Finding the right balance of speed and safety is critical for SOLIDWORKS CAM programmers. Clearance, Rapid and Feed Planes allow us to control how far away the tool will engage or clear the work. Keeping the tool down while cutting saves time.
Retracting to a safe level may help with chip removal and minimize potential crashes and gouges, more time. I will leave it for you to decide. These options are found in the NC tab when you Edit Definition on any operation.
SOLIDWORKS CAM Clearance Plane
SOLIDWORKS CAM Clearance Plane is the absolute Z location the tool rapids to before feeding down in the Z axis. It is also the height the Z axis positions to during rapid moves to get from one cut to another with the same tool.
The Clearance Plane location can be set relative to different depths:
Top of Feature
Specifies that the clearance Z plane, that the tool retract to, will be at an incremental Distance above the top of the feature.
Specifies that the tool retracts to a clearance Z plane that is an incremental Distance above the Setup origin.
Previous Machined Depth
Specifies that the tool retracts to a clearance plane that is always an incremental height above the previous cut depth. The initial clearance plane will be an incremental amount above the top (face) of the feature.
Top of Stock
Specifies that the tool retracts to a clearance Z plane that is an incremental Distance above the Stock. This option will be valid only for Mill Part Setups that are normal to the default SOLIDWORKS planes: Plane1, Plane2 or Plane3.
Specifies that for Rough Mill and Contour Mill operations, SOLIDWORKS CAM automatically computes a minimum safe Z retract position between each cut level within a feature. Only the feature geometry and avoid area geometry is considered in the computation.
For 2.5 Axis VoluMill toolpaths, SOLIDWORKS CAM will limit the Clearance level above the feature top (in Z axis direction) by the Floor Clearance value defined in the VoluMill Settings dialog box.
This value is the incremental distance above the specified location that defines the Z value of the Clearance plane.
For the Skim option, this value defines an amount to clear above the highest Z of the feature or avoid area between the retract of one level and the plunge of the next.
SOLIDWORKS CAM Rapid Plane
The Rapid Plane is the absolute Z location at which all XY rapid moves are executed from. The Rapid Plane is also the height the Z axis returns to when the operation is complete. The amount that you specify here should take into consideration any clamps on the part.
The Rapid Plane location can be set relative to four different depths. Following are the options available:
Top of Feature
Specifies that the rapid Z plane will be at an incremental Distance above the top of the feature.
Specifies that the rapid Z plane will be at an incremental Distance above the Setup origin.
Specifies that the rapid Z plane will be at an incremental Distance above the Clearance Plane for 2 Axis operations. Specifies that the rapid Z plane will be at an incremental Distance above the value of the Skim clearance parameter on the Entry Retract tab for 3 Axis operations.
Top of Stock
Specifies that the rapid Z plane will be at an incremental Distance above the top of the stock. This option will be valid only for Mill Part Setups that are normal to the default SOLIDWORKS planes: Plane1, Plane2 or Plane3.
This value is the distance above the specified location that defines the Z value of the Rapid plane.
SOLIDWORKS CAM Feed Plane
Feed plane is (group box and associated parameters not available for Rough Mill operations with VoluMill Pattern). This option allows the Z Feed plane to be set relative to the Previous Machined Depth or the Current Machined Depth.
Previous Machined Depth
If set to Previous Machined Depth, the tool rapids down in Z to the Clearance plane and then feeds down in Z to the cutting depth.
Current Machined Depth
If set to Current Machined Depth, the tool rapids down in Z to a position above the cutting depth equal to the Distance amount, then feeds down in Z to the cutting depth.
When the Feed plane is set to Current Machined Depth, this parameter defines a distance above the current cut depth that the tool should begin feeding in Z. If the value is 0.00, the tool will rapid to the Z cutting depth.
The Feed Plane is option is not supported for point to point operations viz. drilling, reaming, boring, tapping, etc.
Retract between features
Group box and associated parameters not available for Rough Mill operations with VoluMill Pattern.
Use skim plane
When machining multiple features with a Rough Mill or Contour Mill operation, this option allows you to specify a retract location between features. The Z retract position is based on the perimeter and island geometry for the features being machined by the current operation as well as any avoid areas.
When the ‘Use skim plane’ option is not checked:
When the ‘Use skim plane’ option is not checked, the tool retracts to the Rapid plane between features.
When the ‘Use skim plane’ option is checked:
When ‘Use skim plane’ option is checked, the tool rapids vertically to the minimum Z height needed to clear the feature perimeter, islands and avoid areas, moves in XY to the start of the toolpath for the next feature, then feeds down vertically to the first cut depth.
When Use skim plane is selected, this parameter defines the minimum distance above the feature perimeter, islands or avoid areas to rapid from the end of one feature to the start of the next.
Rapid plane (G98) / Clearance plane (G99)
For single point operations, these options allow you to specify whether the tool retracts to the rapid plane or the clearance plane.
Use Setup Definition
The definition of Planes can be done locally for each operation in the NC tab or globally from the Mill Part Setup level. The Use Setup Definition checkbox option allows you to choose whether to use the global Mill Part Setup definition or to use the local definition for this operation.
To define any of the above planes locally for an operation, ensure that the Use Setup definition checkbox option within the Plane is group box is unchecked. Use the parameters within this group box to define the Rapid Plane Z depth.
If you want to use a global setting, define the Rapid plane on the NC Planes tab in the Part Setup Parameters dialog box (Part mode) or the Setup Parameters dialog box (Assembly mode) and then place a check in the Use Setup definition option within the Plane group box under the NC tab for each operation.
When the Use Setup Definition check box option is checked, all the parameters within the plane group box will be disabled.
Get Certified SOLIDWORKS Services from Javelin
Javelin Experts can help you to: