions, using G10 lines, from within Mastercam. This can be done "for free", if you learn how to properly edit your Post Processor, but it still takes effort to physically measure where the part is located on the machine, because you have to feed that data into Mastercam as "input", to get your Post to calculate the proper "output".

Leave everything where it already lies, and just create a new WCS Plane. Otherwise, no. You've got to "select" an entity, to move it. Or, you could create a "Level Set" > a Name that can be associated to a level, and you can use "All Level Set On" or "All Level Set Off". Or, you could enable and use "Viewsheets", where you are saving a 'Viewsheet bookmark', that has the part orientation, level visibility, active Plane, Geometry Attributes, Etc. This saves untold amounts of time, as you can simply setup multiple viewsheets, for different groups of levels, orientation/zoom, planes, everything. So, switching from OP 10, to OP 20, to OP 30, etc. is super easy.

Another approach is to "turn the visibility of all levels" to "On". (Make all levels visible.) Then, use the "only display associated geometry" button in the Toolpaths Manager. Then, click on an individual toolpath. This will "hide" all other geometry, and only display the geometry which is "associated back to that operation". I like to "select that operation geometry" (regardless of "how you select it"), and then "turn off > display associated geometry". This will leave all entities visible on the screen, but now you've "selected" the associated geometry. Now, you can press "ALT + E" on the keyboard, and this will temporarily "hide" all unselected geometry, and only leave the geometry which was selected, displayed on your screen. Now you can examine this geometry, in detail, and decide if you want to move it to another level, or what. Finally, when you are done, you can now press "ALT + E" again, and then bring all the visible geometry back visible. (Finally, manipulate your level visibility as needed to restore what you want visible on the screen...)

If you go to your "Home Ribbon" the "Statistics" command will only work on "visible entities". So, make whatever level you want to query "visible" and make all other levels "invisible", and then run the "Statistics" command.

This is where the automation in Hole Axis can really be beneficial. > Set a color for a give hole size/type. For example, I picked Green for my 1/4-20 tap drill sized holes. >> [CTRL + Click], to select all holes of matching diameter. (I have my lines set to create a point at the bottom only, and extend 0.500 above, and either "at depth" or "by a certain amount for Thru holes". >> Press Apply to finish creating these line/point vectors for a given hole diameter. > Right-Click in the Graphics Window, and change your color to something else. (Blue, Red, Orange, Etc.) >> Repeat the process, using [CTRL + Click] to select the net set of matching diameters. NOTE: You can also [CTRL + SHIFT + Click] to select matching diameters and vectors (plane/direction). Makes it easy to generate dozens or hundreds of Hole Axis Line/Point sets when setting up drilling operations on a large solid model. I know you deal with parts that are way off the scale, that may have a couple thousand holes, so this may not be worth it with your workflow Ron, but considering how bad the results are when you must move the geometry, or the WCS Origin, it may be worth it in some cases to do the prep work up-front with Hole Axis, versus having a drilled hole axis reverse when you're already done with all the programming, and just trying to update the location on the machine...

Mastercam does not have "Relations" the way other CAD systems do. It is not Solidworks, Catia, NX, Creo, Etc. Create a Line where you want the Centerline, and change the "line style type" display attribute to "centerline". (Left click to select the line, then Right-Click, and use the Attributes bar, to change the Line Style in the drop-down menu.

No worries! If it makes you feel any better, I had to investigate to be sure on the 'sav_' variables, before I posted!

Hi John, The "sav_" Variables are all User Defined in the Post Instructions File (*.PST). All variables in MP (both Predefined and User-Defined), have a "Previous Variable Slot" that is created during initialization. If you define "my_var : 0", MP will create two slots in memory > "my_var", and "prv_my_var". It is the "prv_" prefix which gets automatically created for every variable. I would expect that somewhere within the Post the OP is referencing, that "sav_progno" was defined as a User Defined variable. (So, technically, there would be a 'sav_progno' and a 'prv_sav_progno' variable defined by MP, although it is often the case that the "previous" variable slot is never used by whomever wrote the Post...) Examples of User-Defined "Saved" variables: sav_spc : 0 #Save spaces sav_gcode : 0 #Gcode saved sav_absinc : 0 #Absolute/Incremental Saved Value sav_coolant : 0 #Coolant saved sav_frc_wcs : 0 #Force work offset flag saved

It is also what makes this forum so much fun. Sometimes I need a 10 minute break from dealing with the stress of my day job, so being able to "play" with something like this feels like a puzzle, and is a welcome respite from some of the things I have to deal with. Always nice to come into a test like this with an open mind, and be able to get a good result that helps someone learn. I'm not always successful, and in those case, there is often someone else who is, so I just end up learning something new from them instead.

