Contour and Pocket operations
IN THIS ARTICLE
Under the Mill menu, you can find Contour and Pocket operations.
This 2 machining operations are identical except the fact , by default , contour will work the outer area of selected profiles, and pocket will work the inner area of selected profiles.
Switch profile side
Is possible switch the side of selected geometry.
You can both click on the double sided arrow in geometry list box or click the yellow arrow in viewport . When you hover the yellow arrow with mouse cursor , the arrow will turn red. Click on it to change working side.
The highlighted area in viewport , will be the area machined away by the operation.
Open Profiles
Contour and Pocket operations need a closed profile to work with.
If you select an open profile instead, eCam will try to close it with the outer stock profile.
See image.
Also in this case you can switch working side .
Z Levels
Safe Z : is the Z Plane where the tool approach in rapid movement
Start Z : Is the z plane where the tool start remove material
Depth : Is the thickness of material to be removed , measuered from Start Z
By default these values are applied to all associated geometries.
But if you enable the " DEFINE Z LEVELS FOR GEOMETRY" , these value are applied only to current geometry. The current geometry is highlighted with red strokes in viewport and active in geometry list box
Machining area from profile offset
Roughing plunge points
To force plunge point position for roughing operation, enable "Select Plunge Point" to pick to position with mouse.
If plunge points are defined , the plunge mode will be disabled . Be sure the plunge point positions are in a stock free area.
Use [Clear Points Selection] to remove all defined plunge points.
Finishing Start Points
Is also possible define finishing start points. Use [Define starting points] under finishing operation.
Use [Clear Points Selection] to remove all defined plunge points.
Keep Tool Down
By default, after every pass in Z direction, the tool move to [Safe Z] level . The reason is to keep the maximum safety in toolpath creation.
But if you see there is no issue with stock collision, you can enable [Keep Tool Down] . In this way the tool goes directly to next z level , without moving to [Safe Z] after every pass.
You have 2 different [Keep Tool Down] options, one under roughing operation and one under finishing operation. So you can have active in one operation and disabled in the other.
Finishing Offset
Is possible apply a negative or positive offset value to profile. With this you can remove more or less material from stock with finishing tool.
Custom machining area
Is possible customize the machining area by different modes:
- Defined stock - The machining area is defined by the original stock
- By Custom selection - Is possible select the CLOSED profiles to define the machining area.
- By machined stock section - It will consider the machined stock until the current operation.
The option "By machined stock section" is computationally expensive.
Where applicable, use the "By custom selection" , which is more light to process.