Job

A job object contains all references and parameters needed to calculate a toolpath. After successful calculation, this object contains the resulting toolpath.

The job must be recalculated if a parameter changes or if a referenced object has changed.

Tool reference

The tool reference determines the radius correction, is used by the collision check and contains further parameters for the tool path calculation.

The screenshot shows a tool on a milling path. The contour of the tool lies exactly on the model geometry. — Radius compensation

A tool reference is essential in most cases, because without a tool, neither radius compensation nor a collision check can be carried out.

The tool referenced in send2cnc must match the tool actually used on the machine. Otherwise, the milling result may be distorted and there is a risk of collisions during milling.

It is therefore extremely important that all relevant tool parameters, especially the geometry definition, are correctly defined in the tool.

Job-specific tool parameters

These parameters define the tool and spindle settings for the current job.

Any number of job objects can reference the same tool, but the job-specific tool parameters only apply to the respective job. This allows the cutting data to be optimized and customized for each machining step.

Spindle Speed [spindleSpeed]

This parameter defines the spindle speed. This value is interpreted by the post-processor and must be given in revolutions per minute.

Cooling [cooling]

Defines the cooling mode for the machining. The value is interpreted by the post-processor used.

Spindle direction of rotation [spindleRot]

Determines the direction of rotation of the spindle (clockwise or counterclockwise).

Rapid feed mode [feedMode]

Controls the feed rate mode for rapid movements. The rapid feed can either be controlled by the CNC control (Rapid) or by an optional value entry (Userdefined) in the job.

Rapid feed rate [feedRapid]

Optional feed rate for positioning movements in unit/min. Only active when the rapid feed mode is set to "userdefined".

Feed rate [feed]

The feed rate for cutting movements in unit/min.

Feed ramp [feedRamp]

The feed rate for ramp-shaped plunging movements into the material in unit/min.

Drill feed [feedDrill]

The feed speed for vertical plunging movements into the material in unit/min.

Main

Milling strategy [strategy]

The milling strategy determines the basic calculation algorithm for the toolpath.

The screenshot shows the user interface for the 'Main' tab for setting the milling strategy and for setting the geometry references and the various geometry allowances. — Tab for the job settings

Roughing [strategy=0]

Clears the 3D model layer by layer from the blank.

This algorithm generates planar toolpaths for broaching the blank at each infeed level. The planes between the start and end planes are created and broached at the main infeed distance (Ap Main).

After each main infeed, the rest of the material is optionally removed layer by layer from bottom to top with a finer level gradation (Ap Micro). This strategy minimises the number of toolpaths and therefore milling time, and ensures that the model is quickly and thoroughly premachined during roughing.

Contour Slice [strategy=1]

The contour milling algorithm generates flat toolpaths around the 3D model, layer by layer.

With a small vertical infeed (Ap Main), this job type is also very suitable for finishing steep and vertical areas.

3x Smooth <BASIC> [strategy=2]

The 3x Smooth finishing algorithm covers all flat areas up to a certain slope with a horizontal infeed.

Spiral optimisation reduces the approach and departure movements to a minimum.

3x Carve[strategy=3]

From simple 2D engraving to 3D finishing and "3D V Bit Carving" on 3D surfaces. This strategy can be used universally for a wide range of applications.

The structures are machined in a spiral using three-dimensional toolpaths. The vertical infeed adapts to the model. If the depth of the structure exceeds the main vertical infeed, the level is cleared completely after each main vertical infeed before machining continues in the depth.

Drilling [strategy=4]

The "Drilling" strategy is a semi-automatic process for calculating drilling movements.

Geometry references

Geometry references determine the geometry of the object to be mashined. For a reference to be available to the job, it must be above the job in the project hierarchy.

Multiple selection is also allowed for each reference type. The following is a list of all geometry references:

Model Reference[sumModel]

Model references determine the shape of the object to be milled. The milling tool moves along the "hull" of these selected models.

Generally, the toolpaths are calculated in such a way that the tool does not penetrate the model hull. However, a negative offset can be set and the radius compensation of the tool can be deactivated. In such cases, the toolpath either lies directly on the model hull or even penetrates it.

