Tool Parameters
The Tool parameters area displays the parameters of the selected tool.
If you edit the parameters of a tool used in two or more operations, a warning message is displayed listing the operations that are affected by the change.
The default state of the Don't ask me again option is defined in SolidCAM settings.
Angular dimensions
Using the right-click menu, you can swap the angle value from the degrees/minutes/seconds format to the decimal format and vice versa. You can also use the Undo, Copy, Cut, Delete and Paste commands.
Diameter
This field defines the cutting diameter of the tool.
Shoulder Diameter
This field defines the diameter of the shoulder cylinder (lower cylinder).
Arbor diameter
This field defines the diameter of the tool arbor.
Thread diameter
This field defines the diameter of the thread of the Tap tool.
|
This parameter is relevant only for Tap tools.
|
Tip Diameter
This field defines the lower diameter of the conical part of the Tap tool.
|
This parameter is relevant only for Tap tools. |
Chamfer Length
This field defines the length of the conical part of the Tap tool.
|
This parameter is relevant only for Tap tools. |
Pitch
This field defines the pitch of the Tap tool. The Pitch is the distance between corresponding vertices of adjacent teeth of a thread.
|
This parameter is relevant for Tap tools.
|
Corner Radius/Angle
When the tool type is End mill, Ball nose mill, Bull nose mill the Corner Radius field is displayed. When the tool type is Drill, the Angle field is displayed.
Corner Radius
This field defines the corner radius of the tool. There are three possibilities:
In End mills, the corner radius is zero. In Ball nose mills, the corner radius is equal to the radius of the tool. In Bull nose mills, the corner radius is smaller than the radius of the tool.
Angle
This field defines the drill point angle of the tool (between 0.01 and 180 degrees).
Length
This field defines the length of the tool. In milling calculations, the system does not use this data; the length of the tool is only output to the GCode file. In iMachining calculations however, the Technology Wizard does use the data defined for the Outside Holder and Cutting length parameters.
Total
This parameter defines the total tool length.
This parameter defines the length of the tool outside the tool holder.
The iMachining Technology Wizard modifies the Chip Thickness based on the extension of the tool outside the tool holder. As the Outside Holder length increases, the Chip Thickness is reduced.
This parameter defines the length of the cutting part of the tool.
When a new tool is created in a SolidCAM operation, its Cutting Length is automatically assigned the value of the machining depth in this operation. The depth is determined as follows:
For Face Milling, Profile, Pocket, Drilling, Thread Milling, and Slot (with constant section) operations, the Depth parameter is defined directly in the operation interface.
For Drill Recognition and Pocket Recognition operations, the Depth parameter is automatically determined as the depth of the deepest hole/pocket machined in the operation.
For Contour 3D, 3D Drilling, 3D Engraving, HSM, Slot (with shaped section), T-Slot, Translated Surface, Sim. 5-Axis and HSS operations, the Depth parameter cannot be automatically determined – the default hard-coded value is used for the new tool length definition.
iMachining 2D and iMachining 3D operations, the Depth parameter is automatically determined as the depth of the lowest feature but the default hard-coded value is used for the new tool length definition.
In Automatic mode, the iMachining Technology Wizard uses the Cutting length of the tool to calculate if multiple steps are needed to achieve the total depth.
Shoulder Length
Shoulder length defines the length from the tool tip till the start of the upper cylinder (defined with the Arbor diameter).
This parameter defines the distance from the tool end to the CNC-Machine spindle.
Click 
to view
the H Length dialog box.
In the According to Touch Point field, select the required cutting point from the drop-down list. The H Length value is automatically calculated and displayed in the H Length field. You can customize the H Length by manually entering a value in this field. SolidCAM automatically updates the Outside Holder Length depending on the value of H length entered.
Helical Angle
The flutes of a milling cutter are almost always helical. If the flutes were straight, the whole tooth would impact the material at once, causing vibration and consequently reducing accuracy and surface quality. The flutes being set at an angle allows the tooth to enter the material gradually, which helps to reduce vibration.
The drop-down list contains five typical helical angles available for selection:
- 0 (Straight)
- 30 (Standard)
- 35 (Standard)
- 45 (Medium) (default selection)
- 60 (High)
If necessary, a value can be entered manually ranging from 00 to 900.
This parameter is not available for the following tools types: Engraving, Probe, Broaching, Bore and Tap.
|
Warning: When cutting, keep in mind that the helical angle has a strong effect on the Downward Force on the tool, which should be monitored. If ignored, it can result in the tool being pulled out of its holder. |
Number of flutes
This field defines the number of teeth of the tool. This field is used when calculating the feed in the Feed rate type FZ.
The iMachining Technology Wizard relies on the correct Number of flutes to ensure the proper Chip Thickness is given to each flute.
Rough tools
SolidCAM enables you to define rough tools of all the following types:
The Rough check box enables you to mark the tool as suitable for rough milling. The Rough status of the tool can be used for the tools sorting with the Range option.
Related Topics