Metal Eater, Instead of "hoping QC is aware of this one", maybe an e-mail to QC ([email protected]) explaining what is wrong would help ensure they know about. Please don't assume they already know about bugs or have seen it on this forum, pester them and send them in, even if they do know about it. I forwarded this to QC for you.

DO NOT just add a comma!!! The comma added will tell MP the action associatted with the else is on the next line and that may not be what was intended. I believe this was bug in the release post and you should be able to just delete the ELSE line, but I suggest downloading the latest version as Marc suggested.

A value of -1 in the work offset field should be written to the NCI file (1016 line parameter # 9) as a zero. -1 should never be written to the NCI file. If this file wasn't created in V9sp1, try doing a regen to see if this problem goes away. As far as -1, this does not mean OFF to Mastercam. A value of -1 tells Mastercam to automatically set the value as need. So if there is a change in tool plane or tool origin, then a new WCS value will be generated. If you don't want Mastercam to do this, then always set the work offset to 0 (G54). I hope this helps!

JMD, What Scott suggested will only work if your post uses the MISC Values for work offsets. If your post uses the work offsets inside Mastercam, then you need to edit the work offset field under the T/C Planes dialog box. Edit your post and search for the variable WORKOFS, if you find it, then the post is probably using the Mastercam Work Offset Field and Scott's solution will not work. If your post is using the Misc Values for the work offset value, then do exaclt what Scott and Steve have suggested.

Carl, It's doable, but takes a little work. Seeing you like to pull your hair out (I got this from you working on this for 10 years!!! ) I will gladly give you some ideas on how to do this. First, MP will make a call to a postblock called PPOST. This call is made at the end of processing after all files have been closed and before exiting. Using this postblock, you can open the NC file as a buffer and read the lines of code one at a time, doing a renumber and then writing them back out to a temporary file. Once complete, delete the existing NC file and rename the temp file to NC. Now you can always not write the original file with line numbers and this makes it easy as you just add a line number to every line, however now you have line numbers on blank lines, comments, and any other line where you do not want them. Hint - process the file with line numbers being used and format the line numbers with a suffix character that you will not find in the file otherwise. As you read each line search the line for this character. If found this will tell you the end of the sequence number in the string. Strip it out and replace it with the new line number. Use the strstr and brksps functions. It works real well, but takes some work. If you don't feel like pulling the rest of your hair out, let me know and I will e-mail you an example.

SBA, If you are making the front view your WCS, then you have tols Mastercam this view is now TOP, period!!! That means that the front is now top, the bottom is now front, the back is now bottom, etc..... You can leave the TOP as the Active WCS and continue using front as front, side as side, etc and everything should be fine. I think your problem is related to making the front plane the active WCS. I haven't looked at your file yet, but if you tell me exactly what the problem is upon posting I will take a quick look at it.

Bruce, Mastercam doesn't allow those fields to become inactive. Why? Well probably because those values are a must for a drill cycle. Should they let you grey them out??? I can log it as a bug for you and see what happens. If you delete the text in item number 1, which is the cycle description that shows up in the drop down list, then that position in the list will be blank. You can still select it and use it, but it will not show up in the list. This may be just enough to keep someone from selecting the cycle. Another solution would be to modify your post to call just standard drilling postblocks when that cycle is selected. That way if the the cycle does get selected, at least the NC code would be usable for a simple drill. Hope this helps!

Brent, Check your NCI path settings under SCREE/CONFIGURE/NC SETTINGS/NCI PATH. Most likely what is happening is that these settings are causing the 2 seperate NCI files. One NCI file from the original MC8 operations and one for the new operations added using V9. I hope this clears things up for you.

Greg, The reason this happens is that the pretract postblocks are called after the tool change has been read for the next operation which causes you to lose the information from the previous operation. You can fix this easily by forcing an update of MI8 when high speed is set and then using the prv_mi8 in your logic in pretract. IE. if mi8>=one, n, "G05P10000", !mi8, e pretract if prv_mi8 >= one, "G05P0", e This should do the trick for you. Godd luck!

Dennis, It's hard to tell you were to look without seeing the output, so you know have to become the eyes in this game. First, edit the post and search for fastmode. If you find it make sure it is set to 0 (zero) or no. Next search for bug2 and set it to -40 (ie. bug2 : -40). By doing this the NC file will contain a list of postblocks that were used to creat the NC output line. Then you can track into these postblocks and look for the problem area. Then we can figure out how to remove it. You can post those lines from the NC file showing the problem and the debug output if you need additional help, otherwise contact your local Mastercam Reseller for their assistance.

Keith, The variables peckclr and retr are the ones you are looking for.

Rory, Make sure that you save the CFG file first before trying to assign one. Make the changes to the CFG file and then click on the save as button. Once the CFG file is saved, and the correct post is loaded, use the assign button in Screen/Config to assign the saved CFG file to the post.

Brian, By elaving the decimal out of the Format Statement (FS) you will get no decimals. Example: fs 1 1.4 #4 place decimal change to fs 1 1 4 #4 place, no decimal The number right after the fs is the statement number, you can have 30 of them. The rest of the numbers represent how you want the output formatted. In the above example 1.4, the 1 would represent the whole number, the decimal charater for output and the 4 for the fractional portion of the number. You can also use l and t for leading and trailing zeros. Examples: fs 2 3 0l #3 place integer with leading zeros fs 3 2 4lt #4 place decimal with leading and trailing zeros. I hope this helps!