Blank reference[sumblank]

The blank defines the area to be machined. Toolpaths are usually only generated within the blank.

An exception to this is approach paths and special settings in the job parameters, such as zone boundaries and offset options. If no blank is selected, a blank is emulated internally in the size of the selected model references and all areas are machined. However, a blank reference may be mandatory for some job strategies. A blank reference is only available to the job if the object is located above the job in the project hierarchy.

The screenshot shows toolpaths that run along a model contour. The toolpaths end at a support ridge. — Example of a fence as a boundary model reference

Boundary model reference [sumFence]<BASIC>

Defines areas that are excluded from machining.

Similar to model references, the toolpaths do not cross this area or only after the exceptions and rules already described in the model reference. The difference between a model reference and a boundary model reference lies in the contour machining: the contour of a boundary model is not machined. If the toolpath encounters a boundary model, it ends at this point, lifts off and continues machining in the next area to be machined.

With the help of boundary model references, areas within a machining area can be left out, such as holding tabs. A boundary model is only available to the job if the object is located above the job in the project hierarchy.

3D reference surface [sumSurface]<Pro>

Defines a 3D surface that the toolpaths can follow (required for the "3x Carve/3D Surface" mode).

Special references

Special references can also be used and are described in the general chapter for reference lists

Parameters

The settings for the selected strategy can be adjusted in the "Parameter" tab. This section varies greatly between the different strategies, since not all parameters are relevant or available for each strategy.

Parameters – Milling area

This section is used to define the milling area to be calculated and to make settings for the geometry references.

Vertical milling area

The following planes limit the vertical milling area and determine the positioning plane for the job.

The technical illustration shows the position of the various planes in relation to the zero point.

Positioning plane [planeSite]

The positioning plane defines the height of the plane relative to the workpiece origin. To avoid collisions, this plane must be higher than all geometry references.

The tool usually moves at rapid traverse to the various machining positions at the height of the positioning plane. Whether this plane is approached before the start positioning and after a tool change depends on the postprocessor.

Starting plane (top machining plane) [areaLimitTop][planeTop]

The starting plane determines the height of the plane at which machining begins, relative to the workpiece origin.

This plane limits the vertical milling range upwards. The milling paths are generated from this plane. An exception to this are plunge movements, which can also start above this plane.

End plane (lowest machining plane) [areaLimitFloor][planeFloor]

The end plane defines the height of the plane at which machining ends, relative to the workpiece origin.

This plane limits the vertical milling range at the bottom. The milling paths are generated up to this plane.

Zone limitation

In addition to the selected geometry references, the milling range can be restricted by zone settings.

Zone inside/outside

The zone boundary runs along the outermost silhouette of the model references. Optionally, the zone can be extended or reduced using an offset. Zone limitation can be very useful when using support holding tabs and can even reduce the number of geometry references required.

The illustration shows how the toolpaths are influenced by zone limitation. — Zone limitation
Inside zone | Outside zone | Both zones
Workpiece blank zone: activated

Zone Inside [areaIn][areaOffsetIn]

Toolpaths are created within the outermost model silhouette. The zone can be extended or reduced by specifying an offset.

Islands and holes in the geometry references are not affected and are machined.

Zone outside [areaOut][areaOffsetOut]

Toolpaths are created outside the outermost model silhouette. The zone can be extended or reduced by specifying an offset.

Zone blank[areaLimitStk]

Toolpaths are limited to the area of the blank.

This option is available for strategies where it is not common to limit the toolpath to the blank only.

The technical illustration shows a model contour offset by the allowance and a cutter that respects the allowance.

Geometry allowance <BASIC> [allowance...]

The allowance table allows you to specify a material allowance in the horizontal axis of the workpiece origin (XY) and the vertical axis (Z) for each geometry reference. Negative values are also possible.

Parameters – Properties

The parameters for the selected milling strategy are controlled in the job properties.

Among other things, the infeed, the approach and plunge movements, the plunging behavior and specific properties of the milling strategy are configured here. This area varies greatly between the different strategies.

Infeed

The illustration shows a side view and a top view. The toolpaths and the dimensions for Ae, Ap and Ap Micro are shown.