I used Area Rough, with STL Stock. (Created an "extrude solid" to create the STL.) Try putting both in your "Downloads Folder", but you may have to re-pick the STL in the Operation. I had to use "Maximum Depth", to limit the toolpath to the final Z-passes, otherwise the path wanted to "round" the edges. Dynamic_face_Area-Rough.mcam Dynamic_face_stock.stl

Love it when new learning occurs! I updated my original response too, with a tiny bit of more info...

You must create your chain, with extra "broken endpoints", where you want to make the modifications manually. Chain the Contour path like normal, enter your operation data. Generate the path. Then, expand the tree for the Operation, click on the "Chain/Geometry Manager". In the Chain Manager, Right-Click on the Chain you want to modify. You'll find "Change at Point" in this right-click menu... You can do "all kinds of cool things" with Change at Point. You can "jump clamps", you can "turn sections of a path from feed to rapid motion (just be sure to switch back to "feed", you can invoke Canned Text, change spindle speed or feed, enter a Machine or Optional Stop, the list is pretty broad. This is a function that has been in Mastercam for 20+ years, but very few users are aware of it! I've taught some lessons on how to use it, and modify Canned Text output in the Post, to do some really trick customization...

To do this with finishing, I use "Change at Point" function, break the chain geometry before the corner, and use Change at Point to change the Feedrates on the chain itself. With 'Change at Point', this allows you to save those manual changes into the toolpath geometry, and then be able to make changes to the path, and still have the ability to regenerate your changes. (Still have to make the corner feed adjustments "manually" with Change at Point, if you want to change those sections.) This is a pain in some respects due to the manual intervention aspect, but allows you some serious control over the path results itself.

Not at all!

If you like the videos (there is a full MP 101 class I uploaded, plus other classes/videos), please like and subscribe! @colingilchrist6468

I recommend never using the Copy/Paste method from the "menu" if you right-click and let go to bring up the big menu in the Toolpaths Manager. Instead, left-click to "select" the operation(s) you want to copy, then Right-Click, and continue holding down the Right Mouse Button, as you "drag a copy of the folder". You'll notice if you continue holding down the button as you drag, that your "Cursor" has become a "little folder icon". Now, position your cursor on the Operation that you want to copy the operation after, and let go. A little menu with pop-up with 5 choices > Move Before, Move After, Copy Before, Copy After, and Cancel. Choose the option that works for you. This little "right-click, hold & drag" method works amazingly well, and you can choose between "moving or copying" operations. In addition, having that "Cancel" option can be a savior, because sometimes you can accidentally "drop the operation in the wrong location". Cancel allows you to stop the copy/move, and start over.

Really spectacular contribution to the community David! I second Ron's request to give everyone our thanks!

Since you're stepping down the pocket walls anyway, I'd recommend a Tangent Barrel Mill, instead of just a Tapered Endmill. Check out Moldino Gallea. Either of these tools would be perfect: GS4TN7.5-37.5R-TH3 GS4TN10-50R-TH3 The GS4TN10-50R-TH3, has a 50mm barrel radius, tangent to the 2mm tip radius. With this, you can increase the step-down by 5X compared to a standard ball, keeping the cutting on the barrel, until you get down to the fillet radius, and then you just use a standard stepover only in those areas. Unified 5X should fully support this Tool Type in Mastercam 2023... GS4TN Pages from gs4tn_e.pdf

Emuge, FTW!

By the way man, I loved "The Perfectionists"! Finally made the time to read through the last few chapters. I love his writing style, and the content. Great book. We should get together for lunch soon so I can return it to you.

This is where editing the Defaults File, and setting up a Defaults File > for each machine, where you edit the File Extension from '.mcam-defaults' > to '.mcam', then open the file inside Mastercam, you can then replace the "Default machine" in the Machine Group Properties, with your actual machine. This gives you the same coolant/drilling/misc value strings, available in the Defaults File. Then, just go through the Default Operations, and set all your desired starting values for the various toolpaths, especially Dynamic and Opti-Rough. So, as an example, if you had machines with different Accel/Decel parameters, and wanted your older machines to have a 350 IPM Backfeed, and the more advanced machines to use 875 IPM, you'd just setup different Operation Defaults Files. The Operation Default Files can be associated back to a Control Definition File, (Under the Files page), which means you can have different programming default options, when you use different Machine Definitions (and associated CD Files > pointing to customized Operation Default Files). Just be sure to edit both the actual name of the 'Mill_Inch.mcam-defaults', (make a copy first, then change the file name), then edit the file extension, open as a Mastercam File, then 'replace the machine definition inside this File, edit your Op defaults, (For example, I enable Coolant/After, turn on the Filter on all my operation types, and turn on things like Misc. Values to enable High-Speed output), and save the file. Finally, you need to go back to the Ops Folder, and modify the File Extension from '.mcam', back to '.mcam-defaults'.

Exactly. The idea is to fit a "radius" into the cut motion, without having to manually "trim back" the surface being cut, but I prefer to always "machine entire pass" like Ron, and manipulate the geometry if I need to do something special...