If you are doing tranlations in the same view, not a change in toolplane, you need to check on the tool plane origin only check box right under the tranlate selection box. Also make sure your transform method is by toolplane and not coordinate. Mastercam will only create new offsets for a change in toolplane or change in tool origin. Try these settings: TYPE - Translate / tool plane origin only METHOD - Toolplane Copy source subprogram / inc Work offset numbering - assign new, start 0, increment 1. It should work fine. Jim Evans

Oppiz, May I suggest you contact your Local Mastercam reseller and purchase the Post Processor documentaiton on CDROM. This will cover plenty of information and it is the latest available. In simple terms: fs2 1 1.4lt 1 3 fs2 - function name (fs/fs2 are similar. fs2 allows you to apply an english and metric format at the same time) 1 - Format statement numer - 30 max 1.4 - English format l - Leading zeros t - Trailing zeros 1 3 - Metric format - Do decimal output . - Ouput decimal ^ - Only output decimal on awhole number - using a space between interger and fraction part means omit decimal , - replaces decimal with comma. Hope this helps!

OPPIZ, This is happening because the TLRAD variable is not formatted for output. Anytime you use a variable that hasn't been formatted (with an FMT statement), then MP will apply Formtat Statement 1 (fs 1) for numerical format and output with the Name of the variable as a prefix. IF you add a FMT statement similar to below it will fix the problem. fmt 10 tlrad # XY part plane FMT is the function name, 10 is the format statement (FS) number that will be used to format the numerical output, and then the variable name. IF you need a prefix address with it, then it would look something like this: fmt T 10 xyheight # XY part plane Where T would prefix the numerical data on output. I stil suggest contacting your local Mastercam reseller for help. He may also be able to give you some Post Training.

OPPIZ, I'm going to assume you are using the MPWMTS-F post from the release. IF you are using this post, then this post uses a different methoid for toolchanges (passes) than the MPWFANUC does. This post uses the PSTARTPSOFA (Start of file pass) and PSTARTPOSA (toolchange passes) to control which output postblocks to call. These postblocks make the call to the correct output postblock depending on the situation sp things like CUT/Thread codes, G92 output and condition codes can be output. This is probably whree you really want to add your code. You can still put it in the PSOF and PTLCHG postblock, but these postblocks will call the ones mentioned earlier for output. With that said, if you want the offset registry value (H1, H2, etc..) then you should be using the OFFSET variable. IF you want the Wire diameter you need to use TLDIA or TLRAD for the wire radius. When I performa test of the output variables in the PSOF and PTLCHG they seem to be coming out okay. What version of Mastercam are you using and what is the exact name of the post you are using?

Commenting out the psub_end will get rid of the M99's that come out with the canned cycle, but if you go to use Mastercam's subprograms, you have just commented out necessary code needed for Subprograms. This looks to be a bug in the MPL.DLL and is currenttly being worked on.

Mike, Setting Rot_on_x to zero would disable the rotary axis output completely and I don't think this is what he wants. Correct me if I'm wrong Heavy Metal!!! Jim

Mold100, You can accomplish this using Mastercam and the Transform operation, however your post processor must be set up to handle Mastercam's subprogram output. MPFAN will handle this as will MPMASTER. The transform operation has many options that you should become familar with. I suggest doing an example of what you are trying to do and experiment with the settings such as copy source, work offset and output order. Make sure your tranform method is toolpane. Give it a try and if you have any questions, just holler! Jim

OPPIZ, The changes required depend on your post. The Wire offsets variable is OFFSET, but the wire diameter variables are tldia or tlrad. I can't tell you exactly how to do it wihtout seeing your post. I suggest contacting your local Mastercam Reseller with this request and make sure to provide them with your post and an example of the changes you want to make. Jim

Heavy Metal, If all your post settings are correct, then your toolplane is incorrect. Make sure that the toolplane axes are in the correct orientation so that if you rotated the part into the front view the X,Y,Z of the new toolpane would match the front toolplanes XYZ orientation. For example. If the post settings are set correctly for a horizontal mode, then the only valid rotation of a toolplane would be about the Z axis of the World Coordinate system. If the toolpane cause another axes of rotation, that is invalid!! It's ALWAYS either the post settings or the operation. If you need help provide the MC8 and the post and we can check it out for you. Jim

Bruce, If this is a problem that just started after making modifications to the post, you should back track your changes and check all your syntax. I'm willing to bet it's something simple associated with the cahnges you made to the post. Jim

rot_on_x is the machine relative axis of rotation and is used in the post to detrmine what calculations to perfom based on the machine setup. This allows us to have one post for multple machine setups. In MPFAN you will notice it is sued to determine something as simple as if you have a rotary axis on the machine to what axis we are rotating about so the correct calculations can be performed for axis substituion, 4ax rotary and polar conversion. I hope this helps!

Larry, I would suggest working around it in the post so that you can still take advantage of V9. When the fix is made a patch or app will need to become available which can take some time. You can always do what Dave suggested. Don't use force toolchange in MC, but instead incorporate the tool change code into the post. That way when you use MI10 you can call this toolchange code also. Depending on your post you can use the ptoolend postblock or the ptlchg1002 postblock. The ptoolend postblock is called prior to the next tool change (nul or actual) being called. This means you still have all values related to the current toolpath. The ptlchg1002 postblock is used a little differentl based on your tlchng_aft flag. If you need help with these modifications contact your reseller first.