Axial Depth of Cut (Ap) [stepAp]

Starting from the starting plane (top machining level), the main infeed is made in the direction of the Z-axis until the end plane (bottom machining level) is reached.

Axial Microdepth of Cut (Ap Micro) <BASIC> [stepApMicro]

The material that cannot be reached by the main infeed is machined at the spacing of the intermediate steps.

The main infeed takes over the rough broaching work, while the intermediate steps clean the 3D contour with a finer gradation. The value is optional and must be smaller than the main infeed.

Radial Depth of Cut (ae) [stepAe]

Indicates the preferred horizontal distance between the milling paths.

Regardless of this value, the calculated tool path may also contain cuts with higher distances or cuts into solid material due to the geometry. The angle of contact (pressure angle) of the milling cutter can therefore be greater than would be expected from the specified value.

Broaching strategy[broach]

Defines the pattern of the stepover.

The illustration shows spiral milling paths. One spiraling in and one spiraling out. — "Outward spiral" and "inward spiral"
in the same direction.

Spiral inwards

The milling path starts at the edge of the area to be machined and ends in the middle.

Spiral outwards

The milling path starts in the center and ends at the edge of the area to be machined.

Carve mode[carveMode]<BASIC>

Determines the behavior in the contour area and has a major influence on milling time and quality.

Standard

The material to be milled is always removed up to the contour.

V Bit Optimization <BASIC>

The tool penetrates as deeply as possible into the areas to be machined without losing detail. This results in skeleton-like milling paths that reduce the tool paths to an absolute minimum while increasing the level of detail in the engraving.

This setting is optimized for engraving cutters, but can be used for any tool type.

3D Surface[surfProj]<Pro>

The vertical milling feed (Ap Main) adapts to the shape of the 3D reference surface selected in the geometry references.

This makes it possible to mill engravings on 3D surfaces and to machine residual material. The resulting blank from the previous job can often be used as the 3D reference surface (inherited blank).

Surface Start[surfProjTop]

Enter the offset to the 3D reference surface (default: 0). The tool paths start on this 3D plane and are advanced in three dimensions with Ap Main until the "surface depth" is reached. This parameter can be considered the 3D equivalent of the starting plane.

Surface Depth[surfProjDepth]

Enter the offset to the 3D reference surface (default: < 0). The toolpaths end on this 3D surface. This parameter can be considered the 3D equivalent of the end plane.

Plunge / side approach

In order to reach the actual starting point of the milling process, the program tries to avoid plunge movements if possible and instead prefers side approach movements. In a side approach, the tool is either positioned on an already machined area or laterally outside the blank and mills horizontally from there to the starting point of the actual milling operation.

If a side approach is not possible, plunge movements in the direction of the Z-axis are used in a priority order. The order of priority, from highest to lowest, is: spiral plunge, ramp plunge and finally vertical drill plunge.

The available plunge variants depend on the selected milling strategy, and the individual plunge options can be activated or deactivated as required.

The technical sketch shows the various plunge and approach options – how the tool plunges into the workpiece. — Plunge parameters and safety distance

Plunge angle α [plungeAngle]

Specifies the angle for spiral and ramp-shaped plunging movements.

Spiral plunge <BASIC> [plungeSpiral][plungeDia]

The tool plunges in a spiral from the blank surface to the machining level in the blank.

The dimensions of the spiral are determined by the diameter [plungeDia] and the plunge angle, while the height is calculated from the machining level, the blank surface and the safety distance in the Z-axis.

Ramp-shaped plunge <BASIC> [plungeRamp]

The tool plunges into the blank at an angle.

The start height of the ramp is calculated from the machining plane, the surface of the blank, and the safety clearance. In the XY direction, the path of the ramp runs along the toolpath immediately following the machining plane. If a longer path is required for the ramp than is available, the path repeats in a pendulum-like manner until the machining plane is reached.

Vertical drill plunge [plungeDrill]

The approach movement is vertical through the blank, using the drill feed.

The vertical plunge has the lowest priority and is only used if none of the other plunge variants are possible or if they are disabled.

