Any interest in working for NASA Goddard, in Greenbelt, MD? I can get you in the door for an interview, but not sure if you're interested in uprooting the family...

Yes, 100%. If you're asking the question, then I'm guessing you know the answer. Considering your experience, I know a broad swath of shops that would be paying $120K+ for your level of skills, but likely not in NH. I'm seeing top-level guys asking $125-150K, and getting it, depending on shop and location, for 5-Axis Programming. I know you do a lot with 4X Horizontals, but how is your 5X experience?

Where are you located? At 14-15 years of experience, I could see you getting up into the $100K+ range for sure, considering your 5-Axis Experience, but location, location, location! Any interest in going to work for NASA Goddard in Maryland? Would require relocation (if you aren't in that area), but I know they are looking for several 5-Axis programmers. Amazing shop and machines. They have kind of a weird arrangement in the shop, as they use a Contracting Service to place their shop employees, but the work is full-time, with benefits, and the positions are stable. The contract to manage the employees gets send out for competitive bid every 5-years, but whomever the new contract administration company is just hires on the existing employees, and you maintain your years of seniority once you get on board there. The shop manager is getting a promotion to director soon, and is constantly asking me if I have anyone to refer...

Here is a quick example of how to do this for changing "Z" to "W", on-the-fly using 'nwadrs' function in the Post. I only enabled this for canned cycles currently, but hopefully that gives you something to use as an example for future development. Check out the link in my signature to find videos on Post Processor Development, so you can learn how to do this yourself. (Lots to study!) VIPER 3X VMC - Copy.pst

Also, it would be helpful for you to learn and use "Incremental Depths" for chaining. The "Incremental Linking" option is not G90/G91. It refers to "incremental depth, based on geometry depth. This allows you to utilize "multiple chains", each at different depths, inside the same toolpath. The combination of "Absolute/Incremental" Linking in the path can be very powerful, depending on where your actual Top of Stock sits "in the Z dimension". One other thing I did was to use "Reference Approach & Retract Points", for different paths, based on the tool number repeating. So, for example, there were two paths using the same 1/2" diameter Bull Tool. I set a "3.0 Absolute" Approach Point in the first path, and a "3.0 Absolute" Retract Point in the 2nd path. Then, in each operation, disabled Clearance, and used a 0.25" Retract Height. This allows a "high approach and retract", at the first point where the tool is used, and the final retract when the tool goes home, but then "operation-to-operation" the tool only retracts up to a safe value as it repositions. I did this on the final two paths as well (same tool).

My installs go from X9 to 2023. Installing multiple versions is not an issue.

Check out this example. One thing I noticed is you aren't using any Filtering in your operations. You can really cut down on the amount of NC Code you're generating if you enable Filtering, especially on the Dynamic style toolpaths. DISTRIBUTION CAP 2ND OP_Dynamic-with-Filtering.mcam I used a combination of 3 chains: - machining region > what you want to "cut" - avoidance region > what you want the toolpath "to avoid" - air region > areas of the machining region that "are open for approach". Without using the combination of air & avoidance, the path can "wrap around" the edges of the open slot...

Attach a copy of your Post to this thread so someone can take a look. This is probably 5-10 minutes of work for me, and would be a good example for others, so I'd be happy to do it and share the results. Only for Canned Cycles? Always "W" motion for the cutting, with a Z pre-position? Easy to add a Z Position output before the Canned Cycle call. I would do that in 'ptlchg$' and 'psof$', by reading the value of a Miscellaneous Real Number, which would allow you to plug in a number in the Misc. Values, to trigger the output in the NC Code. (mr4$, or any of the other unused misc reals...) For the Canned Cycle itself, you should use the 'nwadrs' function to "rename the prefix string" from Z to W, inside the canned cycle. (Then, in the Canned Cycle Cancel Post Block, use 'nwadrs' again to switch output back to Z.) 'pretract' and 'peof$' are where the retract cycles occur, so that would be easy to edit. Do you always want "Z0. W0." on every G91 G28 line, or only when a Canned Cycle was used? If always, that is super easy. If "only on the canned cycle", still easy, but would require setting a "flag variable" in the Canned Cycle Common block, to trigger the "W0." output on the retract/home line.

