- Operating Principle: Step-over Turning Method
- Geometry Definition and Automated Calculations
- Tool Definition and Preparation
- Cutting Strategy and Technological Parameters
- Multi-start Worms and the “Q” Parameter (Mazak Specifics)
- Handling Workpieces Without Undercuts (Entry/Exit Motion)
- Finishing Strategy and Corrections
- Coordinate Systems and Safety (EIA/ISO vs. Mazatrol)
- Project Management and NC Code Generation
Cutting Strategy and Technological Parameters
This section explains how EvoSpline controls tool movement and how to optimize settings to avoid machine synchronization errors.
The MAX Button – RPM Automation
Turning a worm is essentially a threading process with a very large lead. This requires the machine to maintain massive linear feed rates to stay synchronized with the spindle rotation.
The Problem: If the RPM is set too high for a large lead, the machine will fail to keep up (exceeding its Max synchro feed), resulting in an error or a mid-process halt.
The Solution: Clicking the MAX button allows the software to automatically calculate the highest safe RPM for your specific setup based on machine limits. This ensures 100% productivity without the risk of a synchronization crash
The „Wedge” Strategy – How the Tool Actually Cuts
It is crucial to understand that EvoSpline does not machine the worm in traditional flat layers (e.g., machining the full width at one depth, then moving deeper).
Instead, the strategy generates progressively larger „wedges” or „cones.” From the very first pass, the tool machines the target profile shape, but at a smaller scale. With each subsequent pass, this shape is „expanded” both in width and depth until the final dimension is reached (minus the finishing allowance and tooth thickness correction).
Why is this better?
- The tool load remains uniform.
- The flank profile is shaped progressively, which improves process stability.
Parameter: No. of Roughing Cuts
This field is key to controlling the process, but it is often misunderstood:
It is NOT the total number of tool passes: Entering „5” does not mean the tool will only make 5 passes in total
Cutting Width: This parameter determines the horizontal density of the tool paths. A higher number results in a smaller chip width (Width cut), which reduces cutting forces and improves surface finish.
What determines the total number of passes? The total number of movements in the NC code is a product of the „No. of roughing cuts” combined with the defined Roughing depth. The software automatically divides the total stock to maintain optimal cutting conditions.
You can set this number manually or let the program calculate it while monitoring the resulting Width cut value.