Depends on the version of the post you have. Typically this is done through the control definition. In mastercam, go into the settings menu, select control definition, then on the left side of the window select the feed menu. There is a check box here for "Convert rapid to maximum feedrate". Check the box and, if the post supports it, you will have all your G0's converted to G1's with high feed rates.

The WCS is used to locate your part zero on the machine. The toolplane/construction plane are used to position the tool relative to your part zero. So if you use a WCS of Front and a toolplane of front, the post recognizes that the toolplane and wcs are the same, which would result in 0 rotation. If, however, you were to use the top wcs and the front toolplane, the post would recognize that the tool was machining along the -ve Y-axis and would calculate/output the necessary rotations to position the part/tool correctly. To summerize, the WCS position is used to locate the part zero. The orientation of wcs axis determine the part orientation relative to the "real world". The orientation of the toolplane and construction plane axis determine the tool position relative to the wcs. So I would suggest to start with, orienting your part as it will sit on your machine and using top wcs for all your operations, only change the toolplane and construction plane in operations to get the rotary output. I should also note that for 5-axis toolpaths, the toolplane does not drive the rotary axis output, the operation itself has a number of different methods to control the tool axis. Are you running a VR (tilting head) or a VF (rotaries on table)?

With out seeing the post, here is the basic code that needs to be applied: #declare variables nt : 0 last_mi4 : 0 last_mr2 : 0 last_mr3 : 0 last_mr4 : 0 #format variables - 2 is the default format for coordinates, 4 for integers fmt X 2 mr2$ fmt Z 2 mr3$ fmt Z 2 mr4$ fmt "NT" 4 nt #Code - put this after the retract (likely pretract, pretract0 or ptoolend), I don't know where to put this without seeing your post. if last_mi4, nt = nt + 1000 if last_mi4 = 1, [ pbld, n$, "M91", e$ pbld, n$, *sm00, e$ pbld, n$, "( *******CHECK INSERTS **********)" pbld, n$, "M90", e$ pbld, n$, *nt, e$ ] if last_mi4 = 2, [ pbld, n$, "( ********TOUCH OFF CENTERLINE OF PIECE*********)", e$ pbld, n$, *nt, e$ pbld, n$, *sg00, *x_home, *z_home, "M4", "S200", e$ pbld, n$, *sg00, "T0101", e$ pbld, n$, *sg00, *last_mr2, "Z2.", e$ pbld, n$, *sg00, *last_mr3, e$ pbld, n$, *sm05, e$ pbld, n$, "M91", e$ pbld, n$, *sm00, e$ pbld, n$, "(CHECK THE LOCATION OF THE TOOL EDGE WITH)", e$ pbld, n$, "(THE CENTERLINE PIECE.)", e$ pbld, n$, "(RESET 'Z' IF NECESSARY AS PER SET-UP INFO)", e$ pbld, n$, "M90", e$ pbld, n$, "T0121", e$ pbld, n$, *sg00, *last_mr2, *last_mr4, e$ pbld, n$, "M91", e$ pbld, n$, *sm00, e$ pbld, n$, "(ADJUST OFFSET #21 TO MAINTAIN SHROUD THICKNESS.)" pbld, n$, "(ADJUST ONLY IF SHROUD WILL BE THIN.)", e$ ] #update values in plast post block plast last_mi4 = mi4$ last_mr2 = mr2$ last_mr3 = mr3$ last_mr4 = mr4$ If you bought the post, why not go back to your reseller for edits??

Ah right...they renamed it from mpgen5ax. Excuse my ignorance, I don't actually use it... Certainly we have engine posts, but not an all encompassing post similar to this one where you can post out for any configuration of machine. Maybe some day though...

Unfortunately I don't think it is available for download...

When in doubt, give your reseller a shout!

So the issue here is that your wcs is set to the same plane as your toolplane/construction plane. Set your wcs to top in both operations and then post out the code and you should be good to go. If you are using a different work offset (G54/55/etc) for each plane, you can just change the work offset value on the planes screen.

The calculations for the rotary axis in the post are based on the setup in mastercam. Are you programming as a horizontal or a vertical machine (ie is the top toolplane B0 or is the front toolplane B0)? For horizontal machines, the default setting is to program using the front toolplane as B0, the right plane as B90, back as B180 and the left as B270 (depending on the direction of rotation). Make sure you have oriented your part correctly for horizontal machining. The error you are getting is because the toolplane you are using in an operation has it's Y-axis not oriented in the correct direction. If you are programming as a horizontal machine, the toolplanes Y-axis must align with the world Z-axis (the Z-axis of the WCS plane). In this case you can get the correct toolplane by rotating the front toolplane about it's Y-axis. If you are programming as a vertical, then the Y-axis needs to always align with the world Y-axis (the Y-axis of the WCS plane). To get the correct toolplane orientation, you can create your planes by rotating the top toolplane about it's Y-axis. Bottom line, make sure the Y-axis is oriented in the same direction for all tool planes you are using.