Try adding "an initial point segment" to whatever you want to be your Retract Height (peck clearance), then add your Pecking section. But you'll end up pecking through air if you do it this way. The Peck portion of the cycle doesn't seem to obey the Linking Parameters. I just added an initial point of "0.5", then used a Peck Cycle drilling to -1.0 inches, a fast-feed move to move down to -2.5 for flange drilling, then a deeper peck cycle with full retract from Z-2.5 to Z-3.5. Here is the output: N100 G20 N110 G0 G17 G40 G49 G80 G90 N120 T62 M6 N130 G0 G90 G54 X0. Y0. A0. S2139 M3 N140 G43 H62 Z5.5 N150 Z1. N160 S500 M3 N170 M8 N180 G1 Z.5 F200. N190 S2000 M3 N200 Z.4 F15. N210 G0 Z.5 N220 Z.41 N230 G1 Z.3 F15. N240 G0 Z.5 N250 Z.31 N260 G1 Z.2 F15. N270 G0 Z.5 N280 Z.21 N290 G1 Z.1 F15. N300 G0 Z.5 N310 Z.11 N320 G1 Z0. F15. N330 G0 Z.5 N340 Z.01 N350 G1 Z-.1 F15. N360 G0 Z.5 N370 Z-.09 N380 G1 Z-.2 F15. N390 G0 Z.5 N400 Z-.19 N410 G1 Z-.3 F15. N420 G0 Z.5 N430 Z-.29 N440 G1 Z-.4 F15. N450 G0 Z.5 N460 Z-.39 N470 G1 Z-.5 F15. N480 G0 Z.5 N490 Z-.49 N500 G1 Z-.6 F15. N510 G0 Z.5 N520 Z-.59 N530 G1 Z-.7 F15. N540 G0 Z.5 N550 Z-.69 N560 G1 Z-.8 F15. N570 G0 Z.5 N580 Z-.79 N590 G1 Z-1. F15. N600 G0 Z.5 N610 G1 Z-2.5 F200. N620 Z-2.6 F15. N630 G0 Z-2.5 N640 Z-2.59 N650 G1 Z-2.7 F15. N660 G0 Z-2.5 N670 Z-2.69 N680 G1 Z-2.8 F15. N690 G0 Z-2.5 N700 Z-2.79 N710 G1 Z-2.9 F15. N720 G0 Z-2.5 N730 Z-2.89 N740 G1 Z-3. F15. N750 G0 Z-2.5 N760 Z-2.99 N770 G1 Z-3.1 F15. N780 G0 Z-2.5 N790 Z-3.09 N800 G1 Z-3.2 F15. N810 G0 Z-2.5 N820 Z-3.19 N830 G1 Z-3.3 F15. N840 G0 Z-2.5 N850 Z-3.29 N860 G1 Z-3.4 F15. N870 G0 Z-2.5 N880 Z-3.39 N890 G1 Z-3.5 F15. N900 G0 Z-2.5 N910 M09 N920 G1 Z1. F300. N930 G0 Z5.5 N940 M5 N950 G91 G28 Z0. N960 G28 X0. Y0. A0. N970 M30 %

#1 recommendation I have is this > Read the manual for your machine. Every machine/control combination is slightly different, and I am always shocked and amazed by how many people have only ever been "told what to do by the other people in their shop", as the only form of training. The manual will explain cutter compensation, for both Diameter/Wear, and TLO (Tool Length Offset). Not sure what kind of machines you've got, but if you have any Haas machines, they have a ton of fantastic documentation online for beginners. Even if you have other machine types, their "Programming Workbooks" are a great wealth of beginning practical knowledge for milling and turning machines. They also publish an "Answers Book", which is helpful for double checking your own work. https://www.haascnc.com/content/dam/haascnc/en/service/manual/operator/english---mill-ngc---operator's-manual---2021.pdf https://www.haascnc.com/content/dam/haascnc/en/service/manual/operator/english---lathe-ngc---operator's-manual---2021.pdf https://www.haascnc.com/content/dam/haascnc/en/service/reference/programming-workbooks/mill---programming-workbook.pdf https://www.haascnc.com/content/dam/haascnc/en/service/reference/programming-workbooks/mill---programming-workbook---answers-book.pdf https://www.haascnc.com/content/dam/haascnc/en/service/reference/programming-workbooks/lathe---programming-workbook.pdf https://www.haascnc.com/content/dam/haascnc/en/service/reference/programming-workbooks/lathe---programming-workbook---answers-book.pdf

