In the "Text_&_post_files_&_misc/" folder on the Fourm FTP site is -> MULTI_POST.ZIP This "post processor" method is similar to what Mick's VBS does, but done using a PST, in that you just define the string variables for the PSTs to be run.

If anyone is interested... It would be possible to create a special 'stripped' down PST that processes the SELECTED operations in the Operation Manager and processes that NCI file thru multiple PSTs. (Pumping the NC files out to separate directories) This would be an extension something I did that automatically created a Setup Sheet (using the .SET type setup sheet templates) immediately after the PST has created the NC file. You just posted your operations as usual and you got the .NC and a .DOC with no additional steps.

quote: Does not always work and you never know is it is the value you want I beg it differ - it always works and you do know what the value in the 'prv' variable is. A 'prv_[varname]' is automatically created by MP for every numeric variable. The prv_[varname] variable is always loaded with the value of the [varname] variable every time the value in [varname] is output to the NC file, or you can explicitly force this update from the value in [varname] to prv_[varname] by using the '!' prefix. Example: !xabs, *yabs Would copy the current value in 'xabs' into 'prv_xabs'. Note that using the '!' this update occurs WITHOUT any output being written to the NC file. 'prv_yabs' would also get loaded from 'yabs' in this example because it's value was FORCED to output to the NC using the '*' prefix.

quote: I understand it as a tolerance in the plane perpendicalar to the arc requiring a specified amount of movement to output the helical arc. You are correct. That is what it is. The motion distance in the plane perpindicular (the Z axis if doing a helix in the XY plane) that is required for the move to be considered a 'valid' helix move. On the helix motions where your Fadal dies, what is the motion distance in the perpindicular axis ? If it is too small, the machine may not like that. That is the reason for the HELIX_TOL post varible. Say that the Z axis is only going to move 0.0005" on a helix motion block. If HELIX_TOL is set to 0.001, the post should not output that helix move, but output just a std. arc motion on that block, since the Z motion is less than HELIX_TOL

Original Code... code: pccdia #Cutter Compensation #Force Dxx# tloffno40 = tloffno + 40 if prv_cc_pos <> cc_pos & cc_pos, prv_tloffno = c9k sccomp if cc_pos, tloffno40 #Changed from tloffno # Change "prv_tloffno = c9k" to be "prv_tloffno40 = c9k" Altered Code... code: pccdia #Cutter Compensation #Force Dxx# tloffno40 = tloffno + 40 if prv_cc_pos <> cc_pos & cc_pos, prv_tloffno40 = c9k sccomp if cc_pos, tloffno40 #Changed from tloffno #

May^Day, Are you going to the Buckley Old Engine Show this weekend ? Buckley Old Engine Show [ 08-15-2003, 09:07 AM: Message edited by: Roger Martin from CNC Software ]

What is the version of MP.DLL you are running? To determine the version of MP.DLL 1. Locate the desired file using Windows Explorer (in the Chooks folder of the Mastercam installation). 2. Right-click on the DLL file. 3. Select "Properties" off the drop-down menu. 4. Select the "Version" tab. 5. Select "File Version" in the "Items name" list. 6. Read the "Value" (to the right). quote: am also getting an error that reads "wrong direction on profile." What is giving you this error ?

My bad... This line in the sample MP_VBS.PST should read -> 91. Name of executable post processor? MP Once you make that change, I'm sure it DID strip the(COMMENTS)! Check the same directory where the your NC file was placed. By default the VBS script "dresses" the input NC filename with "CLEAN_" to create the filename for the NC file - with all (COMMENTS) stipped out. If your operations would be creating TEST.NC You will end up TEST.NC (un-altered) and CLEAN-TEST.NC (stripped of COMMENTS) Check the top of the VBS script for details on how you can alter this behaviour. [ 08-04-2003, 04:06 PM: Message edited by: Roger Martin from CNC Software ]

Rekd, RunVBS() is a "File FUNCTION", which means it has a return value ->> # Define a string that holds the name of the VBS script to be run. strVBS "c:mcam9vbstrip_comments.VBS" # Define a numeric variable to hold the value returned by the RunVBS() function. result : 0 #Run the VBS script (FULL Path/Name is required !) result = runvbs(strVBS)

Screen -> Configure -> NC Setting(tab) Look in the middle-right of the dialog for... Setup Sheet * Post (uses .SET file) * Using Graphical Interface If you select '.SET' type, you can specify the Setup Sheet template file (the .SET) under the Files (tab), look under File Usage and highlight 'Setup Sheet Template'. Now look below in the File name text box for the the ?.SET filename.

