FAQ - AdvantEdge™ Production Module

What is the Tolerance for Arcs feature?

It will set how Face Milling will approximate an arc from a toolpath. Input values can range from 0.0001 to 1. The smaller the arc radius, the smaller the value that needs to be input. If you receive an error saying "Unable to Create Sweep Geometry" when running a force model, try decreasing the Tolerance for Arcs input value. A good practice is to decrease the value by 10 until the force model runs.

What is the proper workpiece orientation in 2D?

Face Milling: face to be milled should be in the XY Plane and the face should be normal to the Z axis.

Drilling: the part should be centered along the Z axis, with the Z axis pointing normal to the face of initial contact.

Turning: the workpiece should be oriented so that the axis of rotation is along the Z axis.

What does each force represent?

The tangential, radial, and axial forces are forces acting on the tool, the direction of which is determined by the cutting direction. The instantaneous X force is the total of the X components of tangential, radial, and axial forces. If sum of components points in negative X direction of the global coordinate system, the X force will be negative.

What is tool compensation?

Tool compensation allows user to account for things such as tool wear. Tool compensation is only necessary if it is defined in the G-code. For example, a G-code might have a line such as this: N1010 G41 X-25.00 D01 F3.0. The G41 command tells you that the compensation should be read in for D01. In AdvantEdge™ Production Module you would need to enter the register as 01 and the value would be whatever the compensation value should be. If you do not want compensation, enter register as 01 and value as 0.

What can I do if my toolpath does not appear correctly?

If the tool path does not extend as far as it should and there are circles where there should not be, it is possible the toolpath goes beyond the current limitations set for your machine. The transient file (Transient.tra) defines the maximum travel of your machine. Increase the xmax, ymax, zmax, xmin, ymin, and/or zmin to a larger number that will allow for your machine to travel the necessary distance defined in your toolpath.

If you are using G-code and your toolpath does not appear correctly make certain that the correct parameter file is being used. The parameter file needs to explicitly define the type of arc definition used in the G-code files. Some of the arc (I, J, K) values are defined as a distance from start to the center. You would have to use Fanuc_DEL.Production Module for such files. Some of the arc (I, J, K) values are defined as the absolute center coordinates. You would have to use the Fanuc_ABS.Production Module for such files.

What do the variables in the transient file mean?

Following are descriptions with units of all variables in the transient file:

txacc, tyacc, tzacc – These variables are the time it takes the selected axis to accelerate to full speed in seconds.
txdec, tydec, tzdec – These variables are the time it takes the selected axis to decelerate to full speed in seconds.
vxmax, vymax, vzmax – This is the maximum feedrate for each axis and is defined in mm per min.
tArotcw – The amount of time a tool change takes, in seconds from the tool change position.
spindlefactor1, spindlefactor2, spindlefactor3, spindlefactor4 – Do not change these parameters.
Spindle rProduction Module ™max – Maximum spindle speed in revolutions per minute.
Rotary A rProduction Module ™max, Rotary B rProduction Module ™max, Rotary C rProduction Module ™max – Maximum rotary spindle speed in revolutions per minute. This parameter only needs to be changed for the specific axis used in your toolpath.
feedlim – This is the maximum combined feedrate for the machine in mm/min.
xmax, ymax, zmax – These are the maximum travel values for your machine in mm.
xmin, ymin, zmin – These are the minimum travel values for your machine in mm.