I built a Post for a SY-3040TG-5X when I was working at Methods Machine Tool. Not sure who you purchased the machine from, but the machine itself wasn't difficult to configure using the Generic Fanuc 5X Mill Post (although admittedly, I've been building Posts for a long time). Your best bet would be to contact your Reseller and have them build a Post to your requirements.

For anything off center, my preference is Y+X+Planes. Sometimes, that just doesn't work due to a lack of Y-Axis travel, and you end up with a situation where rotating in C and using X, is the only option, and this is where Polar Coordinates really work well. When using Helix Bore, you must use the "Perpendicular Entry" checkbox, if you want to use Cutter Compensation, and "start/end at center". This will give you a move to the hole center, then a line move to the start of the perpendicular entry, and finally a perpendicular line move which is also where Cutter Comp is instantiated. Cartesian to Polar Transformation (G112) Cartesian to Polar coordinate programming converts X,Y position commands into rotary C-Axis and linear X-axis moves. Cartesian to Polar coordinate programming greatly reduces the amount of code required to command complex moves. Normally a straight line would require many points to define the path, however, in Cartesian, only end points are necessary. This feature allows face machining programming in the Cartesian coordinate system. C-Axis Programming Notes Programmed moves should always position the tool centerline. Tool paths should never cross the spindle centerline. If necessary re-orient the program so the cut does not go over the center of the part. Cuts that must cross spindle center can be accomplished with two parallel passes on either side of spindle center. The G112 code is intended to be used with a Lathe using the C-axis and Live Tooling to program cutter anywhere along a non-rotating part. The G112 code allows 3-D contouring using the X, Y, and Z axes. The tool centerline programing (G40) and cutter diameter compensation (G41/G42) are available with G112. They are also available for a tool in any of the three plane selection (G17, G18, G19). A Lathe with Y-axis can use G112 and it can be useful to extend the range of travel of the live tool all the way across a part. Circular motion (G02 and G03) in any of the three planes (G17, G18, G19) are also available with G112. Since the spindle is not turning in G112, “feed per inch” (G98) must be selected. Once G112 is active, all motions are programmed with XYZ and C cannot be used. All X values are in radius when using G112.

Give this a look, and see what I did to get Y-Axis output, and where C-Axis Polar Conversion really shines on the big center hole. C-Axis and Y-Axis Output including Polar Example for Haas ST Lathe example.mcam If you need to Mill on your Y-Axis Lathe, just do yourself a favor and completely skip the C-Axis Paths. Use a Mill Path, set the proper planes, and you'll get much better results and control.

