www.kxcad.net Home > CAM Index > EdgeCAM Index >
Sequence Name - Enter a descriptive name for the new machining sequence (eg. 'OP1'). Please note that each machining sequence must have a unique name.
Choose a Code Generator
Discipline - Select the appropriate machining discipline, Mill, Turn or Wire. This filters the available Code Generator files that appear under Machine Tool.
Machine Tool - Select the appropriate Code Generator file. The Code Generator defines which commands and options are available within the EdgeCAM manufacturing environment. The Code Generator also formats the CNC code to suit your machine tool. The code generator can also contain machine graphics and the kinamatic information required for Machine Simulation.
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...
You can subsequently change these settings, if required, by editing the sequence (M-Functions menu ► Machine Parameters for example).
Mating Location - Select a 'Component' location point within the machine where the part is to appear. When left at 'None' this defaults 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 are no component locations 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..
Mating Offset - Check this if you want to digitise a point where the Mating Location of the machine (see above) is to be placed. This overrides the 'Mating CPL' setting above.
Initial CPL - (For wire erosion this must always be set to ‘Top’). Choose a CPL to be the initial Output Coordinate System. This is the coordinate system that the CNC code X, Y and Z coordinates are relative to. This also becomes the initial working CPL as you enter Manufacture mode (the tool is oriented parallel to the CPL Z Axis).
Kit Name (only displayed if a Tool Library is active (Options menu, Preferences, Tool Libraries tab) - Select a predefined kit of tools for the machining sequence. This option is .
Machine Datum - (Milling and turning only). Check this if you want to digitise a position for the machine datum. For example if the machine datum was on the back of the main spindle, you would digitise a Machine Datum position somewhere behind your part geometry, on the centre line.
The 'machine datum' is the origin for the tool change and home position coordinates (see an illustration). In milling this is also the point in milling about which the rotary axes rotate (see an illustration). (Or for a four axis machine it is the first rotary axis origin).
In milling Machine Simulation the machine datum is defined in the code generator, and is therefore automatically placed according to your 'Mating Location' and 'Mating CPL' settings above. In this case you should only check Machine Datum if you need to override this automatic position (although this is not recommended).
If not otherwise positioned (that is Machine Datum unchecked and with no 'mating' information), the machine datum is placed at the origin of the selected 'Initial CPL' (in turning - see above), or at the origin of the 'Top' CPL (in milling).
Checking this option makes 'Part Stick Out' in the Lathe Setup tab unavailable (using Part Stick Out is an alternative way to position the machine datum).
For accurate simulation
(especially if this is full Machine Tool Simulation), it is important
that you position Machine Datum correctly. (As well as specifying other
critical dimensions such as tooling gauge distances.)
To help visualise the machine datum, you can display the primary and secondary axes by selecting the Machine Datum check box on the General tab of the Configure View menu dialog.
Output Tolerance - Specifies
the smallest distances that the Code Generator can define in the CNC output
file.
In general you should set the output tolerance to the same precision as
the controller's decimal point format. For example 0.001mm or 0.0001 inch.
Note that 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. 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.
Datum Type - (Milling only) Specify the type of coordinate shift from the World Co-ordinate System origin:
Absolute - This typically invokes a co-ordinate datum position on the machine tool similar to a G54. This must be supported by the code generator and machine tool.
Incremental - This typically invokes a co-ordinate system shift similar to a G92 (reselection is not easy from another co-ordinate system).