Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

MP Master G10's?


Recommended Posts

Any simple way to get MPMaster to output G10 L12 P1 R0.0?

I've had enough of the operators running a muck! I'm throwing down the hammer on Wear Comp. But in order for it to work Im having to do manual entries with My G10's. I want to do them at the beginning of the program to zero the tool diameters and would like to do them at the end to reset the value to the the tool Diameter encase the next job uses the same tool but is programmed in Control. Its the only way I can see to keep these guys from messing up a good thing. Would be even more awsome if it were attached to a misc integer so I could switch it on and off. This is obviously deeper down the rabbits hole then I've been. But it could make my job sooooooo much ezier... Thanks as always

Link to comment
Share on other sites

Here's what I use before firing up the laser setter programs;

%
O9026(M501 -- TOOL OFFSET REMOVAL PROGRAM)
(PARAMETER 6086)

(A = FIRST TOOL TO REMOVE, DEFAULTS TO 6)
(B = LAST TOOL TO REMOVE, DEFAULTS TO 200)

IF[#1EQ#0]THEN#1=6
IF[#2EQ#0]THEN#2=200

WHILE[#1LE#2]DO1
#3=10000+#1
#4=11000+#1
#5=12000+#1
#6=13000+#1
IF[#1EQ4]GOTO1
#[#3]=88.8888
#[#4]=0
#[#5]=0
#[#6]=0
N1
#1=#1+1
END1
M99
%

This program will clear out the comped offsets and adds 88" to the geometry length offsets. If a tool is missed the 88.8888 will over travel the empty pocket.

  • Like 1
Link to comment
Share on other sites
  • 1 month later...
16 minutes ago, MichaelH said:

Hi there, I am using a g10 post from the ftp page for outputting work offsets (G54.1 P-) I know this is short and sweet with no detail but my output is missing values in X Y Z

G10 L20 P7 X0. Y0. Z0. B0
G10 L20 P8 X0. Y0. Z0. B0

any simple reason why?

 

Because the code in the Post is not configured to use the Tool Plane Origin values. This is fairly simple to add if you know the MP Post Language.

The variables that hold the Tool Plane origin are: tox$, toy$, and toz$. But, those XYZ values are relative to the Tool Plane orientation. The variables tox4$, toy4$, and toz4$ hold the XYZ values, relative to the WCS matrix.

If what I'm describing sounds like Greek to you, then you should pay a Post Developer to fix this for you. 

  • Like 1
Link to comment
Share on other sites

Thanks, I did think that would do it, and no it didn't sound greek.

This is how it posts

G90 G10 L20 P1 ( G54.1 P1 ) X0. Y0. Z0. B90.
G90 G10 L20 P2 ( G54.1 P2 ) X0. Y0. Z0. B90.

Changed tox$,toy$,toz$ to to4x$,to4y$,to4z$ at 6 places as below.

This was an old 2011 post on ftp and although it has been through updatepost I am not sure if its relevant.

 

while rc9 <= size9, # Determine if current workoffset/origin is unique
        [
        b9_tox = rbuf(9,rc9)
        b9_cabs = atan2 (m1$, m7$)


        if b9_tox <> tox4$, new_x = new_x + 1 -------HERE
        if b9_toy <> toy4$, new_y = new_y + 1 -------HERE
        if b9_toz <> toz4$, new_z = new_z + 1 -------HERE
        if b9_workofs <> workofs$, new_workofs = new_workofs + 1
        ]

        if new_x = size9 | new_y = size9 | new_z = size9 | new_workofs = size9, # If current workoffset/origin is unique, write to buffer 9
        [
        b9_tox = tox4$ ----HERE
        b9_toy = toy4$ ----HERE
        b9_toz = toz4$ ----HERE


        b9_workofs = workofs$
        b9_cabs = atan2 (m1$, m7$)

        b9_tox = wbuf(9,wc9)
        ]

Link to comment
Share on other sites

All sorted, I decided to download the mpmaster from here and add the G10 code from another post file. Datums are output from machine origins .

0000 (test)
G00 G17 G21 G40 G80 G90
G90 G10 L20 P1 ( G54.1 P1 ) X-1000. Y-552.38 Z-740.044 B90.
G90 G10 L20 P2 ( G54.1 P2 ) X-1279.9 Y-666. Z-995.044 B0.
G91 G28 Z0.
T2 M06 (SOLID CARBIDE DRILL 5XDC - 8.5)
M22 (UNLOCK)
G00 G17 G90 G54.1 P1 B0. X0. Y2.38 S4868 M03
M21 (LOCK)
 

  • Like 3
Link to comment
Share on other sites
  • 5 months later...

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...