Something like this: % O0000 (Y-AXIS WITH ROTATED PLANES) (DATE=DD-MM-YY - 17-10-22 TIME=HH:MM - 15:20) (MCAM FILE - C:\TEST\TEST_CAXIS.MCAM) (NC FILE - C:\USERS\CGILCHRIST\ONEDRIVE - PHIL...\Y-AXIS WITH ROTATED PLANES.NC) (MATERIAL - STEEL INCH - 1030 - 200 BHN) G20 (TOOL - 1 OFFSET - 1) (.375 ENDMILL) (STANDARD C-AXIS OUTPUT) G28 U0. V0. W0. G50 X20. Y10. Z10. T0101 M154 G97 P1333 M133 G98 G17 G00 Z.5 C0. X6.5 Y0. M14 Z.1 G01 Z0. F25. G41 X6.5541 Y-.0156 F6.67 X6.5229 Y-.0427 G03 X6.6082 Y-.0313 I.0157 J.0271 Z-.03 I-.0541 J.0313 Z-.06 I-.0541 J.0313 Z-.09 I-.0541 J.0313 Z-.12 I-.0541 J.0313 Z-.15 I-.0541 J.0313 Z-.18 I-.0541 J.0313 Z-.21 I-.0541 J.0313 Z-.24 I-.0541 J.0313 Z-.27 I-.0541 J.0313 Z-.3 I-.0541 J.0313 Z-.33 I-.0541 J.0313 Z-.36 I-.0541 J.0313 Z-.39 I-.0541 J.0313 Z-.42 I-.0541 J.0313 Z-.45 I-.0541 J.0313 Z-.48 I-.0541 J.0313 Z-.51 I-.0541 J.0313 Z-.54 I-.0541 J.0313 Z-.57 I-.0541 J.0313 Z-.6 I-.0541 J.0313 Z-.63 I-.0541 J.0313 Z-.66 I-.0541 J.0313 Z-.69 I-.0541 J.0313 Z-.72 I-.0541 J.0313 Z-.75 I-.0541 J.0313 Z-.78 I-.0541 J.0313 Z-.81 I-.0541 J.0313 Z-.84 I-.0541 J.0313 Z-.87 I-.0541 J.0313 Z-.9 I-.0541 J.0313 Z-.93 I-.0541 J.0313 Z-.96 I-.0541 J.0313 Z-.99 I-.0541 J.0313 X6.5 Y.0625 Z-1. I-.0541 J.0313 J-.0625 F2. X6.4376 Y.0313 J-.0312 G01 G40 X6.5 Y0. G00 Z.5 (STANDARD C-AXIS OUTPUT) M15 C90. M14 Z.1 G01 Z0. F25. G41 X6.5541 Y-.0156 F6.67 X6.5229 Y-.0427 G03 X6.6082 Y-.0313 I.0157 J.0271 Z-.03 I-.0541 J.0313 Z-.06 I-.0541 J.0313 Z-.09 I-.0541 J.0313 Z-.12 I-.0541 J.0313 Z-.15 I-.0541 J.0313 Z-.18 I-.0541 J.0313 Z-.21 I-.0541 J.0313 Z-.24 I-.0541 J.0313 Z-.27 I-.0541 J.0313 Z-.3 I-.0541 J.0313 Z-.33 I-.0541 J.0313 Z-.36 I-.0541 J.0313 Z-.39 I-.0541 J.0313 Z-.42 I-.0541 J.0313 Z-.45 I-.0541 J.0313 Z-.48 I-.0541 J.0313 Z-.51 I-.0541 J.0313 Z-.54 I-.0541 J.0313 Z-.57 I-.0541 J.0313 Z-.6 I-.0541 J.0313 Z-.63 I-.0541 J.0313 Z-.66 I-.0541 J.0313 Z-.69 I-.0541 J.0313 Z-.72 I-.0541 J.0313 Z-.75 I-.0541 J.0313 Z-.78 I-.0541 J.0313 Z-.81 I-.0541 J.0313 Z-.84 I-.0541 J.0313 Z-.87 I-.0541 J.0313 Z-.9 I-.0541 J.0313 Z-.93 I-.0541 J.0313 Z-.96 I-.0541 J.0313 Z-.99 I-.0541 J.0313 X6.5 Y.0625 Z-1. I-.0541 J.0313 J-.0625 F2. X6.4376 Y.0313 J-.0312 G01 G40 X6.5 Y0. G00 Z.5 (STANDARD C-AXIS OUTPUT) M15 C180. M14 Z.1 G01 Z0. F25. G41 X6.5541 Y-.0156 F6.67 X6.5229 Y-.0427 G03 X6.6082 Y-.0313 I.0157 J.0271 Z-.03 I-.0541 J.0313 Z-.06 I-.0541 J.0313 Z-.09 I-.0541 J.0313 Z-.12 I-.0541 J.0313 Z-.15 I-.0541 J.0313 Z-.18 I-.0541 J.0313 Z-.21 I-.0541 J.0313 Z-.24 I-.0541 J.0313 Z-.27 I-.0541 J.0313 Z-.3 I-.0541 J.0313 Z-.33 I-.0541 J.0313 Z-.36 I-.0541 J.0313 Z-.39 I-.0541 J.0313 Z-.42 I-.0541 J.0313 Z-.45 I-.0541 J.0313 Z-.48 I-.0541 J.0313 Z-.51 I-.0541 J.0313 Z-.54 I-.0541 J.0313 Z-.57 I-.0541 J.0313 Z-.6 I-.0541 J.0313 Z-.63 I-.0541 J.0313 Z-.66 I-.0541 J.0313 Z-.69 I-.0541 J.0313 Z-.72 I-.0541 J.0313 Z-.75 I-.0541 J.0313 Z-.78 I-.0541 J.0313 Z-.81 I-.0541 J.0313 Z-.84 I-.0541 J.0313 Z-.87 I-.0541 J.0313 Z-.9 I-.0541 J.0313 Z-.93 I-.0541 J.0313 Z-.96 I-.0541 J.0313 Z-.99 I-.0541 J.0313 X6.5 Y.0625 Z-1. I-.0541 J.0313 J-.0625 F2. X6.4376 Y.0313 J-.0312 G01 G40 X6.5 Y0. G00 Z.5 (STANDARD C-AXIS OUTPUT) M15 C270. M14 Z.1 G01 Z0. F25. G41 X6.5541 Y-.0156 F6.67 X6.5229 Y-.0427 G03 X6.6082 Y-.0313 I.0157 J.0271 Z-.03 I-.0541 J.0313 Z-.06 I-.0541 J.0313 Z-.09 I-.0541 J.0313 Z-.12 I-.0541 J.0313 Z-.15 I-.0541 J.0313 Z-.18 I-.0541 J.0313 Z-.21 I-.0541 J.0313 Z-.24 I-.0541 J.0313 Z-.27 I-.0541 J.0313 Z-.3 I-.0541 J.0313 Z-.33 I-.0541 J.0313 Z-.36 I-.0541 J.0313 Z-.39 I-.0541 J.0313 Z-.42 I-.0541 J.0313 Z-.45 I-.0541 J.0313 Z-.48 I-.0541 J.0313 Z-.51 I-.0541 J.0313 Z-.54 I-.0541 J.0313 Z-.57 I-.0541 J.0313 Z-.6 I-.0541 J.0313 Z-.63 I-.0541 J.0313 Z-.66 I-.0541 J.0313 Z-.69 I-.0541 J.0313 Z-.72 I-.0541 J.0313 Z-.75 I-.0541 J.0313 Z-.78 I-.0541 J.0313 Z-.81 I-.0541 J.0313 Z-.84 I-.0541 J.0313 Z-.87 I-.0541 J.0313 Z-.9 I-.0541 J.0313 Z-.93 I-.0541 J.0313 Z-.96 I-.0541 J.0313 Z-.99 I-.0541 J.0313 X6.5 Y.0625 Z-1. I-.0541 J.0313 J-.0625 F2. X6.4376 Y.0313 J-.0312 G01 G40 X6.5 Y0. G00 Z.5 M155 M135 G53 Y0. G53 X0. G53 Z0. M30 %

