Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Colin Gilchrist

Verified Members
  • Posts

  • Joined

  • Last visited

  • Days Won


Everything posted by Colin Gilchrist

  1. 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.
  2. 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!)
  3. 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.
  4. 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.
  5. 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...
  6. 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$, e$
  7. 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.
  8. Look at the PDF for MP Post Ref Guide - Legacy Chapters > Rotary Processing This chapter covers: Rotary processing types Variables that control rotary processing Processing 4-axis motion Mastercam view matrixes Examples Processing 5-axis motion Matrix mapping Are you already familiar with Linear Algebra concepts, specifically Vector and Matrix mathematics?
  9. There is absolutely nothing wrong with this method of adding a blank line > " ", e$ However, it does add an extra ASCII blank space character to your NC Program. An alternate method of forcing the empty line, is to omit the string literal, and just "force" the end-of-line command (*e$) if prog_stop = 1, pbld, n$, *sm01, e$ if prog_stop = 2, pbld, n$, *sm00, e$ <<============ after *e$ #<======== That will force a blank line, with no space character.
  10. Hi Paul, Not sure why you'd be getting the different angular output between Probing and Drilling. That would really be a question for Renishaw and/or your Mastercam Post Developer. Is this a question of being "off" by 90-degrees, or 180-degrees for the C-Axis Rotation? If it isn't an easy answer like "90-or-180 degrees out", then I think it would warrant some investigation for Renishaw and the Post Developer. Have you looked in the RenMF File? (Renishaw Machine File = Renishaw Post). I know there are some unit vectors defined in that file, were the values are either "0", "1", or "-1", to defined rotary axis directions. Perhaps the unit vectors aren't setup correctly, which could be giving you a 90 or 180 degree shift in the C-Axis output. Are you using the "Miscellaneous Values" (Integers and Decimal Numbers), at the operation level, to control the rotary output? Could this be giving you a different output for the C-Axis when drilling? As a Test, can you program the Drilling Operation as a separate Operation, then take the Probing output you're testing, and edit the C-Axis value to match the Drilling Cycle output? If you hand-edit the code for testing purposes, does the Probing cycle now work as expected? All of the actual rotary axis angle output should be generated by the Mastercam Post Processor, not the
  11. Is your Post encrypted? Does it have both a PST portion, and a separate PSB portion? If the pwrtt$ with the dollar sign ($) being added, is giving you "duplicate Post Block errors", then you've likely got no access to 'pwrtt$'. Did you attempt searching for 'pwrtt$' in the Post, before adding a new section? It may be located in a different spot from where you are used to seeing it, unless it has been encrypted in the PSB seciton. If the section has been encrypted, you'll have to go back to whomever supplied you with the Post, to see if they can expose that section of code, or if they can give you a user-defined Post Block Call, that would be called from inside the encrypted 'pwrtt$' section, and thereby give you access to capture the parameter values, before writing them to the Buffer File.
  12. I had the same attitude which got me into Post Processor Development in the first place. I wanted my code to come out "edit-free", and eventually through learning about the MP Language, I was able to attain that and never looked back. Start with MPLMaster. Both MPMaster (Mill), and MPLMaster (Lathe) are excellent "base" Posts. They make take more initial "tweaking" versus the 2X Hitachi, but the 2X Post will not support 4-Axis output, including Y-Axis. The 4X Posts are much more involved and robust from a "plane handling standpoint". Both the Generic Fanuc 4X MT_Lathe Post and MPLMaster, are great starting posts, but MPLMaster is like a "beefed-up" version of Gen Fan 4X MT_Lathe.
  13. I've setup the Generic Fanuc 4X MT_Lathe Post, and/or MPLMaster, to fit a variety of custom machine and control configurations. M-Codes for machine mode activation, Axial and Radial Live Tool Canned Cycles, Pick-Off/Cut-Off to support all of the Part Handling code between Main and Sub Spindles, Part Flip, or Tailstock operation. Mori Seiki's, Hwacheons, Haas, Okuma, Mazak, Etc. I doubt there is anyone with a personal copy of a Post they have customized for this particular machine/control combination, who has: #1, seen this thread, and #2, is willing to share their work, but I wouldn't be surprised if either Postability, or In-House Solutions, has a post "off the shelf", which would support the basic options of your control. When I was working at CNC Software back in 2013, In-House Solutions was celebrating their "100,000th Paid Post Processor", so considering we're about 10-years on, I'd guess you could probably double that number. (*NOTE: I do not speak for, nor represent, CNC Software, In-House Solutions, or Phillips Corporation in making these comments, for which I'm solely responsible for here.) If you're interested in taking a stab at it yourself, check out my YouTube Channel in my signature. I've uploaded my Basic Mill Post Class (MP 101), 5X Post Class (MP 301), and the start of my Lathe Post Class (MP 201). This reminds me that I should finish uploading those videos...
