Source operation
This page enables you to choose original operation that will be converted and define a number of the conversion parameters.
Source operation
In this section, you need to choose the operation to be converted from the corresponding list. Currently, convert HSM to Sim 5. Axis Milling supports tool paths of 3D HSR, 3D HSM, Turbo 3D HSR and Turbo 3D HSM modules.
The Disassociate button cancels the connection between the source operation and the converted one.
|
The 3 Axis tool path created with only Ball nose mill tools will be availabe for HSM to Sim. 5 Axis conversion. |
Conversion data
The Cut tolerance value defines the tool path accuracy.
The Arc approx. tolerance enables you to create G2/G3 GCode output. SolidCAM checks whether successive points of the calculated tool path can be connected using an arc or a circle. If arc or circle connection within the specified arc approximation tolerance can be made, you receive arc and circle interpolation commands G2 and G3 in the generated GCode.
This feature can drastically reduce the number of lines in GCode files. Most CNC-controllers and machines work much faster on arcs and circles than on single tool path points or splines. Arc approximation will increase actual feed rates on older CNC-Machines and the machine will work smoother. The Tolerance value defines the tolerance SolidCAM uses to position tool path points on arcs or circles.
|
The arc approximation value should be smaller than the specified value for the surface offset. A warning message is displayed if a larger value could cause gouging of the model. |
The Max. distance option enables you to limit the distance between two adjacent points on the tool path when using the Conversion technology.
The Conversion link type option enables you to choose between using the original source links from the HSM operation or relinking the tool path. When the Relink option is chosen, the options in the Levels and Link pages become available for editing.
The Contour feed rates option lets you use the feed rates defined in the converted operation or define new feed rates. The New feed rates option in the list allows you to define the feed rates in the Data tab available on the Tool page. The Feed rates from input tool path option allows you to keep using the same feed rates from the converted operation.
|
The options of Conversion link type, Contour feed rates are available only with the Conversion technology. |
The Workpiece clearance
option allows you to set a value by which the tool clears the
workpiece when moving between two positions. This value
defines the offset that has been used for creating the 3 axis
tool-path
|
|
Plunge moves after conversion (in case of axis 5)
This section allows you to either Keep feed rates at plunge moves after conversion or to change them to machining feed using the Change rapid feed rate to machining feed rate option.
|
This option is available only with the Conversion technology. |
Input tool path points
The Input tool path points allows you to maintain the number and distribution of points on a high quality tool path by either keeping the input points or applying a filter for conversion.
Keep input points- Selecting this option allows you to maintain the number of tool path points.
Apply filtering for conversion- Selecting this option allows you to find additional points from the 3-axis input and trim them.
Points are added when the tool path is converted to 5-axis in order to provide the best angle step tilting. In case, the cutting tolerance of the conversion is not in the range of the number of input tool path points, the chances of points being filtered is less likely.