% O0000 (T) (DATE=DD-MM-YY - 17-10-22 TIME=HH:MM - 14:54) (MCAM FILE - T) (NC FILE - C:\USERS\CGILCHRIST\ONEDRIVE - PHILLIPS CORPORATION\DOCUMENT...\T.NC) (MATERIAL - STEEL INCH - 1030 - 200 BHN) G20 (TOOL - 5 OFFSET - 5) ( 1/4 SPOTDRILL) T0505 M154 G97 P1069 M133 G98 G18 G00 G54 Z-.8124 C60.44 X4.85 X1.85 G241 X.6 R1.85 F1.07 Z-.7905 C119.543 Z-.7832 C208.199 Z-.8124 C291.929 G00 G80 X4.85 M155 M135 G53 Y0. G53 X0. G53 Z0. M30 % Generic Haas ST 4X MT_Lathe (2).mcam-content I downloaded the Generic Haas ST 4X MT_Lathe Post (mcam-content) files from the Tech Exchange. Creating a Radial Drill path, using a Mill Drilling path, and Axis Substitution, gives G241 for the radial drilling path, plus the proper start/end codes for Live Tool Drilling. That is the 2022 version. Let me know if you need a different release. Downloading takes just a minute. For the "mcam-content" file, you open up the Mastercam version, and just "drag and drop" the mcam-content file into the graphics window. It will (rather painlessly) install the MD/CD in the correct CNC Machines Folder, and put the Post in the Lathe/Posts folder auto-magically for you.