  14. By the way, check out the link in my signature. I've got an entire Basic Post Processing Class which was recorded back in 2016, which I've uploaded to YouTube. Be sure to watch the "Office Hours" video sessions, where we are doing the bulk of the "hands on" post development work.
  15. Both of these lines: (TOOL - 1 OFFSET - 1) (RGH TURN .03R INSERT - CNMG-432) Are output by the call to: ptoolcomment ltlchg$ #Toolchange, lathe toolchng = one gcode$ = zero copy_x = vequ(x$) pcc_capture #Capture LCC ends, stop output RLCC c_rcc_setup$ #Setup LCC on first 60000 plcc_lead_begin #Save original in sav_xa and shift copy_x for LCC comp. pcom_moveb #Get machine position, set inc. from c1_xh c_mmlt$ #Position multi-tool sub, sets inc. current if G54... ptoolcomment <<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<< Both lines, are output from this subroutine (post block) call comment$ Inside 'ptoolcomment' > the output comes from the following Original Block: ptoolcomment #Comment for tool if tool_info = 1, [ tnote = abs(t$) toffnote = tloffno$ strtool$ = ucase(strtool$) stinsert2 = ucase(stinsert2) !spaces$ spaces$ = zero scomm_fx_arg = drs_str(2, tnote) + drs_str(2, toffnote) pcomment_out if posttype$ = two, #Lathe toolpath operation [ if tool_op$ = 64, [scomm_fx_arg = strtool$, pcomment_out] #Drill operation else, [scomm_fx_arg = strtool$ + " " + stinsert + stinsert2, pcomment_out] ] else, [scomm_fx_arg = strtool$, pcomment_out] #Mill toolpath operation spaces$ = prv_spaces$ ] Block, with Comments added for clarity: ptoolcomment #Comment for tool if tool_info = 1, [ tnote = abs(t$) toffnote = tloffno$ strtool$ = ucase(strtool$) stinsert2 = ucase(stinsert2) !spaces$ spaces$ = zero # ************ The two lines below, output the TOOL - 1 and OFFSET - 1 > scomm_fx_arg = drs_str(2, tnote) + drs_str(2, toffnote) pcomment_out # ************ This code block, either outputs "lathe drill" comment, or "lathe insert" comments if posttype$ = two, #Lathe toolpath operation [ if tool_op$ = 64, [scomm_fx_arg = strtool$, pcomment_out] #Drill operation else, [scomm_fx_arg = strtool$ + " " + stinsert + stinsert2, pcomment_out] ] # ************* This "else" block, outputs "Mill Tool Comments" else, [scomm_fx_arg = strtool$, pcomment_out] #Mill toolpath operation spaces$ = prv_spaces$ ] I didn't see originally that this was a Lathe Post. For Lathes (with milling capability), the 'psof$', 'tlchg$', and 'tlchg0$' blocks are expanded, to include separate "milling" and "turning" toolchange blocks: lsof$ > Lathe start-of-file (1st toolchange) ltlchg$ > Lathe actual tool change ltlchg0$ > Lathe Null Tool change (tool number repeats) msof$ > Mill start-of-file (1st toolchange) mtlchg$ > Mill actual tool change mtlchg0$ > Mill Null Tool change (tool number repeats)
  16. That should be where you want to add it. Basically > psof$ = "the 1st tool change operation" in the Post ptlchg$ = "the next 'actual' tool change operation ptlchg0$ = "null tool change, tool number repeats"
  17. I'd really need some more specifics of what you are trying to measure. Just the "diameter" of the counterbore (0.57186 hole), or are you trying to gauge "rotation" of the features in that pocket? I do not see a single "straight wall" in that pocket, just a series of tangent arcs, and the two "ramped surfaces" at the X- and X+ ends. Are you trying to determine the "size" of those features, or the angular rotation of the pocket as a whole? To determine "size", I'd suggest running a "3-point Bore" (O9823) Macro, on each of the 4 Lobes, at the pocket corners. You must perform "Vector Calibration", to have success measuring bores "not at the quadrant positions". An example, would be the lobe in the X+ Y+ quadrant. You could use A30., B60., and C90., to make 3 hits on that radius. (See Variable Outputs - Chart 2 > #188 = "feature size", in this case "diameter".) You could then save that output (#621 = #188), after executing the cycle, and then repeat the process, on the other 3 lobes, using #622 = #188, #623 = #188, and #624 = #188), where you are placing that equation just after each cycle being executed, to capture the results, for each probing cycle. NOTE: be sure you are cancelling "Block Lookahead", otherwise you won't get correct results. To cancel "lookahead", place > "G103 P1", just ahead of the equation. The G65 P9833 call should turn "lookahead back on". It doesn't hurt to place a "G103" on a line afterwards, just to be sure it is enabled. The code below only shows execution of a single cycle. You'd need to repeat this in at the 3 other lobes, and save #188 results to a unique variable. Then, afterwards, you can compare the results, and make a judgement on "do you need to adjust Cutter Radius Compensation values to make the feature "on size". G65 P9832 G65 P9810 X25. Y40. (GO TO CENTER OF 3-POINT BORE) G65P9810Z-10.F3000 (PROTECTED FEED TO DEPTH) G65P9823A30.B60.C90.D50. G103 P1 #621 = #188 G65P9810Z100. G65P9833 G103 G28Z100. english---renishaw-inspection-plus---programming-manual---2008.pdf
