The General Properties section is found on the NC Output tab of the SolidTurn Machine Setup. General Properties are used to control the format for posted code through use of the following settings:
- Program Name
For NC machines that accept this value, enter a program name. The name is typically output near the top of the program file.
- Program Number
Enter the program number output at the top of the program file. This is a useful way to distinguish one program from another. This number is often referred to as the "program ID number".
- Coordinate Mode
Specify how tool positions are determined. NC code output for most machines is G90 for absolute and G91 for incremental.
- Absolute: All positions are referenced from the origin
- Incremental: All positions are referenced from the previous position.
Unit for NC Code
Specify the unit of measurement for the NC code in either inch or metric units.
- NC Code Output
Click the 'Settings' button to associate one or more post-processor files with this machine setup.
Spotlight: Tool Editor Add-in
The Tool Editor Add-in is a function that can be found on the Common Machining toolbar. This function greatly simplifies the process of editing tools and their parameters by allowing the user to edit multiple tools without having to open each tool technology page individually. The parameters that can be adjusted for tools range from the tool number, offset number, and simulation cut color, to feeds and speeds for tools associated to operations.
Spotlight: Tool Change Position Convention for Swiss Machines
Tool change positions control the behaviour of tools when they are finished machining and approaching a tool change. When defining a tool in ESPRIT that is used for Swiss machines, it is generally recommended to use the following conventions for the Tool Change Position setting.
Axial tools refer to tools aligned parallel to the turning axis of the machine. Generally, it is not desired to have axial tools position along the X or Y axes after machining. Moving along these axes is oftentimes unnecessary, so commanding the tool to do so leads to longer cycle times and unnecessary risk.
Positioning the Z axis after machining is sometimes necessary. On the main spindle, a Tool Change Position Z of “Home” will cause the stock to retract into the guide bushing. On the sub spindle, a Tool Change Position Z of “Home” will cause the sub spindle to retract to its home position. Depending on whether the user desires this retraction, Tool Change Position Z can be set to “None” to prevent it. The convention for Tool Change Position when using axial tools is as follows:
Position X: None
Position Y: None
Position Z: Home(or None)
Radial tools refer to tools aligned radially from the turning axis of the machine. Like axial tools, it is unnecessary to position along the Y or Z axes. The X axis is typically positioned at its home position, so that the tool is clear of the stock after machining has occurred. The convention for Tool Change Position when using radial tools is as follows:
Position X: Home
Position Y: None
Position Z: None
Cutoff tools conventionally remain positioned in front of the stock after the cutoff has taken place. This is to ensure that the stock maintains its position along the Z Axis. The convention for Tool Change Position when defining a cutoff tool is as follows:
Position X: None
Position Y: None
Position Z: None
Spotlight: Solid Modeler Toolbar
The Solid Modeler toolbar is used to create and manipulate solid models using the following functions.
- Extrude Boss/Cut Solid
Extrude Boss/Cut Solid creates a solid model by projecting a planar profile along a normal vector.
- Revolve Boss/Cut Solid
Revolve Boss/Cut Solid creates or modifies a solid model by rotating a profile around an axis at any angle from 0 to 360 degrees.
- Constant Fillet
Constant Fillet puts a fillet on the edges of a solid model.
- Edit Fillet
Edit Fillet modifies fillets on the edges of solid models or generates a spine curve.
- Chamfer
Chamfer puts a chamfer on the edges of a solid model.
- Split Face
Split Face splits one or more faces of a solid model along a system-generated path.
- Merge Faces
Merge Faces merges a group of tangent faces into a single face or a single surface.
The rough pass of a Cutoff operation uses the features end point along the Z axis to determine where to apply the rough pass. This means that two features with entirely different shapes can create the same toolpath if they share an end point position along the Z axis. This is useful to know in cases where the backmost part of the turning profile is not a vertical segment. It is important to note that unlike the rough pass of a Cutoff operation, the finish pass will follow the shape and direction of the profile when added to the operation.
Spotlight: Create and Remove From Feature Set
Create Feature Set and Remove From Feature Set are functions that are found on the Feature Accessories toolbar, and are used to organize the Features tab of a program.
Create Feature Set creates a feature set, or folder, from a group of selected features. To use it, group select the features and/or any operation associated to the features prior to running the command.