What kind of machine do you have? Let's start there. There are some free posts available on the Mastercam Tech Exchange, and the MPLMaster Post is available on this website, and does a bang-up job for Fanuc-Style machines, but customization is of course required, depending on machine type. (Mostly, just updating the correct M-Codes, and Drill Codes, stuff like that...)

Multi-Axis Operations are using Moduleworks paths, so they are likely not being calculated correctly through the MP.DLL post engine. Hmm. Try posting out the raw NCI Data, and looking at the 1014, 1016, and 1027 data lines. Are the values correct there, or are they signed differently from what is being entered into your Construction Plane dialog box for Plane Origin? If the values are correct in the NCI, but the predefined variables are not being populated correctly, it is possible to capture the values using 'pparameter$' Post Block, and manipulate/calculate whatever you need. (But, obviously more work, and not convenient.) Can I ask "why the Construction Plane Origin", and not the "Tool Plane Origin"? Typically, Construction and Tool Planes would be set identically, but curious if you are setting them identically, or differently? Do you need values ahead of every operation? There could be some options, although not ideal, by using 'Misc. Real Numbers' in the Operation, to pass XYZ Data, or, by using the Manual Entry Toolpath, to pass comments or NC Code to the Post. (Need to modify the Comment handling, to store Operation Comments, and suppress output, until the correct time, but this solution presents many opportunities to directly code data into your Toolpaths Manager, and get the output you need where you want it. Doing this "programmatically" is the best solution, but might be more work dealing with Vector/Matrix math and Parameter Post Blocks, versus just adding Misc. Reals or Manual Entry.

Axis Substitution is only for "wrapping about a cylinder", not for machining on the face of a part. Three different ways to approach this, depending on what you prefer: Standard C-Axis Path (XZC output) Y-Axis output (G17 + XY moves, with G02/G03 Arcs), typically my preferred method, as you can use Cutter Compensation Mill Cycle Conversion > G112 Polar Milling on Face, G107 Cylindrical Milling on Diameter To use Y-Axis output, AHarrison is correct, you'd need to make two different planes, each a rotation of "Right", so the C-Axis Start Angle would put the arc on the X-Centerline. Should be able to build these very quickly with Dynamic Planes. Mill Cycle Conversion G112 would be the "easy button", provided your Post is setup correctly. Use a "Mill Toolpath" (I prefer Circle Mill, since you're just cutting holes.) Typically, 'miscellaneous integer #4' is setup to activate the G112/G107 output.

Operation Defaults File > controls what "settings" are used for defaults in your Operations. Load your Wire Machine in your Toolpaths Manager. > Open Machine Group Properties > Files Tab > Click on the [ ! ] Button, for Operation Defaults. > Mastercam opens an "Edit Operations Defaults" window, which looks like an Operations Manager. > Expand "Wire - Contour", and press "Parameters". > Click on Wire/Power in the Tree. By default, the "associate to library" checkbox will be grayed out. Use the [ ! ] button to browse for a Power Library. (If you are sent to "CNC Machines", navigate up one folder, and go to > Wire/Power folder, then pick your Power Library. > After selecting the Library, the "associate to library" box will be usable. Check the box. > Uncheck "Wire", "Power", and "Fill Tank". > Green Check to close the (default) Operation, and Green Check to close the "Edit Operation Defaults" box. Now, try creating a new Wire Contour path, and those options will be set as the default configuration.

