Or use the MD_CD_PST Rename AddOn available here -> Mastercam-Support-Downloads

Scroll down until to see the Add-Ons section and be sure the download the package with the proper (32/64) "bit-ness".

*Of course, first make sure you have a backups of your original Machine/Control/Post files!

Hi Roger,

That's great that the c-hook is again available. I think it was unavailable for a version or two but I'm glad its back. It will make my job easier.

M30

How involved would it be to post out Number of points drilled like min and max values??

 

Example:

 

M01

N72 T72 M06 ( 1/4 SPOTDRILL)

(MAX - Z2.)

(MIN - Z-.56)

(26 PLACES) *****ADD TO POST*****

M11 (UNLOCK)

G00 G17 G90 G54.1 P59 X-.81 Y9.5 B0. S12000 M03

M10 (LOCK)

G43 H72 Z2. M08 T75

G94

G98 G81 Z-.56 R.1 F20.

X0. Y10.31

X.81 Y9.5

ETC....

I don't think this would be trivial. You are saying you would like a comment stating the number of drill points prior to the drill operation. The NCI file is linear and so the only way to find out that piece of information is to suspend all code output until after all the points are drilled while counting the number of points. Then the number of points could be output, and then release all the "buffered" code. It would be a bit of a pain to set up, but I doubt it would be impossible. You should contact your reseller and see what they suggest.

M30

I am new and am looking forward to learning more about post processors. I have two HAAS mills. One has thru-tool collant and a 10000rpm spindle. The other has a 15000rpm spindle with no thur-tool collant. I am using the same post for the two machines. I would like to have a different post for each machine due to the differencs in spindle and collant options. Is there a way I can copy and rename the CONTROL-6, MastercamX6 MMD, and the PST files so I can have two different posts and tweek some of the settings to make them machine specific?

I do this all the time. The best method I have found:

1. create a copy of, and rename the "pst" (and "psb" if there is one) using windows explorer or similar.

2. rename the mmd-6 and control-6 using mastercam:

- after creating your copied renamed "pst" file go into mastercam settings menu -> machine definition manager.

- load up the machine definition you want to rename

- "save as" this machine definition as the new name

- from the machine definition manager dialog box, click the edit the control definition icon.

- once in the control definition, hit the "save as" button, and save as the new name.

- under the post processors button, add the newly named post into the list, and remove any old posts from the list

- at this point if you hit save on the control def manager you should see a green check mark beside the post processor path for the new post.

- last important step, you need to import all settings from the old control def:

*select any of the control def settings on the left side.

*right click over top of the settings on the right and select import -> all pages

*select the original named control def, and the original named post to pull settings from

*save the control def

Everything should then be renamed and you should be good to go. Long process I know! If in doubt contact your mastercam reseller.

M30

M30,

 

I'm glad you've taken an interest in editing Post Processors, but some of the information you posted is incorrect, so I'm going to take a minute and clear some of that up.

Much appreciated. There is always more to learn. Some of what I assume to know is empirical, and based on working with posts alone. I love hearing the straight facts from the source. It would be awesome if some of this information was stickied in a post processor section of the forum.

Good discussion all. I'm enjoying it.

Cheers,

M30

[email protected]

Thanks M30..............(I guess)......you know anything about the parameters for the limits shown in the pic attached to the first post in this topic?

haha. Sorry i would have commented if i had tried pulling those before. I haven't run into a situation where i've had to pull those variables, and currently don't have mastercam to test.

I wish I could help further.

Regards,

Your local post processor Guru

Some general notes on parameters for everyone with regards to MP posts:

- There are several ways parameters must be obtained.

* some parameters are available in the NCI file and can sometimes be read using sparameter$ or via existing variables.

* Some values with existing variables do not need a parameter read, but a parameter read could be used to fill a new variable with the same information. * There is a long list of existing variables in the V9 documentation and you can also find several in some of the newer documentation

- Contrary to popular belief there are many parameters that do not appear in the NCI file in any form, but they still exist. They are passed by some method directly from mastercam to MP and then to the post when called for.

* in order to call for parameters not available via the NCI file some commands like rd_params$, rd_cd$, rd_md$, rd_tlpathgrp$, etc must be present in the correct location in the post. This can be difficult to troubleshoot. Some of this information is in mpmaster already but there are no guarantees it is all there, especially for newer parameters that are not used in any of the mpmaster output currently.

* some parameters are only accessible via parameter tables.

parameter table calls:

#Read parameter lookup tables -

if prmcode$ >= 17000 & prmcode$ < 18000, result = fprm(1) #Run the parameter table for Machine Definition Parameters

#Leave lines below commented until you enter values in related lookup tables

if prmcode$ >= 18000 & prmcode$ < 19000, result = fprm(2) #Run the parameter table for Control Definition Parameters

#if prmcode$ >= 19000 & prmcode$ < 19900, result = fprm(3) #Run the parameter table for Toolpath Group Parameters

parameter table contents:

fprmtbl 1 42 #Table Number, Size

# Param Variable to load value into

17008 spostname #Post Processor Filename

17060 minfrdeg_old #this parameter no longer functions MU00008b

17054 minfeedpm #Limit for feed in inch/min

17055 maxfeedpm #Limit for feed in inch/min

17058 maxfrinv #Maximum feedrate - inverse time - inch - Minimum value from MD as this is inverse time

17059 minfrinv #Minimum feedrate - inverse time - inch - Minimum value from MD as this is inverse time

17922 maxfrdeg #Maximum feedrate deg/min

....

....

* there are other parameters still that are only available as a filled group of variables. essentially the parameter number is called and a bunch of variables are filled at once in sequence all from the main call parameter, like so:

declaration of all variables associated with the parameter:

fmt 2 slot # 20004 Parameter line

fmt 2 tool_type

fmt 2 matl_type

fmt 2 corner_rad_type

fmt 2 diameter

fmt 2 corner_rad

fmt 2 threads

fmt A 2 tip_angle

fmt 2 dia_off

fmt 2 len_off

fmt 2 tool_feed

fmt 2 plunge

fmt 2 retract

fmt 2 rpm

fmt 2 coolant1

fmt 2 n_flutes1

fmt A 2 tip_angle_ch

call of the parameter group to fill the variables in pwrttparam or pparameter:

if prmcode$ = 20004, slot = rpar(sparameter$,16) - note the total number of variables is the 2nd argument in the function.

- i have probably forgotten a thing or two but that's most of the critical stuff. In summary obtaining information from parameters in MP can vary in complexity depending on how they must be obtained. Also the system of information itself is somewhat more complex than it needs to be, which is mainly due to the MP language being built upon over a number of years and the needs for information expanding beyond the original scope of older MP post processors.

Regards,

Your local post processor Guru