  18. The probe is driven from the spindle centerline, so there is no direct "callout" for the probe diameter. At least, not on the G65 Pxxxx Macro Call Line. Calibration on a Haas should be done through VPS, where you'll have a series of Templates to execute, and here is where you would enter the nominal Probe Stylus Diameter. Do not run "Complete Probe Calibration Macro". Instead, execute Calibration Macros 2, 3, and 4 (Tool Probe Calibration, Spindle Probe Length, and Spindle Probe Diameter), in order. You'll get more accurate results if you run all three sequentially, instead of running "complete probe calibration". On the Spindle Probe Diameter Calibration Macro Page (VPS), this is where you'll enter the Probe Tip Diameter, along with other calibration inputs. The "diameter" actually doesn't get stored. The Calibration Macros will calculate the Probe Radius, and store that value. The "variable ranges" are typically in the #500-#590 range of values. Should be #520-#527, or something like that, for where the actual calibration numbers are stored.
  19. You're welcome Josh. There is a ton of stuff that is possible with Prod+, but it requires education in how the product works. That education is best sourced from Renishaw, as Prod+ is a product produced by them, and integrated into Mastercam as an add-in. While CNC Software is familiar with how the system works, and is responsible for the integration into the Mastercam Interface, Renishaw are the ones who build the product and are the experts in Probing. Getting some training from Renishaw will pay huge dividends.
  20. What Post are you starting with? The variables for "comment start" and "comment end", are typically: sopen_prn & sclose_prn or scomm_str & scomm_end Example, change from this: sopen_prn : "(" #String for open parenthesis "(" sclose_prn : ")" #String for close parenthesis ")" To this: sopen_prn : '(MSG" ' #String for open parenthesis "(" sclose_prn : ')"' #String for close parenthesis ")" Example, change from this: scomm_str : "(" scomm_end : ")" To this: scomm_str : '(MSG" ' scomm_end : ')"'
  21. The advantage is simply the "existing mechanism" which exists inside MP-based Post Processors. There are 3 Canned Text Post Block Calls: pcan, pcan1, and pcan2. pcan = Canned Text "Before" (the tool change) > will output a line of code with standard architecture. This includes the call to 'pbld' to output Block Delete (if active), Sequence Number (n$ > only if active), the "canned text" (loaded in 'pcant_out'), and the End of Line (e$). pcan2 = Canned Text "After" (the tool change) > will output on a separate line, like 'pcan' does. pcan1 = Canned Text "With". This must be used in 2-parts. First, the "call" to 'pcan1' (generally at the start of the output line), and then the Post Developer includes 'strcantext' as an output parameter, generally at the end of the line of code. Because of the existing architecture, it allows the Post Developer to 'simply move the call to 'pcan', 'pcan1/strcantext', or 'pcan2', and the output location becomes very easy for you to "move around", to get exactly where you want it to occur. There is nothing inherently wrong with the way you may be utilizing Canned Text, but when you modify the 'pcant_out', you are simply changing how 'strcantext' gets loaded with output strings. Technically, you can even leverage Canned Text to "set variable values", or otherwise pass data to the Post, so you "as the developer", can do whatever you want with it. The biggest advantage to Canned Text, is the ability to trigger events "during the Toolpath itself". We typically do that with "chain-based" (Contour) paths, using the Chain Manager, Right-Clicking on a Chain, and using the "Change at Point" command. Here, you can either use Canned Text, Manual Entry, or just trigger changes like Rapid/Feed switching, Jumping Z-Height (super awesome for hopping over clamps), adding a Dwell Command, or modifying Feed or RPM values. The tricky part with modifying RPM/Feed or Feed/Rapid, is the changes are Modal. So, you generally need to make multiple changes at different points in the path, to get the output you desire. But it allows customizing "the motion" to a very high degree, with minimal Programmer inputs needed.
  22. Yes, it is certainly possible to add functionality from one Post, to another. You do need to know the architecture of the Post, as you generally can't just "copy and paste" Post Block Sections, because you need to know if there are variables which are shared across the original post and new "code sections" you're adding. Also, variables must be initialized and/or formatted, so there are often additional sections which must be copied, to support either Post Blocks, or sections of code being added to existing blocks.
  23. You should include the "top surfaces of the screw" in the Machining Geometry Selection. To control the depth of the 1st cut, you should be using the "Stock" page of the Rotary Advanced Toolpath, using a Stock Model, to represent the "current stock condition" of the part you are machining.
  24. What you want to setup is some logic that reads the value of "t$", and then outputs a different "block" of spaces, based on the knowledge of "how many digits is the numeric variable". This would be for "numeric variables only". For Strings, you can use the "String Length" function, to get the number of characters in the string, and then "append" (concatenate) additional space characters, to create output that maintains your "column spacing". Unfortunately, there is no way to control "starting column", as lines of G-Code are assembled, and "things added" to the string line (strings or numeric variables, with their associated prefix strings), one-at-a-time, until the line is forced out with the end-of-line variable (e$). ptspc #Post Block to pad Tool Variable Space Characters if t$ < 10, " " if t$ > 9 & t$ < 100, " " if t$ > 99, " "

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us