I would suggest building a Master Tool List, and forcing your programmers (you?) to always use the "Tool List Tool Number", rather than always renumbering every job as T1-Tx. (T1-T40, T1-T28, etc.) When you create a tool assembly, and that gets loaded in your Tool Magazine, it should always be that combination of Holder + Tool + Stickout, so you can rely on that tool not only "being there" in your magazine, but also that it is defined and built to match the Tool Assembly in your database. You can build a master library in the Tool Manager (.tooldb) in Mastercam, or you can build one using Excel, but someone has to manage and maintain that list. The moment you get a cowboy who makes a swap/substitution, because "that holder wasn't available", or another excuse, you're running the risk of a collision or scrapped part, because the proper Tool Assembly wasn't being used. For "common tools", which get used across multiple jobs, or see heavy wear/use, consider using "backup or redundant" tooling (Tool Life Management), so you've got multiple of the same common tools. This way you're assured that even when "T10" has reached it's limit, that you've got T101, T102, and T103, with the exact same configuration (tool assembly) ready to go. The control will take care of grabbing the "fresh" tool, and should also grab the Tool Offset for the redundant tool, provided you are programming your Tool Length Offset values using the "H" value where the machine will actually "look up what tool is in use". (H99 or H999 on Fanuc machines.) I'd implement Tool Breakage Detection using your Tool Probe, so the tool is checked either before or after use. (Sometimes, both on a critical job/feature!)

I think I probably use a different workflow to find chains associated to an operation. This may or may not be helpful to you: First, I turn on the visibility of "all levels". Then I enable the "Display only associative geometry" button, and click on the operation I want to investigate. Clicking on the operation hides all "non-associated" geometry on the screen. The only geometry displayed is "attached to the operation". I window-select all the geometry, and then I disable the "Display only associative geometry" button. This leaves the "op geometry" highlighted (selected), but all other geometry not selected. I then press "ALT + E" for the Screen Hide command. All other geometry is temporarily hidden, and I can now use Analyze Entity Properties, to figure out what levels the geometry exists on. I will often select all the remaining (op) visible geometry, and then use Move Level command to place all the Operation's chains on a new level, or figure out what levels I want to remain visible so I can work with/on that geometry. Final step after working with the geometry is to press ALT + E one more time, to bring all the other geometry back to visible, and then choosing which levels I want to be visible in the Levels Manager. This also affects any chain, on a level where the visibility has been toggled, not just the chain you had selected. I had 3 levels with different chains (and other non-chained geometry). When having any chain highlighted in the Chain Manager, and exiting the dialog box, any chained geometry on those levels disappeared. Toggling visibility again restored the visibility of those levels.

I tested what you were referring to, and yes, I get the same behavior. If I open the chain manager with levels that are invisible, and highlight any chain in the manager, then turn on visibility of those levels, and exit the Chain Manager dialog box, then any chain geometry (multiple chains) on those "now visible levels", are not displayed. You either have to toggle the level visibility again, or run "Regenerate display list" command.

I always disable: > Glow Highlighting > Use stipple on solids/surfaces/meshes > Use dashed on wireframe These are some of the most performance killing eye-candy, and I prefer the simple yellow highlight of yore. I'm probably a luddite though...

Are you only looking for the Origin of the Construction/Tool Plane, relative to the Active WCS? Current Toolplane Origin Values are "relative to the Plane orientation", not the original WCS itself. The MP Language has some special variables to help you make sense of the Plane Origin. Check the variables for "Tool Plane Origin" > tox$ toy$ toz$ Those variables are the "unmapped origin values", which means the numbers are relative to plane, not the WCS. Look at these: tox4$ toy4$ toz4$ These variables should contain the "mapped" values, or the XYZ positions relative to the WCS Plane and Origin. For debugging purposes, just put the variable with a Tilde character on an output line, to see the value: ~tox4$, ~toy4$, ~toz4$, e$

It was great meeting you at the show Alex! James is a heck of a guy, and someone I really respect and admire. You two will get along great.