Robert, Good to hear things are working well for you ! You could determine the actual character hidden in that "square" by looking at the NC file in an editor capable of viewing in Hex mode. If you do not have that Hex viewer capability, try the two (semi-educated guesses) shown below first... Usually the control characters you would see at the end of a program for these older machines would be either: [ESC] or [ctrl-D] To output a raw character value in an MP type post you enter the control character's decimal value on a line by itself. In the PEOF (end of file) postblock try these ->> code: peof # End of file for non-zero tool n, "M30" # or "M02" here 27 # Outputs an [ESC] character -or- peof # End of file for non-zero tool n, "M30" # or "M02" here 4 # Outputs a [ctrl-D] character

Each punched row (across the tape) takes up 1 byte of memory. If my memory serves there are 10 punches per linear inch of tape. So, 120 bytes of information per foot of tape. One kilobyte is 1024 bytes, so 1024 / 120 = 8.53333... feet of tape.

You can usually get away with taking a v7 post that was updated to v9 using the UPDATEPST9 utility and still use it under Mill v7.2 Note that you usually CANNOT take a post that came on the v9 CD and run it under a previous version of MC! Also, the UPDATEPST9 utility always makes a backup of the PST & TXT files that were updated. So you could look for the .PV7 and .TV7 files. (note the filename extensions) The same holds true for v8.1 Instead of .PV7 & .TV7 files, they will be .PV8 & .TV8 Just rename the .PV7 to .PST and the .TV7 to .TXT and you have your original v7 post processor. [ 09-27-2002, 03:46 PM: Message edited by: Roger Martin from CNC Software ]

The NCI2.NXT file is NCI type data. This file is created whenever you post process with a post that has the "getnextop" setting enabled. getnextop : 1 #Build the next variable table In Mill and Lathe, this allows access to these "next" variables -> nextop, nextplane, nextccomp, nextdc, nextxc, nextyc, nextplane, nextx, nexty, nextz, nextu, nextv, nextw and nextcflg For Wire, the "next" variables are -> nextop, nextccomp, nextdc, nextx, nexty, nextxc, nextyc, nextwt, nextwt_immd, nextwc and nextcflg.

Just copy your PST (posts) and their .TXT files into the new MCAM9|MILLPOSTS folder. Start v9, and from Main menu select -> NC Utils, Post Proc, Update PST On the screen that appears make your setting telling it what type of post it is updating Mill/Lathe/Wire and which version the post is from. Then enter the PST filename and click the Update button. The .PST & .TXT files are now updated for use with Mastercam v9.

Rick, Not sure what you have going on. If you could upload the MC9 file and your post (PST file) to the forum FTP site, it should not take more than a few minutes to figure out. If you have a HELIX involved in the entry/exit, that could get broken up by the post processor. Check for this in your PST file -> helix_arc : 2 #Support helix arcs #0=no, 1=all planes, 2=XY plane

gstephens, That was part of the problem. Note that (starting) in Mill v9 you have the Total Tolerance button with that value next to the button. This is probably the value you REALLY want. Retrieving the CUT Tolerance value from the .OPS parameters (parameter #10204) will fine as long as yo do NOT have the toolpath filter active. CUT Tolerance = Total Tolerance is THIS case. If the filter is active, getting #10204 will get you the CUT Tolerance, which now is NOT the Total Tolerance value. If the filter is active, you need to add the FILTER Tolerance & CUT tolerance values together to get the value that will now show up for Total Tolerance in the toolpath dialog. Explaining it all here would not be too useful for most. (Mr. gstephens being an exception!) If someone is really interested is how to do this in a post processor - please post a reply. I can do up a simple sample PST that shows how to do this.

You need to determine the "name" of the function to know what name to give your icon (.BMP file) First, goto Screen->Configure->Toolbar/Keys Find the function you want in the list. Now assign that function to an unused Toolbar position (Click the Add button under "Current Assignment")and select an unused ToolBar position. (Note the 'B' number!). Now exit config. and save the MILL9.CFG file. Load the MILL9.CFG file into a text editor and search for the ToolBar 'B'utton number you used. (example -> B85) Note the 'name' after the question mark on that line -> 2385. (B85) assignment? tsfbnd That is the name you must use for your .BMP icon file!

Henry, Since the response is a bit long, I uploaded a Forum_Post_Question.TXT file to the forum FTP site in the "Text_&_post_files_&_misc" folder.

Oppiz, Adding the 'Z' parameters is a simple procedure. What I've found is most people do NOT want these settings output by the post. Yes, at first they wanted them, but after had me remove them from the post output. (This happened many times). They want to be sure that who ever sets up the machine enters these settings, since he is the one you KNOWS what they actually are for the setup he is doing. If you really want them - email me.

quote: Its weird though, because should it be actually outputting the text thdxclr as well? Yes... If you output the value of a variable that does NOT have a "fmt" format assignment, the variable name is output just prior to the value held in that variable.

The value for "thdxclr" is from the Stock Clearance field on the Thread Cut Parameters page. So the question is - What value is in the "thdxclr" variable when you add it to "thdx1dia" ? If that looks good, make sure the "thdx1dia" is not getting re-calcuated else where in the PST. You can determine this by adding some temporary diagnostics into your post. Output the vaue of "thdxclr" just prior to your formula and check the value of "thdx1dia" immeadiately after the formula line -> "THRDXCLR = ", ~thdxclr, e # temp. postline thdx1dia = thdx1dia + thdxclr "THDX1DIA = ", ~thdx1dia, e # temp. postline Does the value if "thdx1dia" change from this point to when it is actually oputput for the threading cycle ?

