Application area:

ENCY Tuner is a software designed for machine operators working with CNC machines and industrial robots. As part of the ENCY X ecosystem, it focuses on managing NC programs at the shop-floor level. ENCY Tuner enables users to simulate, fine-tune, and re-engineer NC code (G-code) before sending it to the machine.

ENCY Tuner provides the following functions to accomplish these tasks:

It simulates NC program execution using an extensive set of monitoring tools. It tracks potential failures, including collisions, and the state of the workpiece after each operation, including unmachined areas part gauges. The system supports subtractive, additive, and hybrid process simulations using high-quality voxel or solid modeling. See more.
Users can build digital twins of the manufacturing systems with 3D models of equipment, tooling, and workpieces. These digital twins can serve as templates for future simulations with different NC programs.See more.
ENCY Tuner displays the final result of the simulated machining process and enables users to compare it with the target 3D model of the part. See more.
The software displays the positions of machine axes throughout the simulation process. See more.
Users can open and manage several NC program files in parallel, using functions such as file addition, removal, replacement, and renaming. See more.
ENCY Tuner allows users to analyze and compare the code in two different NC program files to track G-code revisions, their changes or inconsistencies. See more.
The system allows manual command-level editing within NC programs. See more.
ENCY Tuner provides live toolpath visualization throughout the NC code development process. See more.
ENCY Tuner simplifies program structuring by auto-inserting commonly used address templates such as block numbers. See more.
The system allows automated editing of command structures, including address fields and corresponding values. When editing addresses automatically, it ensures intelligent handling of dependent references such as block numbers. See more.
Users can retrieve detailed information on allowable ranges for command values, like position coordinates. See more.
The software performs toolpath transformations such as shifting by a specified value, rotating by a given angle, and applying mirror symmetry. See more.
Users can reformat control programs for use with alternative CNC control systems. See more.
ENCY Tuner lets users to create CAM project structures from existing NC code to enable further operations in ENCY ecosystem. Such it useful for teams with large libraries of old G-code from outdated systems.

Workflow:

Perform all operations with NC programs within the ENCY Tuner project environment. Each project utilizes:

one or more NC programs (See more);
an interpreter to translate G-code into technological operations and CLDATA commands (See more);
a postprocessor to transform edited operations into G-code (See more);
tools for editing NC programs (See more);
a technology tree with tools for editing technological objects (See more);
tools for simulating programs and technological operations (See more).

According to the defined objectives, work in ENCY Tuner can follow these procedures:

Creating a new NC program.

When ENCY Tuner starts, it automatically creates a new project, enabling the creation of a new NC program from scratch. The project automatically opens a new Code Editor Panel window. The Main Panel loads the machine used in the last project.

Click here to expand..

Load the machine you are planning to use for the machining process. See more.

2. Click on the Explorer button to open the Explorer Panel. See more.

3. Load the interpreter file that corresponds to the NC system for which you intend to write the NC program.

4. To translate the NC program to a different NC system format, upload the corresponding postprocessor file.

5. Type the NC program in the NC Code Editor Panel. It is not necessary to assign block numbers right away; you can add them later using the Block Numbers tools on the Main Panel in Edit mode. While typing the program, you can manually divide it into operations using the context menu tools. See more

6. After you finish entering the NC program, divide it into operations using the Split command in the Project Management Panel. See more. If the automatic split is not appropriate, change the operation divisions with the context menu options in the NC Code Editor Panel. See more

7. Use the Main Panel's tools in Edit mode to edit and format the NC program according to your needs. See more.

8. Configure technological operations using the commands on the Main Panel in Setup mode. See more. If needed, reassign tools for technological operations using the Tools on the Project Management Panel or the Tools tab on the Main Panel. If you have prepared your tool library in the CAM project earlier, load it using the Import Tools to the Project command on the Project Management Panel. See more.

9. To enhance debugging and simulation of the NC program, you can upload 3D models of the part, workpiece, and fixture, as well as create a workpiece and fixture using the respective tabs on the Main Panel in Setup mode.

10. Position the part on the machine using the Setup tab on the Main Panel. See more. To accurately align objects with machine nodes, enable the Smart Snap mode on the Project Management Panel.