When all the member features are of the same feature type then the resulting feature set will allow processes to be applied to it for the creation of child operations on all of the member features along with a parent operation on the feature set itself.
This does not apply if the feature set contains a mix of different types of features (processes would have to be applied to individual features within the set, and a parent operation cannot be created on the feature set itself). Remove From Feature Set will remove the selected features and the features of selected operations from whatever feature set the feature is in.
To use it, group select the features and/or any operation associated to the features prior to running the command. If all features are removed from a feature set, then you will also be prompted if you want to remove the empty feature set.
Spotlight: Support
For any questions related to ESPRIT, reach out to Support at esprit.support@hexagon.com. Support is useful for questions regarding toolpaths, for outputting specific NC code in the posted program, and for installation help. If the question references a specific ESPRIT file, make sure to attach the ESPRIT file to the support request. Support is available between 8AM Eastern time to 5PM Pacific time Monday through Friday.
Spotlight: Properties – Editing Values
All elements in ESPRIT have properties. This includes elements such as geometry, features, and toolpath. There are geometric properties, such as X, Y, and Z coordinates, length, and radius values. There are attribute properties, such as color and line type. There are also associative properties like Layer, Work Plane, and Sub Elements, such as the arcs and line segments of a chain feature. All properties may be viewed in the Property Browser, but not all properties can be edited.
When you select an element in the graphic work area, its properties immediately appear in Properties. In general, to change a value, select it under the "Value" column. If it is editable, then you can type in a new value and press enter on the keyboard to confirm. The properties of multiple elements can be changed simultaneously as well. When selecting multiple elements, only the properties common to all selected elements appear. When changing a property value, that change is applied to all selected elements.
Spotlight: Clearance Parameters
Clearance is a parameter commonly found on the Links tab of many traditional milling cycles. The value entered is used to define a safety distance measured from the feature, so that the tool safely approaches and retracts from a machining operation. The values for Full Clearance and Clearance can be used in defining a Return Plane, a Retract Plane, or behavior for a Retract Between Cuts.
- Return Plane
The plane position of the tool before the start and after the end of the cutting operation.
- Retract Plane
The plane position of the tool between repositioning moves within the cutting operation. Repositioning moves take place when the tool completes machining in one area and retracts before machining another area.
- Retract Between Cuts
Sets the retract position before and after each lateral pass for contouring operations that have lateral stepover passes.
Spotlight: Custom Cycles
To create a Custom Cycle, select "Custom Cycle" from the Common Machining menu to display the custom cycle page. Custom Cycles can be used to output specified code if a post processor manual calls for its use, but the primary use of a Custom Cycle for any user is found on the Text tab of the cycle. The Text tab allows the user to enter hand-written NC code that is then output “as-is” at a user-defined location in the program.
Spotlight: Default Technology Manager
The Default Technology Manager is part of the KnowledgeBase in ESPRIT. It allows the user to define default values for parameters found in operation and tool technology pages and can be used in conjunction with expressions to improve automation within ESPRIT. Use the Default Technology Manager to reduce programming time and increase efficiency when working on similar projects.
Spotlight: Help
The Help includes descriptions and instructions for every feature and function found in ESPRIT. It can be found on the Menu toolbar by selecting Help > ESPRIT Help, or by clicking the question mark in the upper right corner of many technology pages. The Help is a powerful resource to help answer questions or obtain more information when needed. There are several ways to find information in this Help system:
- Use the menus at the top of each page to find topics organized in the logical order of steps needed to take you from design to finished part.
- Click Search to type a keyword and search for all topics that contain that word.
- Click Contents to find topics organized by area of interest.
- Click Index to find topic keywords in alphabetical order.
Spotlight: Simulation Tolerance
Simulation Tolerance is a user-defined tolerance found in Simulation Parameters that affects the accuracy of simulation objects that are not defined on the Solids tab. Some simulation objects, such as rounded tools and tool holders, are triangulated for simulation. Triangulation is a process where many adjacent triangles approximate the shape. The difference between these triangle approximations and the ideal shape is controlled by the Tolerance setting in Simulation Parameters. A smaller value for Tolerance creates a more precise simulation. A larger value improves simulation processing but reduces the quality.
No prerequisites required for this course.
No resources available for this course yet.
