www.kxcad.net Home > CAM Index > EdgeCAM Index >
Sequence Name - Specifies a new name for the current machining sequence.
Kit Name (only displayed if a Tool Library is active (Options menu, Preferences, Tool Libraries tab)) - Specifies the name of the tool kit to load. Toolkits from EdgeCAM's Tool Library contain a list of pre-defined tools.
Code Generator
Machine Tool - Selects a Code Generator file for the machining sequence. This file defines which machining commands are available and controls the output of the CNC code.
When switching milling code generators, you can only
switch to a code generator that is of the same type as the current one.
For example if you currently have an 'adaptive' code generator selected
(based on an adaptive template), you will only be able to switch to another
adaptive code generator (other types are filtered out from the list).
You can only successfully switch to a code generator
with the same capabilities as the current one. For example, moving C axis
operations to a turning centre not equipped with a C axis control would
result in an incomplete machining instruction list.
Component and Machine Setup
These settings are for Milling Machine Simulation milling only. They are unavailable for lathes and if there are no machine graphics in the code generator.
The settings position the machine graphics around the part, by bringing the 'Mating Location' of the machine and the origin of the 'Mating CPL' (one of the part CPLs) together. (Note how in World coordinates, it is the machine which is adjusted to the part; the part remains stationary). The Z axis of the Machine graphic aligns with the Z axis of the initial CPL. See illustrations...
The settings were originally made when you created the sequence. Edit them here if, for example, you realise you need to re-position the part after machining it and running a simulation - see an illustration.... (To be more accurate you are re-positioning the machine, in World coordinates.)
Mating Location - Select a 'Component' location point within the machine where the part is to appear. When left at 'None' this default to the first 'Component' location defined in the code generator. These locations have been configured into the code generator using Code Wizard - see the code wizard help for more details. If there is no component location in the code generator all the Component and Machine Setup options are unavailable and the machine graphics are given a default location.
Mating CPL - Select the part CPL whose origin you want to be placed at the 'Mating Location'. When left at 'None' this defaults to the active CPL set in EdgeCAM.
X/Y/Z Mating Offset - A distance to move the Mating location on the machine, which re-locates the part within the machine.
Initial Plane - Specifies the absolute height of the initial plane, used to move around at the rapid rate. The default value is set in the code generator.
Note that while toolchange and home positions are defined
in world co-ordinates the initial plane is defined from the initial CPL
of the sequence. These two datum points may be different.
You must ensure that this height is clear of any obstruction
including holding devices and material.
Output Tolerance - Specifies the smallest distances that the Code Generator can define in the CNC output file. Also see Note on conversion of arcs to lines below.
Units - Selects the units (mm (millimetres) or inches) that the final CNC code is to use. Any units used in the model are automatically converted. The default value is set in the Code Generator.
Max High Feed (milling only) - Specify a value for a high feedrate to use instead of rapid moves to ensure that the tool is moved in a straight line and no unresolved or 'dog-leg' moves are produced.
Rapid 3D - Check to allow the
tool to rapid move in all three axes. Each axis may accelerate
to rapid at differing rates. There is therefore a risk of collision as
the resulting move is not easily predictable. Refer to your machine tool
documentation.
Spindle Priority Mode - This
is only available in turning, and with the later 'adaptive' code generators.
Check this to prevent conflicting spindle control being programmed into
the sequence - the Toolchange dialog Spindle Control tab settings will
be unavailable in the non-priority turret. Uncheck this if you want to
be able to program conflicting information, and resolve this when you
add Synchronise Turrets instructions to the sequence.
Note on conversion of arcs to lines
EdgeCAM converts an arc move to a linear move when the chord height (see this illustrated) of the arc is less than the output tolerance of the machining sequence. The output tolerance is normally set to the same precision as the controller's decimal point format. For example 0.001mm or 0.0001 inch.
EdgeCAM performs this conversion to inhibit the output of potentially invalid arc moves which could cause an error on the controller where
arcs have a radius greater than the control can interpret. This can be encountered in smoothed surface toolpaths.
the arc start and end positions are so close that when formatted they are the same position. This can result in the controller interpreting it as a complete circle move.
the arc start or end positions in one axis are close enough to become the same position when formatted. This can result in the controller reporting an error that the point does not lie on the arc.
