To tell MC to use a .SET type setup sheet generator do this-> Screen->Configure->NC Settings Look for "Setup Sheet" in the middle-right of this dialog box. Check "Post (uses .SET file)" To check the name of the .SET file MC is going to use, check this -> Screen->Configure->Files Under File Usage select "Setup sheet template" below in the Filename field is the name of the .SET file that will be used. I believe that Router v8 shipped with a MILL.SET file in the POSTS folder and the configuration may specify ROUTER.SET has the name of the file MC is looking for. You can either; rename the MILL.SET to ROUTER.SET -or- change the configuration. If you still wish to use the Graphical Setup method AND the .SET method you can do this. Leave the configuration set on "Using Graphical Interface" and use the .SET just as a post processor (which it really is!) To make it easier to select this "post" you may wish to rename MILL.SET (or ROUTER.SET if that is what you have) to something like -> SS.PST

fs2 2 0.4 0.5 The 0.4 is the format used for INCH The 0.5 is the format used for METRIC If you want trailing zeros, you would make it -> fs2 2 0.4 0.5t Added the 't' to preserve trailing zeros.

You mean that now if you program a contour operation with the Plunge Feedrate and the cutting Feedrate different you never see the plunge rate output? If so... It would definitely be tough to guess at what is going on in your post, without seeing a copy of the PST along with a sample program.

This code sample is from what postblock ? (The devil is in the DETAILS when doing posts!) If you only want this to output on the fist tool of the program... Declare a variable to be a switch for this output. do_M58 : yes Now in your code, just check the setting of that variable -> code: if stagetool <= one & do_M58 = yes, pbld, n, "G58", e do_M58 : no # Turn OFF the switch

The PCOMMENT postblock is a 'special case'. You never want to call it directly from another postblock. You use the command variable COMMENT to initiate a call to the PCOMMENT postblock. Also, you cannot do any boolean formuals in the PCOMMENT postblock. If you need to have any logic testing, you would want to do that this way -> code: pcomment # COMMENTS output postblock (pre-defined) pcomment1 # just call our postblock pcomment1 # Only output COMMENT if from a 'real' toolchange if gcode = 1008, "COMMENT = ", scomm, e

The Dialog Box functions in the MP post language using the MPPRINT formula does NOT allow for the user the enter text. (See 'mprint' in Formulas - Vol#3 Chapter#3 in the Post Docs) It allows the post to display a text message and wait for the user to select a button on the dialog box. What buttons (OK, CANCEL, etc) that are on this box is programmable. To get text or numeric input from the user when the post is running you would use the 'FQ' function. (See "How prompt questions work" in Vol#1 Chapter#18 in the Post Docs) You define the question to be asked using the 'FQ' and then ask the question using the 'Q' command. The response is returned as a Numeric or String dependant on the type of variable used in the 'FQ' line. code: numinfo : 0 # Declare a Numeric variable stextinfo "" # Declare a String variable FQ 1 numinfo Enter the Job Number # Define the question (#1) FQ 2 stextinfo Enter the Customer Name # Define the question (#2) pheader # NC file header information Q1 # Ask the question (Question #1) = Numeric result in numinfo Q2 # Ask the question (Question #2) = String result in stextinfo "%" "Job Number - ", numinfo, e "Customer Name - ", stextinfo, e "G90", e ... etc ...

You could try this... Post a (2-axis) program using the std. MPWFANUC.PST Now edit the NC file and make the changes shown -> All 'M60' to 'M06', 'M50' to 'M07, etc... code: Fanuc Makino (MGW-E control?) M60 M06 = Thread Wire M50 M07 = Cut Wire "Snnn" "Ennn" = Power setting M81 M17 = Power ON (maybe does Wire & Power also?) M82 ??? = Wire ON M83 ??? = Flushing ON This might give you a starting point to work from.

Maybe you are referring to the CSURF C-Hook from /www.camaix.com

quote: The text file will also be updated if you select NC Utils -> Post process -> Change, and then select the existing post processor. * Note for anyone reading this thread. * This solution will NOT work for what Robby needed. The UpDatePST utility will update the .TXT file to work with Mastercam v9, but would NOT alter the text that appears on the canned cycle parameters page!

quote: There exists a "first peck" and "subsequent peck" dialog box. Is it possible that the "subsequent peck" box is fighting you? Quite right ! If you have the post setup for long-hand output for Peck drilling, the values shown for -> Subsequent peck and Peck clearance ARE going to be used (does not matter that they are 'greyed out'. The TXT file for the post you are using is doing the 'gray out' on those input boxes. To enable those fields you need to alter the TXT file. *** Is this in the v8 MPMASTER.TXT ->> [peck drill] 1. "G83 - Peck Drill" 2. "Feed rate" 3. "Dwell" 4. "Clearance..." 5. "Retract..." 6. "Depth..." 7. "1st peck" 8. "" 9. "" 10. "" 11. "" *** CHANGE to this ->> [peck drill] 1. "Peck Drill" 2. "Feed rate" 3. "Dwell" 4. "Clearance..." 5. "Retract..." 6. "Depth..." 7. "1st peck" 8. "Subsequent peck" 9. "Peck clearance" 10. "" 11. "" After altering the TXT fkle for a post you MUST either; Re-start Mastercam or Change to a different post processor and then change back to your post.

Krispy Kreme Doughnuts just opened their 2nd store in CT last week. (These are the first stores north of NY in New England) When the 1st store opened last month, they had *many* people camped out in front of the store and lined up in the drive thru the night before the opening. Local TV news coverage and all. They were so busy for the first 3 days they had to pay for the police to handle traffic. Cars were constatnly back up out onto a major multi-lane road. We are in Dunkin' Donuts world around here (The 1st Dunkin' Donuts was in MA.) Like Tim Horton's for you people "north of the states".

