Multus B300-w programming issue.
Close
Login to Your Account
Results 1 to 3 of 3
  1. #1
    Join Date
    Aug 2012
    Location
    VIC, Australia
    Posts
    56
    Post Thanks / Like
    Likes (Given)
    23
    Likes (Received)
    10

    Default Multus B300-w programming issue.

    I have recently been learning to run and program a b300-w multus. We do a family of parts with a slot that goes into a sharp corner. We do this by a combination of horizontal base b and vertical base b. To get into the corner we use the b axis ba=45. Its fine with using horizontal and vertical but when ba=45 the tool is not where the programmed values are. We set the tool off the setter in horizontal b position. We fudge the program values to get why we want but we know it's not correct. Eg if programmed position in ba=45 is (metric) z1 x23 y0 the actual tool position is more like z.7 x21.8 y0. Where are we going wrong? Should it not automatically compensate when in ba based on the x and z offsets for that tool and whatever angle ba is set to?

  2. #2
    Join Date
    Aug 2016
    Country
    ALAND ISLANDS
    Posts
    1,393
    Post Thanks / Like
    Likes (Given)
    43
    Likes (Received)
    96

    Default

    Quote Originally Posted by ISO86 View Post
    I have recently been learning to run and program a b300-w multus. We do a family of parts with a slot that goes into a sharp corner. We do this by a combination of horizontal base b and vertical base b. To get into the corner we use the b axis ba=45. Its fine with using horizontal and vertical but when ba=45 the tool is not where the programmed values are. We set the tool off the setter in horizontal b position. We fudge the program values to get why we want but we know it's not correct. Eg if programmed position in ba=45 is (metric) z1 x23 y0 the actual tool position is more like z.7 x21.8 y0. Where are we going wrong? Should it not automatically compensate when in ba based on the x and z offsets for that tool and whatever angle ba is set to?
    tool corections deliverd by touch senzor are available for future use, only if B is at same value

    dynamical comp relative to a variable B is not "default"

    please consider that this type of machining can be achiever without touch senzor

    thus, the key, is not the touch senzor

    ... try too write a program that compensates it thus try to cut a circle with the B axis, after measuring the tool at a random angle

    program inputs should be :
    ... required radius
    ... tool angle when touch senzor had been used

    that's the key if you have the patience to do it, you may debug all future issues of this kind !

  3. #3
    Join Date
    Apr 2015
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    46
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    10

    Talking

    ISO86, I assume this is a P200L control machine. On the P300S control, some things related to tool offsets are different.

    In order to work with a milling tool at the BA=45 plane, you need to use G52 in the tool change call statement. Also, it might be a good idea to use G174 and G127 to rotate the tool plane coordinate to the 45 degree angle. That way the Z-axis will be parallel to the tool. More about Slope Machining Function and Zero Point Shift are explained in your Macturn/Multus Operation Manual (LE32-114-R*). Below is some sample code of how it works:

    N0001 G140
    N0002 G00 X50 Z50
    N0003 G50 S2800
    NAT01
    N0100 G00 X50 Z50
    N0101 MT=0101
    N0102 TC=01
    N0103 M421
    N0104 M110
    N0105 G94 M146 M15 M08
    N0106 G00 X50 Z50
    N0107 TL=0101 BA=45 G52 SB=2674 M241
    N0108 X5.6264 Z0.1061
    N0109 G138 C0
    N0110 G174 SX=2 SZ=0
    N0111 G127 B45
    N0112 G00 X0.5 Y-1
    N0113 Z0.65
    N0114 G17
    N0115 G00 C0
    N0116 Z0.25
    N0117 M13
    N0118 G01 Z0 F85.56 M147
    N0119 Y1 F17.11
    N0120 G00 Z0.25
    N0121 Z0.65
    N0122 G126
    N0123 G175
    N0124 G136
    N0125 G95 M12 M146 M09
    N0126 M109
    N0127 G00 X50 Z50 TL=0100 BA=45
    N0128 M02


    Hope that helps


Tags for this Thread

Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •