Community
From what you wrote, I think the Mach3 controller doesn't have RTCP functionality.
"Without RTCP there is no fluent simultaneous movement of the machine it just rotates B axis for a long time before starting to use Z"
- This behavior is independent of the RTCP / without RTCP option, but depends on the value of "Linearise Multi-Axis Moves". If you set it to "None", it would disappear, but you would not be able to do this without the RTCP function, because a faulty tool path would be created.
-"while with RTCP gcode due to inadequate y distance it tool collides with B axis table."
This is correct behavior, because for machines with RTCP function the kinematic correction must be made by the control.
Take a look at the following pictures of cigra.cut: both have only linear axis movement, rotary axes are off, and high speed movement off
.
with RTCP with RTCP
with RTCP with RTCP
without RTCPwithout RTCPChange these with your Fanuc5osa postprocessor:
Option File Settings:
Program Generation - General - General -Use Model Location = No (If set to Yes then always fill the Nc-program Model Location in Powermill)
Program Generation - Multi Axis - Workplane Definition- Ignore Toolpath Workplane Shift = Yes
Program Generation - Machine Kinematics - 2nd Rotary(A) - Origin Y,Z exact measured values. Such as Y0;Z19 -> Y-0.03;Z18.982
Program Generation - General - General -Use Model Location = No (If set to Yes then always fill the Nc-program Model Location in Powermill)
Program Generation - Multi Axis - Workplane Definition- Ignore Toolpath Workplane Shift = Yes
Program Generation - Machine Kinematics - 2nd Rotary(A) - Origin Y,Z exact measured values. Such as Y0;Z19 -> Y-0.03;Z18.982
In Move Rapid/ Move Linear Commands:
X,Y,Z axis -Workplane for Output = Machine Workplane
X,Y,Z axis -Workplane for Output = Machine Workplane
Preparation on Powermill:
The Nc-programs Output Workplane always set to Machine Tool reference workplane.
The Nc-programs Output Workplane always set to Machine Tool reference workplane.
It will be necessary to adjust the tolerance and the point distribution. https://forums.autodesk.com/t5/powermill-forum/best-way-to-have-better-surface-finishing/m-p/8380088...
The result:
Sorry, I was ambiguous when I wrote about the C axis and in the quote about the A axis, in your configuration it corresponds to the B axis.
I found the following in the Mach3 config manual:
I modified the postprocessor you sent:
Replace rotary _axis1_2020 and rotary _axis2_2020 with Machine A, Machine B in Move Linear/Move Rapid Command.
I tested the new settings in postprocessor with default Mach3 settings
B axis rotates in both directions so I guess this is better. With Ang short options on it is a bit better when it comes to line
466 N563 X3.2799 Z23.2525 B0.0
467 N564 B360.0
although I'm not sure why it is doing this. Also I noticed that Y coordinates are working strange it just alternate between coordinates 117 and 227 while starting to change a bit latter in code and never in simultaneous mode but always independently. What do you think of this? Here is the first few minutes of video.
Also at begging and in the end it has at line 25 N122 G53 Z0.0 and N9955 G00 G53 Z0.0 command which if stock was in the place would plunged the tool and the spindle into it. How to change this?
I create a simple macro that will help you compare machine simulation data to "wihout-RTCP" postprocessors output.
Need a short (macro working slowly) 5 axis toolpath activated, Machine Tool model activated, Model Location selected. Output is created in the project \ ncrpogram directory
FUNCTION MAIN () {
STRING ActiveProject=project_pathname(0)
IF $ActiveProject == "" {
MESSAGE INFO 'Please save the project'
RETURN
}
IF NOT entity_exists(entity('MachineTool', '')) {
MESSAGE INFO 'Please activate Machine Tool'
RETURN
}
IF NOT entity_exists(entity('Toolpath', '')) {
MESSAGE INFO 'Please activate Toolpath'
RETURN
}
ENTITY TP=entity('Toolpath', '')
IF (NOT $TP.Computed) OR (SEGMENTS($TP)==0) {
MESSAGE INFO 'Toolpath not computed/empty toolpath'
RETURN
}
STRING LIST Axes=filter(Machine()._keys,"(this < 'max') OR (this > 'minZ')")
$Axes=sort($Axes)
STRING Config=""
FOREACH C IN $Axes {
$Config=$Config+$C
}
STRING LIST Kinematics={'ABXYZ','ACXYZ','BCXYZ'}
IF not member($Kinematics,$Config) {
MESSAGE INFO 'Unknown configuration'
RETURN
}
$Axes[3]=$Axes[0]
$Axes[4]=$Axes[1]
$Axes[0]='X'
$Axes[1]='Y'
$Axes[2]='Z'
STRING SimuLogFile=Project_pathname(0)+'/ncprograms/'+map_key($TP.name)+'_log.tap'
REAL ToolLengthComp=entity('tool',$TP.Tool.Name).Overhang
EDIT PAR 'SimulationState.Issues.Collisions.CheckCollisions' 0
EDIT PAR 'SimulationState.Issues.CheckReconfigurations' 0
EDIT PAR 'Powermill.Simulation.Issues.PlaybackSetting' 'never'
SIMULATE TOOLPATH $TP.Name TOOLBAR SIMULATION RAISE
SIMULATE END
INT SL=simulation_location().Point
SIMULATE REWIND
EDIT PAR 'Powermill.Simulation.Step' 'point'
EDIT PAR 'Simulation.Speed' 100
FILE OPEN $SimuLogFile FOR WRITE AS simu
REAL ARRAY Prev[]={-9999,-9999,-9999,-9999,-999}
STRING Out=''
DO {
CALL GetMachinePosition($Config,$Axes,$ToolLengthComp,$Prev,$Out)
IF $Out != '' {
FILE WRITE $Out TO simu
}
SIMULATE STEP FORWARD
} WHILE simulation_location().PoINT < $SL
CALL GetMachinePosition($Config,$Axes,$ToolLengthComp,$Prev,$Out)
IF $Out != '' {
FILE WRITE $Out TO simu
}
FILE CLOSE simu
}
FUNCTION GetMachinePosition(STRING $Config,STRING LIST Axes,REAL ToolLengthComp, OUTPUT REAL ARRAY Prev[],OUTPUT STRING Out) {
REAL ARRAY Pos[]={0,0,0,0,0}
$Pos[0]=round($Machine().X,4)
$Pos[1]=round($Machine().Y,4)
$Pos[2]=round($Machine().Z-$ToolLengthComp,4)
SWITCH $Config {
CASE 'ABXYZ'
$Pos[3]=round($Machine().A,4)
$Pos[4]=round($Machine().B,4)
BREAK
CASE 'ACXYZ'
$Pos[3]=round($Machine().A,4)
$Pos[4]=round($Machine().C,4)
BREAK
CASE 'BCXYZ'
$Pos[3]=round($Machine().B,4)
$Pos[4]=round($Machine().C,4)
}
$out=''
INT I=0
WHILE $I < 5 {
IF $Prev[$I] != $Pos[$I] {
IF $Out !='' {
$Out=$Out+' '
}
$Out=$Out+$Axes[$I]+$Pos[$I]
STRING CMD='$'+'Prev[$I'+']='+$Pos[$I]
DoCommand $CMD
}
$I=$I+1
}
}The 0/ 360 a problem one possible solution: extend teh B-axis range 0-720, then in the Move Linear/ Move Rapid Commands change the Machine B parameter Value to expression: "(%p(Machine B)%) % 360" aka modulo 360.
The result:
Forums Links
Can't find what you're looking for? Ask the community or share your knowledge.
Post to forums