The motto - "It it isn't broke, don't fix it" applies when talking about the Posting DLLs. If you do load a newer Posting DLL on your system, backup the current files FIRST. FYI... Mill/Router uses -> MP.DLL & MP.TXT Lathe usese -> MPL.DLL & MPL.TXT Wire uses -> MPWIRE.DLL & MPWIRE.TXT Quoting Dave - "Generally the updates cover obscure bugs along with additional functionality." Much of any additional functionality in the DLL versions mentioned is for the future v9.1 release, and for new stuff in the upcomming Router product release. *IMPORTANT* When v9.1 is released the Posting DLLs for v9.1 will NOT be compatible with v9.0 ! (This is due to compilation differences between the Mastercam versions) quote: "Would be nice if some changelog info would be included in the files though. Like in the appmch updates." The situation between the Posting DLLs and the APPMCH updates is a bit different. If there is anything REALLY important in the update, that would be noted (in the Mastercam download area) www,mastercam.com/Support/downloads/ -> MP_V904.ZIP (158KB) - MP.dll (V9.04) (05/08/02) -A very IMPORTANT fix in the v9.04 DLL files corrects arc outputs in the XZ & YZ planes. When posting toolpaths where arcs in the XZ & YZ planes were created by the filter, some of these arcs (in rare cases) would output as a straight line move. Post Processing Services CNC Software Inc.

"Setup Sheet" WHICH setup sheet are you refering to? The Graphic setup sheet The .SET type setup sheets or The HTML setup sheet stuff from InHouse ???

Are you refering to Cycle Times produced by a .SET type setup sheet generator ? If so... What version of MC are you running ? What .SET file are you using?

Try the MPA2100E.PST that was on the v9 CD It was based of the MPFAN which allows for Vertical/Horizontal configurations. You will need to alter (at least) these post switch settings ->> code: vmc : 1 # 0 = Horizontal Machine, 1 = Vertical Mill rot_on_x : 1 # Default Rotary Axis Orientation, See ques. 164. # 0 = Off, 1 = About X, 2 = About Y, 3 = About Z rot_ccw_pos : 1 # Axis signed dir, 0 = CW positive, 1 = CCW positive index : 0 # Use index positioning, 0 = Full Rotary, 1 = Index only ctable : 5 # Degrees for each index step with indexing spindle It does not have any support for the pallet system that you have, but your Dealer should be able to help you out with that.

Start MC with no MC9 loaded. From Main menu select NC Utils, Def. tools, Current The Tool Manager screen will appear (it will be blank). Right mouse click on the white area of the Tool Manager screen. Select "Create a library from text..." from the pop up menu. Hope that helps !

ProtoTrak MX2 & MX3 ? The are MANY people programming them with Mastercam. Looking for their 'language' type output -or- ISO (G-code) ? Contact your dealer...

quote: The other day I downloaded the Metacut utilities to try out as well as Predator's editor... Now I get "(Manual Entry)" at the end of my programs that look like: I don't know how downloading and trying out the MetaCut or Predator prodcuts would !change! your post output??? Have you (or someone) made changes to your MPFAN.PST ? Does these (MANUAL ENTRY) blocks appear in EVERY program you post process?

quote: How much does the Post processor guide CD cost and where does one get one?Contact your Dealer for this....

Chad, Modality - that's why. Look at the X,Y axis positions at the end of the 1st contour. They are at the SAME coordinates that the 2nd contour starts at. So, the post does not need to state the X,Y - because it is already there. Changing work offsets here is what changes the situation. You would want to re-state those X,Y coordinates. This would require a fairly simple post change to force output of the X,Y coordinates whenever the programmmed work offset changes.

I do not recall all the details, but I did do communications to a couple AB Series 9 controllers using std. Mastercam RS-232. These were Series 9 controllers approx. 3 years old (now) on lathes.

RATH, This is not real hard to do, but without having the actual PST file.... Also, you probably need 2 variables. You need one for you PLUNGE feedrate in addition to the Q30 variable for the CUTTING feedrate.

The ol' 7M sure was a different beast. I've run ino 2 of them, and one was a used one (aren't they all ?) that was the FIRST CNC machine this shop had purchased. Complete rookies to the world of CNCs! Boy, was that fun! BTW, I was told years ago by someone that worked for Fanuc that less than 350 7M controllers were ever produced.

Using the MPWPRIMA.PST from the Wire v9 CD I was able to post this out... 1>Start Position was set to -> X0,Y0 2>Thread was set to -> X0, Y-1.70452 3> "Auto Start position" was un-checked on the Lead in/out page. % G90 G92X0.Y0.U0.V0.Z0.H1. G00X0.Y0. Y-1.70452 M60 G69X1.U101W0 G62 X1 G41 G01Y-1.95452 X1.16365 Is this what you wanted ?

As I understand it, you are just trying to preserve the value from a Misc Integer at the start of the program so you can check it (use it) later one. You mentioned storing it to a Buffer ("Buffer" means an external FILE to a post). If you just trying to save this ONE misc integer value, that would probably be overkill. I would just declare a variable to hold that value. Then in the Start of File postblock, capture the Misc. Integer you want to save. (The postblock would be either LSOF -or- PSOF) code: my_value : 0 # Declare a variable lsof #Start of file for non-zero tool number, lathe my_value = mi1 # Save value in "mi1" at start of 1st operation. --------------- Since this is the only place that "my_value" is loaded with a value, you know that when you look at it later on in the post, it will hold the 1st operation (program startup) value.