Using the Rationalise Command

Did you know you can re-order the instructions in the active milling sequence using the Rationalize command?

In the milling environment, you use the Rationalize dialog to re-order the instructions in the active sequence by ‘Tool’, ‘CPL’ or ‘Index’.

Before running the Rationalize command, you will need to set the ‘Sort Priority’ of the tools in the sequence.  The Sort Priority can be found on the ‘More’ tab when editing the tool.  Lower Sort Priorities are placed above higher values, so give toolchanges a value that will produce the correct order of machining, such as:

100 = Roughing
200 = Semi roughing
300 = Semi finishing
400 = Finishing
500 = Centre Drill / Spot face
600 = Drilling
700 = Tapping / Reaming / Boring

The Rationalize can be found in Instructions\Rationalize or you can access the command by right mouse clicking on the active sequence.

The dialog options are:

Strategy – Choose how you want to re-order the sequence:
•  By Tool – Reorders the sequence based on the toolchange instructions.  Instructions are moved in blocks that start with a toolchange instruction and extend to the instruction before the next toolchange.
o  The toolchanges (along with their ‘block’) are placed in order of their Sort Priority value. The lowest value is placed highest up the sequence.

A blank value is treated as ‘0’. If tools have the same Sort Priority, the sort on priority will group them together and their order within the group will be determined by their original (pre-rationalise) order.

o  All the repeat toolchange instructions (that is toolchanges back to the same tool) are then deleted. To be the ‘same tool’, all the toolchange parameters must match (Turret Position, Diameter, Offset and so on), as well as the Sort Priority setting.

•  By CPL – Reduces index moves by grouping together instructions that have:

o  The same rotary axis positions (as specified by Move menu ► Index). Any necessary retracts to safe distance are kept/inserted before the indexes.

o  The same datum (as specified by Move menu ► Index and/or M-Functions menu ► Datum Shift).

•  By Index – This produces the same result as by ‘By CPL’ above, except that the instructions datum is not taken into account.

Merge Hole Cycles – (Only available with Strategy set to ‘By Tool’)  Check this for the separate Hole cycles under a toolchange to be merged into one Hole cycle that machines all the holes.

Milling Safe Clearance – Retract moves to a safe clearance height may be inserted; before inserted index and datum shift instructions for example.  For these moves, specify how the safe Z value is to be derived:

•  Toolchange – The ‘Z Change’ parameter, as set in the Machine Parameters dialog, Tool Change tab

•  Max Clearance – The Maximum ‘Clearance’ value (as found in a Roughing cycle’s Depth tab, for example) of any of the instructions that are moved.
•  Z Initial – The ‘Initial Plane’ parameter, as set in the Machine Parameters dialog, General tab.

•  Safety Zone – Check this if you want to specify and ‘exclusion zone’, which determines the safe clearance height for the tool to retract to.  You use the ‘Safety Zone’ options (below) to specify the shape and extent of this zone.

Safety Zone – The Safety Zone options are only available with ‘Milling Safe Clearance’ set to ‘Safety Zone’.  Use these options to specify the shape and extent of an ‘exclusion zone’, which determines the safe clearance height for the tool to retract to.

•  Clearance Type – The shape of the safety zone.
o  None – No safety zone set.  If required, you will need to move the tool manually to a safe position.
o  Level – Safety clearances are referenced to a plane, relative to the Initial CPL. This is generally used when indexing and approach moves need to be above the component. Ideal for head/head and head/table machines where the tool can move above the component
o  Radius – Safety clearances are defined as a radius.  This option is generally used on  head/table machines. The tool will retract a radial distance from the centre of rotation or a specified CPL.
o  Sphere – Similar to the 5-Axis clearance type, safety clearances are referenced not to a ‘plane’ but a sphere

•  Distance – Specifies the extend of the safety zone.

•  Origin – (Only available with ‘Clearance Type’ set to ‘Radius’ or ‘Sphere’) Select a reference origin from a drop-down list. Please note that availability of this option is dependent on your machine configuration.

Bestill vårt nyhetsbrev

autorisert forhandler av