Your feeds will post out as zero because of the output formatting assigned to the feedrate. Mill posts are setup for IPM feed mode (probably 1 or 2 digits to the right of the decimal). You plug in a feedrate of .005 IPR and the output in the NC file will be ZERO. If you cannot handle changing the formatting (It is not very difficult), contact your dealer. One important thing is - are you running ALL toolpaths in IPR mode? If you run milling paths in IPM and drilling in IPR the post work is more involved.

Try this. Menu select: Create, Point, Srf Project Then select your Surface(s) and/or Solid(s) Menu select: Done, Done It will ask you -> Want to select existing point entities? If you answer NO, you can then select positions by the usual methods (endpt, etc) Menu selects... Now you select the projection details/options. 'Make Pts' = Y Note that you can also output an APT file with the XYZIJK of these vectors. Set 'To file' = A Menu select: Do it

FYI, On Lathe v9 CD => MPLOKUMA.PST It may have the same name as the one on the v8 CD But it is NOT the same post. Give it a try...

You will need more than one variable for Feedrates if you want to be able to control the Plunge and Contour rates independently. This is not a difficult change to make. But, it may be a bit much if you are a rookie at altering post processors. Your Mastercam Dealer can help you out with this.

quote: Is it something to do with the format statement? Yes, it is. If you output the value of a variable that does not have a format assigned to it, the default format used is format #1. In this special situation the name of the variable is output along with it's value. One reason for this is to let you know that you have not done something you want to do -> assign a format to the variable. Assign a format to 'mr2', something like this -> fmt B 1 mr2 Note that this also gets you the letter 'B', so if you had "B" hard-coded in your PST, you will want to remove that.

For information on the post update process to v9, please go ->> Start, Programs, Mastercam abd select "Post Processors - What's new in v9" Whend the PDF opens, select the link -> "Post changes for FULL ARCS and HELIX ARCS capability in v9" This will jump you to -> "Using do_full_arc and helix_arc functionality" Updating a mill post from v8 to v9 using the update utility would not have changed the ability of the PST to cut "full circles". The new variables it adds to a mill post that are related to ARCs & HELIXs are -> do_full_arc & helix_arc With "do_full_arc : 0" in the PST, the post will act exactly like v8 when doing ARC motion. (In v8 you would NEVER get an ARC move that did 360eg. of sweep in a single NC block) With the setting above, v9 will act the same. A 360deg (full circle) in the toolpath will be broken into two 180deg motion blocks. To get HELIX motion to work in the post as it would in v8, make sure that "helix_arc : 2" is set in the PST. If you are not getting X,Y AND Z motion on the same circular block, the PST needs to be altered. Exactly what needs to be added/altered is dependant on your specific PST. It is a simple edit that you can try to do (make a BACKUP of your PST first!) or your Dealer can do this for you.

Could you be more specific?

thad, The "Reset post to default in file/get" checkbox option sets this line in the MILL8.CFG file -> 944. Always use default post processor? n Double check it by looking directly at the MILL8.CFG file. NOTE: If you ever directly edit a .CFG file (not recommended), Make SURE you have a backup copy BEFORE changing anything! Now check for a these lines in each of your two post (PST) files -> (Same note as above, have backups of these files BEFORE editing!) 76. Name of associated CFG file? 400. Name of associated CFG file? Make sure that there is NOTHING after the '?' mark in these lines. If there is something after the '?', just make note of it for possible future reference.

Jim, Is this a NEW Variaxis machine? Which controller is on it?

quote: I'm pretty sure the problem is some kind of tolerance setting in Mcam, Probably not, unless you have altered the default intsall tolerances. More information would be required to be able to assist. The two blocks shown look fine, but want is the X,Y position PRIOR to the first arc move? Take that location and draw it in MC. Then draw the X,Y arc endpoints and the arcs based on the NC code coordinates. Does this look like it should be "good" motion? Also, are you running comp in control ? If so, how much comp is in effect, offset to which side on these arcs?

Very strange... Does this occur with ANY MC9 file? What OS is on your computer? If you wish, you can e-mail me the MC9 file that causes this problem when trying to generate the .DOC setup sheet file. I also MUST have the .SET file that is being used. You can determine the .SET filename by -> Screen, Config, Files, highlite 'Setup Sheet Template' in the File Usage area, then read the File Name below.

quote: Settings are for .set setup sheet and is html in my config file. ??? Which option is set on your config on the NC settings page? 1> Post (uses .SET file) 2> Using Graphical Interface The '1' setting produces a text file (with a .DOC filename). The '2' setting produces an HTML file. Are you running Mill, Lathe, or???

quote: Is there any control that allows you to turn comp on in an arc move? Always assume you need a LINEAR move to activate/de-active comp. in the machine. On some machines that move must also be a G01 mode move. I've only ever seen one machine/control that SUCCESFULLY activated comp. on an arc move. I've had people tell me that their machine would, but many time it was just that the machine was not complaining about it - NOT that it was actually comping properly!