When discussing Setup Sheets, you need to let everyone know WHICH setup sheet generator you are talking about -> 1> the Graphic setup sheet option in MC 2> the .SET (post type) setup sheet option in MC 3> the HTML Setup Sheet (from In-House Solutions) The .SET type setup sheet generators for LATHE that shipped with MC v9+ DO output times -> (for each tool ->) Time for tool 2: 0 hours, 1 minutes, 24 seconds (and program total ->) Total time: 0 hours, 34 minutes, 41 seconds

MP v9.15 -> added the RunVBS() command and corrected a problem with the value of the pre-defined variable ARC_PITCH always being ZERO. 'rekd - Are you sure you are running MP.DLL v9.15? To determine the version of MP.DLL (or MPL.DLL, MPWIRE.DLL) 1. Locate the desired file using Windows Explorer (in the Chooks folder of the Mastercam installation). 2. Right-click on the DLL file. 3. Select "Properties" off the drop-down menu. 4. Select the "Version" tab. 5. Select "File Version" in the "Items name" list. 6. Read the "Value" (to the right). Check out the sample files in the "Run VBS sample.zip" located the 'VB_Scripts' folder on the Forum FTP site. The MPPARAM.DLL goes in the MAIN Mastercam directory, with MILL9.EXE (NOT in the CHOOKS!)

FYI, In MC v9.1 Create -> Next Menu -> Spirial/Helix

Harryman, As someone who as never used TextPad, I downloaded an eval. copy and in their Help is this -> ------------------ How to Use as the Editor for Other Applications TextPad can easily be used as the editor for other applications. By using its dynamic data exchange (DDE) capabilities, each file to be edited can be opened in a new window, rather than starting another copy of TextPad. The TextPad installation directory contains a program called DDEOPN32.EXE in the SYSTEM folder. This translates command line requests to open files into the appropriate DDE commands for TextPad. The first parameter must be the registered server name TextPad, and the second parameter is the file to open, with an optional line and column position immediately following in brackets. Example 1: To use TextPad as the editor for WinCIM 2, add the following line to the [General Preferences] section of WINCIM.INI: Text-Editor=C:Program FilesTextPadSYSTEMDDEOPN32.EXE TextPad Example 2: To use TextPad as the editor for WinGrep, add the following line as the editor command on its Configure dialog box: C:Program FilesTextPadSYSTEMDDEOPN32.EXE TextPad $f($l) Example 3: To use TextPad with Visual C++ 6, so that it edits the same active file as MSVC, customize the Tools menu of MSVC.EXE with the following command: Command Line: C:Program FilesTextPadSYSTEMDDEOPN32.EXE Menu Text: &TextPad Parameters: TextPad $(FilePath)($(CurLine),$(CurCol)) Notes: Whenever TextPad is reactivated, it checks the last modified date of each file that you are editing, and asks if it should reload any that have been changed by another application. ------------------ You can test this by creating a BATch file called TP.BAT that contains this one line -> "C:Program FilesTextPad 4SystemDDEOPN32.EXE" TextPad %1 Now open a DOS (aka CMD) command window, CD into the folder that contains the TP.BAT and type a command like -> TP C:TEMPMY_FILE1.NC [enter] This will fire up TextPad (if NOT already open) Now repeat the TP command using another filename -> TP C:TEMPMY_FILE2.NC [enter] TextPad will just open file file into the current session. Sounds straight forward and it is, EXCEPT when you get Mastercam involved. MC expects the specified Editor to be an EXE file. That combined with TextPad's requirement of having 'TextPad' as the first argument to the DDEOPN32.EXE, and you're stuck. (At least for a simple solution) --------------- As for columar editing - it definately is cool. I used Multi-Edit for years with this feature. Now use CodeWright, which also has this ability. You just right-mouse click (and hold the button) and mark your text!

Rekd, PATH, NAME and EXTENSION of the NC file -> "spathnc -> ", spathnc, e # NC file path "snamenc -> ", snamenc, e # NC file name "sextnc -> ", sextnc, e # NC file extension I assume that you are going to use the launch() command to fire off an EXE. Note that we now have the ability (from within a PST) to directly run a Mastercam VBS script. This is using a *NEW* runVBS() post command avaible in MP v9.15 By "directly", I mean that execution goes directly to the called script, no stopping at the 'VB Script Editor' dialog! [ 07-30-2003, 05:47 PM: Message edited by: Roger Martin from CNC Software ]

Have to tried the MPWSDMK30.PST on the CD ? Yes, it says it is for the "Mark 30", but I beleive the the programming is VERY similar to what the "LN1W" needs.