11. Configure the workpiece coordinate system (G54...G59) using the Workpiece CS command in the Setup tab on the Main Panel. Additionally, you can create and manage a local coordinate system using the Coordinate System Control Panel. See more.

12. Use the Run Program button to compute the operation toolpathes if you did not select the Auto Run option.

13. Manage the visibility of objects in the graphic window using the filters on the Visibility Control Toolbar. See more.

14. Use the Simulation Panel tools to configure the simulation process. See more.

15. Simulate the technological operations using the tools on the Simulation Panel. For extra control over the machine axes, utilize the Machine Control Panel on the Project Management Panel. Check the machining results against the reference model for residual material or overcuts using the Verify Compare option on the Project Management Panel. Each block in the NC Code Editor Panel will have status markers based on the simulation outcome. Analyze and correct errors by selecting the appropriate blocks of the NC program. The tool and machine nodes will be positioned according to the selected block.

16. When needed, convert the NC program to the new format, save it, and ensure that the project file is also saved.

Handling an existing NC program.

The process in this case is similar to the previous one, except for the following point:

Click here to expand..

5. Open the NC program file using the Add Existing command on the Explorer Panel. You can open multiple files if they belong to the same project (a single part manufacturing process on one machine). Each new file will appear in a new NC Code Editor Panel. You can also write new code in a blank NC Code Editor Panel. When multiple NC program files are loaded, the operation segmentation will occur in the order of the files in the Explorer Panel. To rearrange the files, drag them to the desired position with the left mouse button.

Operating with a CAM system project.

You can utilize NC Tuner to debug the NC program within a configured CAM system project environment.

Click here to expand..

Select the Open ENCY Project in New Tab command from the File Control Panel. Choose the desired file in the dialog box. If the CAM project had post-processing done earlier, the generated NC program file will be opened. Otherwise, the system creates a new blank NC Code Editior Panel. The Main Panel lists the technological operations as they were in the project. Additionally, the machine, part, and workpiece used in the project will be loaded if they were saved in the CAM system. See more.
Click the Explorer button to access the Explorer Panel. See more.
Upload the interpreter file that matches the NC system, if it was not initially loaded in the project.
Upload the post-processor file that matches the NC system, if it was not initially loaded in the project.
If the NC program was not previously generated, return to the CAM program and perform post-processing. Then, load the generated NC program into ENCY Tuner via the Explorer Panel using the Add Existing command. Post-processing in ENCY Tuner is possible only after the operations have been set up and calculated.
The Main Panel displays the list of technological operations that was generated in the CAM system. You can proceed directly to toolpath calculations. If the current list of operations does not meet your requirements, you can generate a new list using the Split command on the Project Management Panel. See more. The existing list will be updated according to ENCY Tuner's rules. Note the splitting options available in the dialog box that appears.

If you select Yes in the dialog window, all existing operations will be replaced by new operations identified from the NC program text. The project tools will be replaced by the new ones.
If you choose No in the dialog window, all existing operations will be retained. The NC program text will be unlinked from existing operations, analyzed and, if possible, re-linked to them. If linking to existing operations is not possible, new settings and operations will be created.

If the automatic splitting does not meet your needs, you can modify the operation segmentation using the context menu commands in the NC Code Editor Panel. See more

The following process is the same as that for Creating a new NC program.

Creating a new project using a CAM system setup file.

If you want to debug the NC program using a previously defined template from the CAM system, load the setup file with a .stms extension. This file contains a template with specific configurations, such as tools and fixtures, for machining similar parts.

Click here to expand..

Open the Create from Machine Setup File in a New Tab command. The new project will include the following definitions if they were previously established in the CAM system:

interpreter;
postprocessor;
fixture (along with its location);
project tool list;
machine;
setups and parts treated as groups of operations;
list of workpiece coordinate systems;
tool block types and tool positioning in the turret head.

This template allows you to either write a new NC program or debug an existing one. Further work proceeds in the same manner as when Creating a new NC program or Handling an existing NC program.

If you want to apply such a template to an existing ENCY Tuner project, select the Import Machine Setup command. In this case, the active project will incorporate the following elements from the selected setup file:

project tool list;
fixture (along with its location);
list of workpiece coordinate systems;
tool block types and tool positioning in the turret head.