Miscellaneous parameters page
This page contains the miscellaneous parameters for the operation.
Message
The Message field enables you to type a message that will appear in the iMachining GCode file.
Extra parameters
This Extra parameters table displays the list of additional parameters defined in the post-processor of the current CAM-Part.
If you prefer working with a larger window, the Flyout Window option displays the Operation Option window.
Z level sorting
When the 
mode is enabled in the Operation dialog box, the Z level sorting feature
appears on the Misc. parameters page.
The Retract after every cut option enables you to quickly disable detouring of the tool when repositioning from one cut to the next. When selected, the tool will retract up to the Clearance level and then reposition via a straight line movement before making the next cut.
Fit arcs
By default, this option is enabled to fit arcs in the iMachining GCode.
The Cutting angle tolerance parameter is used to group sections of iMachining tool path that fall within the specified tolerance, and then arcs are applied to those sections.
|
A small tolerance can greatly reduce the amount of GCode that is generated. It can be especially beneficial for machines with limited memory. |
Tolerance (Beta)- By default, the iMachining technology minimizes the arcs in the tool path according to a small arc fitting Tolerance. The result is many tool path points but very precise engagement angles. Click the Tolerance (Beta) check box to overwrite the default tolerance with a preferred, larger tolerance.
|
A large tolerance can greatly reduce the amount of GCode that is generated but also decreases the accuracy of the engagement angles. It can be especially beneficial for machines with limited memory. |
In process simulation
The Show tool path during calculation option enables you to display the iMachining tool path directly on the solid model during calculation.
|
This option is useful for verifying the iMachining tool path during calculation of the operation. |
Technology wizard
The Classic helical cutting conditions option automatically specifies a Ramping angle parameter of 2.5 degrees for the current iMachining operation.
Prior to SolidCAM 2012, the iMachining technology output the value of 2.5 degrees for all operations by default, which is believed to be the absolute safest maximum descent angle of a helical entry.
The Technology Wizard is now designed to automatically calculate the helical cutting conditions based on material hardness and aggressiveness of the Machining level slider.
|
If the value of 2.5 degrees is preferred, the Classic helical cutting conditions option can be selected. The Ramping angle override must not be used. |
Constant chip thickness control for arcs
When cutting in a straight line (G1), the Feed rate at the center of the tool is identical to the Feed rate at the wall of the workpiece (periphery feed). However, when cutting in a corner (G2), the periphery feed is much higher. As a result, tool wear increases due to undesired chip thickness (CT).
In iMachining calculations, the Feed rate is automatically corrected when cutting in corners in order to maintain a constant CT.
|
When milling aggressively, it is believed that a feed correction for arcs is critical. By maintaining a constant CT, it is proven that tool life is maximized because tool load is kept constant. In addition, it is more unlikely that dangerous Cutting conditions could develop. |
Since a constant CT is achieved by a reduced Feed rate, you may find an increase in cycle time. If you decide that a faster cycle time is more desirable than maintaining a constant CT, then you should consider using the Constant chip thickness control for arcs slider.
This slider enables you to control the feed correction for arcs. The position of the slider is set to 100% by default. If kept at 100%, the iMachining technology is informed to maintain a constant CT when cutting in corners.
Moving the slider to 0% informs the iMachining technology to maintain a consistent Feed rate between cutting in a straight line (G1) and cutting in a corner (G2). The result is a faster cycle time; but beware, with increased CT in corners comes increased tool load.