Dan, You cannot "add" additional Coolant options, but you can "change" any of the 3 Coolant type options in MC. Example: Make FLOOD become AIR, in the posted output AND in the screen selections in MC when a specific post processor is active.

There are several option switches in the MILL.SET # Post specific "switches" to allow turning ON/OFF the following functions -> # The 'xyz_limits' switch allows selecting WHERE to output this information. # Setting the 'xyz_limits' variable -> #xyz_limits = 0, Do NOT output ANY Max/Min X,Y,Z information. #xyz_limits = 1, Output Max/Min X,Y,Z info. ONLY for EACH tool (not Program) #xyz_limits = 2, Output Max/Min X,Y,Z info. ONLY for entire Program #xyz_limits = 3, Output Max/Min X,Y,Z info. for EACH tool AND Program xyz_limits : 2 # Output Max/Min X,Y,Z information, where?

quote: go the way of the turbo pascal WHAT! Turbo Pascal is gone ??? I'm always the last to know ! BTW, Who on the forum has had the priviledge to program with Borland Turbo Pascal v3. ? How about Borland Turbo 'C' v1.0

Bruce, quote: My problem is with the posts from mastercam The first step in finding a solution - is determing where the problem is. Is the problem the Post Processor (PST file)? Or the posted NC code? Yes, the PST produces the NC code, but if the data coming into the PST is not clean, the output will not be any better. Usually, if the PST is bad, your surface finish wouldn't be the problem - those big nasty gouges would! The problem may be the Post Processor or the surfaces, toolpath strategy, toolpath parameter settings, filtering settings, etc. If the toolpath is the problem, I'm sure there are surface toolpath experts here that can assist. Have you run this by your Mastercam Reseller ?

Try this... Go to the Screen, Configure, Communications page and un-check the "Read PST parameters (q.80-89)" option. With this option checked, MC reads the Post Numbered Questions "80. thru 89." in the active PST for the Comm. settings to use)

The setting to force the PST to linearize arc moves is -> linarc : yes # yes (or '1') = linearize ALL arcs # no (or '0') = leave the arcs alone! Most PST files do NOT have "linarc" defined in them, so you may need to add this declaration. Also, the Chordal Deviation (breakup tolerance) is controlled by the setting of -> vtol : 0.0002 Note the "vtol" usual IS defined in a PST Maybe more than once (for INCH/METRIC differences)

You can do that... Use the LAUNCH() command to start your "post" Post Processor EXE code: peof # This is the PEOF postblock that ALREADY exists in your PST n, pcooloff n, "M00" # ADDED CODE (START) # Define the full PathNmae of the EXE to be run strEXE "C:Mcam91CommonTempMY_SPECIAL_EXE" # This string will hold the built up PathName of the NC file created by the post. strfilename result : 0 # Needed for the 'launch()' command ppost # This posblock is called AFTER all the files from the PST run are closed! if not(fastmode), pdiags # This postblock is ONLY for explanation purposes ! strfilename = spathnc + snamenc + sextnc # Build up the PathName of the NC file result = launch(strEXE, strfilename) pdiags # This postblock is ONLY for explanation purposes ! *e "---------------------------------------------", e "DIAGNOSTIC outputs (for explanation purposes)", e "---------------------------------------------", e *e "PATH, NAME and EXTENSION of the NC file", e "spathnc -> ", ~spathnc, e "snamenc -> ", ~snamenc, e "sextnc -> ", ~sextnc, e *e # ADDED CODE (END)

Murlin, code: "Sorry Rodger, I didn't mean to offend by my use of the "B" word:)" No offense taken, it's just that if they IS a bug - I want to know about. That's the way to eliminate them! As for your post problem... I kind of see what you are taking about, but a real world sample to probably to much to clarify. Question about -> "Plane changes on a line by itself with no other G codes. Circular blocks as follows" This means NO G17,G18,or G19 plane code output is needed? If you could supply me with sample files -> 1> MC9 with toolpaths to process 2> The original NC output from your PST (with the 'bad' stuff) 3> The corrected NC file that works on your Big Blue Roger

quote: It has to do with me having Circular Interpolation turned on in the xz and yz axis in some of the toolpath algorythms. It is a....... *whispers*... "bug". Opps I said the "B" word:) Murlin, What "bug" are you referring to ? What version of MC are you running ? What would this script be fixing in the NC output from the post ?