Multus B300-w programming issue.

ISO86 · Jul 14, 2017

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?

deadlykitten · Jul 14, 2017

ISO86 said:
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 !

Tskinner · Jul 18, 2017

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

Search

Largest Manufacturing Technology Community on the Web

Search

Multus B300-w programming issue.

ISO86

Aluminum

deadlykitten

Banned

Tskinner

Plastic

Similar threads