Jim, I'm saying that the post needs to output the G7 in a very specific way to make sure your X,Y and Z coordinates are mapped correctly. The only difference between the two G7 commands you've listed is the direction of the X and Y axis, the Z axis should be pointing in the same direction in both cases. The post should be looking after rotating the coordinates to match the A, B and C output. Just because the plane you are cutting on in mastercam is a 46.5 degree rotation about the Y axis does not mean the code needs to be output as a rotation about Y. If indeed you do need to change the post, chances are it's in the encrypted section of the post. You will most likely need to contact your reseller to make changes. Chris

Jim, In some cases it is possible to perform a tool plane rotation such as your post is outputting, but it depends how the machine rotates your coordinate system. If both the A and C rotation happen about the original machine coordinate systems (ie rotate 46.5 degrees about x, then rotate this new tool plane 90 degrees about the ORIGINAL z), the resulting tool plane will be equivalent to the single B rotation. This is how the G7 command should work. Some machines/controls don't allow this though and require the rotations be done in a specific order. In these cases typically a post will output the rotation about the z axis first (ie G7 L1=1 A5=0 B5=0 C5=-90) and then about the x/y axis (G7 L1=1 A5=46.5 B5=0 C5=0). I doubt this is the case for your machine, it should handle everything on one line. Not sure that this will help out your posting problem, but may help you understand the logic behind why the post is spitting out what it is. Chris [ 02-21-2008, 10:54 AM: Message edited by: Chris McIntosh ]

Robert is right. The manual entry comes out from pcomment2. So, just put the comment$ whereever you want that to appear in your tool change block. Gcode 1005 - As Comment Gcode 1006 - As Code

Just use all the variables that are shown but add a $ to the end of them.

Sorry rcdie, It is not appropriate to share this information for various reasons. Brett

SIG, Steal the phsm post blocks and the calls to them from the new mpmaster and smash them into your version. Also anything to do with misc real 1 and 2. Good luck with it. Brett

Kevin, There is a customizable update file that you will need to get your hands on to update correctly from X to X2. I've put them up on the ftp Here Just place these files in your chooks directory and then run the updatepost chook again. Chris

Yeah, it's really 100% handled in the post. You've got to handle the rotary axis and tool comp in the XY plane to start. Then, you need to make arcs work too.

jgary, Yes, use the misc int 10 to force the M00 then you'll get all your startup stuff as well. There's an mpmaster_okuma post available that does this (then you can just add your custom stuff to the mi10$ logic). Just have your dealer request the post on your behalf. Brett

All, A short explanation of how work offsets work follows: If you do not set a work offset value in Mastercam (leave it as -1), Mastercam increments the variable called workofs$ for every new tool plane it encounters. So, you're effectively telling the post you want a new offset for every new plane. For some posts, that means G54,G55,G56, etc. The integrex works a little bit differently. For the Mazatrol side of the control you've only got 1 or 2. G53(.5), and on the Mark II you could get a P1/P2 option. So, when you want to chagne to a new work offset, you need to do a G50 shift. Every time the post sees a new work offset, it sees asks for that shift variable then outputs accordingly. Hence the message YOU MUST SET YOUR WORK OFFSET IN MASTERCAM FOR EVERY OPERATION I encourage people to set all ops on the main to work offset 0, and all ops on the sub to work offset 1. this can be done through the view manager as Ron had shown earlier.

The ` in posts is actually to tell it to output if something else comes out on the that line. While we're at it: * is update and force output ! is update and no output ~ is output but no update @ is apply formatting (this is nice to use so you don't always have to use the fmtrnd command)

For the peck and dwell se usually do something like [if peck1$, *peck1$]....same goes for the dwell. Check out the cycles that are in there, you'll see how to do it.

You guys want peck Q added to mplmaster tapping? We've already put it into mpmaster.

code: #sav_rot_on_x = rot_on_x #Uncomment this line to output rotary axis value even when it's not used You must set the misc reals for high speed/look ahead/acc/dec in all ops.

All, Further info on that G73 item as discussed above. Uncommenting the call to pcc_capture is step 1. However, this will blow away the z motion after the canned cycle due to the setting of the no_nc_out$ flag. To fix, go to pcc_capture and make the following change. code: pcc_capture #Capture ends of canned turning path, stop output w/rough #Stop output in rough only lathe canned cycles #between rough and finish paths #if cc_stop_fcc & rcc_flg$ = 6, no_nc_out$ = one # 05/28/04 if cc_stop_fcc & rcc_flg$ = 6 & lathecc <> 2, no_nc_out$ = one #wbt - do not want to stop output before/after pattern repeat I hope this helps. Brett

All, Here's the logic for it. Uncomment out the line shown and you'll get the A0/B0 output. the reason it's here is for 3-axis users. code: pwrtt$ # Write tool table, scans entire file, null tools are negative if rotaxis$ > 0 | rotary_type$ > 0 | mill5$ <> 0, [ sav_rot_on_x = rot_on_x output_z = no$ ] if vmc = 0 & tlplnno$ <> 2, sav_rot_on_x = rot_on_x if vmc = 1 & tlplnno$ > 1, sav_rot_on_x = rot_on_x #sav_rot_on_x = rot_on_x #Uncomment this line to output rotary axis value even when it's not used Brett

Search for a switch called one_rev. Disable it. One_rev sets all indexing output between 0-360. It's only applicable for indexing ops though. Reason behind your tool plane error: 3/4-axis posts do not do any mapping. Code is supplied to the post already mapped. This mapping is done before the post gets hold of the coordinates. For horizontal machines the table rotates about the machine Y, so Mastercam rotates your current toolplane about it's Y around to the base plane (that's the front where the tool comes from). For verticals, same thing. The current plane is rotated about it's own X (because the machine rotates about it's X). This becomes a problem on the back toolplane. It's X faces the opposite direction. So, you must rotate it 180 deg (to gets it's X to line up with machine X) then Mastercam's mapping will work for you. Sound confusing? It is. 5-axis posts don't work like this. you can just pick any plane you like and it just works. This is because all mapping is done in the post so we've got a little more control over it. Brett

Don't slice and dice it too much!

Huh....no clue on that one. Mplmaster didn't exist in 2004 so this is an mpfan thing.

All, I have found the problem with the G73 pattern repeat. To recap, his problem was to do with the UW vector for pattern repeat G73 not coming up with the right values. code: pl_ncoutput #Movement output pcc_capture #Capture LCC ends, stop output RLCC # 05/28/04 #This was previously commented out but I have removed that as it affects G73 pattern repeat. I'm not sure what else this affects at this point. WBT I hope this helps anyone that uses G73....and I hope it doesn't break anything else! I'll send it into CNC for them to take a look at. Brett

It appears the mplmaster based posts are suffering from the same variable issues as the mill post. As a result there are some changes need to correct this. First, comment out the bottom two lines and change the table size: code: fprmtbl 17000 5 #Table Number, Size - Machine Definition parameter table 17391 axis_label #Axis label - 1=X,2=Y,3=Z 17402 rot_dir #Rotary direction 17408 rot_index #Index or continuous 17409 rot_angle #Index step 17410 rot_type #Rotary type #17101 all_cool_off #First coolant off command shuts off ALL coolant options #17102 v9_coolant #Use V9 coolant option At the top of the post the v9_coolant and all_cool_off variables should be set if needed. v9_coolant if you would like to use version 9 coolant and the all_cool_off if the first coolant off command turns off all the coolant. A revised version of the post will be available for download shortly. Chris

Much thanks to Greg Williams and Nguyen Ho for their help on it! I just don't know how you can know so much about these machines and be good at Mastercam. We all worked very hard together on mpmaster_okuma and a post for the MU400/500VA trunnion machine as well. Brett

Scott, Yes, it's possible to do what you're looking for. We've done it for a customer of ours. Brett

1. Get the latest and greatest version of machine sim. It's available from your Mcam dealer. 2. Run the exe and specify your mcamx dir. 3. The Machine sim icon is located in the advanced multiaxis category. Drag and drop it to your desired toolbar or mouse right-click button. Alternatively, you can run it as a C-hook....alt+C them machsim.dll. 4. Your Mastercam origin is coincident with the machine's origin. eg. At the intersection of rotary and tilt for a trunnion. 5. When you run it, pick your machine. Then pick your workpiece, all elements for it to recreate the stock STL or recently used to save time and skip recreating it. 6. If you want to shift your datum, select user defined. So, if you Mastercam origin with respect to the part is not at that intersection of rotary and tilt, you can shift where machsim thinks it is. eg. if your part is 10" tall and your datum is at the top of the part, you'll want to place a Z+10 shift in becasue the machines 0 is at the table top height. 7. Select your stock. Use Mastercam's stock or have machsim create STL stock based on your current surfaces on the screen. 8. If you're setting up an In-House post, the folder including the post, .xml file, stl. files, etc. to this directory with all the other machines: C:McamX2-MR2moduleworksmachsim Brett

Hi Rakesh, Use top, back, front, or bottom plane (depending on how your part is setup), turn off the rotary axis button, you're done. Brett