What post are you using to run this machine? Also, please clarify as to exactly which lines of code need to be added to differentiate the new code from what the post is already producing. I'm assuming that when checking the shroud thickness the coordinates are going to vary from part to part. Are you going to edit the values after posting or are you wanting the values setup as misc reals? When setting the misc values, are you wanting the insert check/shroud check to appear after the operation the value is set (ie around the retract) or before the operation? Will this only apply when changing tools or also in between operations with the same tool?

Perfect!

Open the post and go to the ldrill$ post block. This is what the post block should look like to work correctly: ldrill$ #Canned drill cycle, lathe pdrlcommonb pcan1, pbld, n$, *sgdrlref, pgdrlout, pxout, pyout, pzout, prdrlout, dwell$, pffr, strcantext, e$ pcom_movea pcanceldcl

I think you'll want to check which drill cycle you have selected in your operation. On the drop down select the first or second cycle on the list and you should get a different output as long as someone hasn't been monkeying around in the post itself.

This can be done by opening your control definition in the settings manager, selecting the machine cycles menu and looking at the lathe drill cycles page. There should be a list of lathe drilling cycles. Enable which ever cycle you would like to output as a canned cycle rather than longhand. I believe by default the mplmaster post is setup to use g83 for the simple drill - no peck and the peck drill - full retract drill cycles. Once the cycle has been enabled you should get the canned cycle. You may need to modify the post if you are not getting the correct canned cycle output though. Let me know if you are still having issues after enabling the canned cycles.

Is this on the same post? I thought the 8055 only took a D value, no H. If you don't mind some redundancy in your code you can search for any tloffno$ or tlngno$ variable and put a * in front of it to force it out every time. Make sure the variables are in lines that aren't commented out in the ptlchg_com post block and you shouldn't have these issues. if you are using H for length and D for diameter offset, then the tloffno$ should be located in the pccdia post block. Stuff a * in front of the tloffno$ to force the D value to output every time cutter comp is applied.

Bryan's right, add the code in as shown where you want the output in the post. If you don't always want an output, you'd set the output to: if mi3$ = 1, pbld, n$, "M919", e$ if mi3$ = 2, pbld, n$, "M919 S2", e$ If you give us more information on where you would like the code to output and what post you are using, we could steer you closer to a solution. I'm not sure if you've done this yet or not, but you also need to add the string to appear on the misc values screen. You can add the string through the control def by opening the control def and going to the Text menu, and select the misc int/real page. Alternatively, if you go to the bottom of the post you'll see something like this: [misc integers] 1. "" 2. "Absolute or Incremental [0=ABS, 1=INC]" 3. "" Put the text you want to see in your misc values window in the third string, so: [misc integers] 1. "" 2. "Absolute or Incremental [0=ABS, 1=INC]" 3. "Tool Life Counter [1=M919,2=M919 S2]" Make sure when adding this that the header for the text is either default (if there's only one) or the name of your control def: So for Mill: [CTRL_MILL|DEFAULT] or [CTRL_MILL|XYZ] (where XYZ is your control def name. HTH!

Since the configuration of the machines is different, the math in the post is different to calculate the correct angles, so you will need a different post to run the machine, specifically for the 5-axis motion. You are correct that 3+2 should be usable across the two machines based on the cycle 19.

Look in the ptlchg_com post block. Should be a section of code that looks like this: if stagetool >= zero, [ if omitseq$ = 1 & tseqno > 0, [ if tseqno = 2, n$ = t$ pbld, *n$, *t$, "M06", ptoolcomm, e$ ] else, pbld, n$, *t$, "M06", ptoolcomm, e$ ] change to read this: if stagetool >= zero, [ if omitseq$ = 1 & tseqno > 0, [ if tseqno = 2, n$ = t$ pbld, *n$, *t$, *tlngno$, e$ ] else, pbld, n$, *t$, *tlngno$, e$ pbld, n$, "M06", ptoolcomm, e$ ] then we need to remove the tool length call later in the post. Here's the original line: pbld, n$, "G43", *tlngno$, pfzout, scoolant, next_tool$, e$ Should be this: pbld, n$, pfzout, scoolant, next_tool$, e$ Depending on the version of mpmaster you have, the tool length may cancel after retracting, so look for "G49" of sg49 in the retract and retract0 post blocks and remove them if unwanted. There is also a G43 Dxxx call in the ptlchg0$ post block. If you need to recall the tool length here, position the tlngno$ where you would like the output, otherwise delete the G43, *tlngno$ from this post block

Jeremy's right, we'd need to know the model/style of Integrex to get the part setup correctly. The programming is also going to be dependent on how the post has been setup. Some people will program the vertical styles horizontally, some program them vertically, it all depends on how the post was initially setup for the machine. Some posts will need to make use of specific misc values to control the nc output or have the toolpaths setup in specific ways based on the post setup. From a generic programming perspective we can get you something, however the output from the sample file may not be good for the machine. Can you tell us which post they are using or who the supplier is? The supplier would likely have something programmed to suite. Also what version of mastercam are you looking for a sample for?