Safety Gap [safetyGap]

The safety gap defines the minimum distance in all three axis directions (X, Y and Z) between the tool and the geometry references for rapid positioning movements.

In rapid traverse, the tool approaches the geometry up to the safety gap. Ramp-shaped plunge movements are extended up to this distance.

Tip:

A large value for the safety gap has a significant effect on the processing and calculation time and also increases the milling time due to longer plunge distances. The value should be selected so that safe milling is ensured, taking into account all tolerances and deviations, without being unnecessarily large.

Parameter – Optimization

The technical drawing shows a tool and a toolpath point. The toolpath point is slightly away from the model contour. The tool is aligned with the toolpath point and the cutting edge is in exact contact with the model contour.

3D radius compensation [radiusCorr]

Radius compensation takes the tool geometry into account when calculating the toolpaths and enables a collision check to be carried out.

With radius compensation activated, the collision check is applied and the tool path is calculated so that the tool geometry does not enter the model contour, or only according to the tolerance and the geometric oversize.

If the radius correction is not activated, the tool paths are created directly on the model geometry. In this situation, the (unknown) tool used would penetrate the model geometry up to half of its diameter or up to the tool axis. A collision check is not possible in this case.

Preferred feed direction [feedDir]

The preferred feed direction determines the direction of tool movement in relation to the model contour.

It should be chosen taking into account various factors, such as the material, machine, cutting tool and its tool life, the desired surface quality, accuracy and infeed strategy. A detailed description of all influencing factors is beyond the scope of this manual. For some applications, such as a full cut, this parameter is not important.

As already mentioned in the heading, this parameter is the preferred running direction. This means that the program tries to use the running direction set here. However, depending on the geometry and other job parameters, this may change several times in the resulting toolpaths.

This technical illustration shows the difference between climb milling and up-cut milling. In climb milling, the tool moves like a wheel on the floor. In up-cut milling, it moves in the opposite direction.

Climb milling [feedDir=0]

In climb milling, the tool advances in the feed direction.

The cutting edges of the tool make contact with the material abruptly, with the chip thickness being at its maximum at the start and decreasing steadily until the cutting edges exit. In practice, climb milling is usually selected for CNC milling these days, provided that the machine's guide play allows it. This method generally causes less vibration and less tool wear and usually produces a better surface quality on the final workpiece.

Conventional [feedDir=1]

In conventional milling, the tool moves in the opposite direction to its direction of rotation.

The chip forms from zero as the cutting edge enters, and builds up to its maximum thickness by the time the cutting edge exits. Conventional can be advantageous when machining harder materials or when roughing, as it allows for a higher metal removal rate and improves chip formation. However, conventional milling can lead to increased tool wear and stronger vibrations, which can have a negative effect on the surface quality and the tool life.

Pause [pause]

Inserts a pause command into the NC program.

The position at which the pause is actually set depends on the postprocessor. Usually, this occurs after the execution of the job.

No NC output

If this parameter is activated, the job is not forwarded to the postprocessor.

This can be useful, for example, if an object that has already been milled is to be recreated as a virtual blank for further processing.

Collision Check[collisionCheck]

When the check box is activated, a collision check is carried out for the calculated tool path.
Attention: A deactivated collision check can pose a risk to the machine and safety!

For more information, refer to the sub-chapter "Collision Check".

Path Optimization [optimize]

Selecting a path optimization mode improves the calculated milling path.

No path optimization [optimize=0]

The calculated rough path is not optimized.

The generated path offers the highest possible precision, but results in very fine stair-step movements. This mode can be useful if the control of the CNC machine is to smooth the path.

Standard [optimize=1]

Staircase-shaped movements are reduced by smoothing the calculated raw path. A low tolerance ensures that the details of the model are largely retained.

This option ensures an optimal balance between precision and machine performance.

Smooth [optimize=2]

The calculated toolpath is smoothed and rounded generously. This results in very gentle tool movements that conserve material and enable the use of high feed rates.

However, since the tolerance is higher here, the tool path may deviate further from the original geometry, which can result in the impairment of the smallest details.

Parameters - Drilling

The "Drilling" strategy is a semi-automatic process for calculating drilling movements.

The screenshot shows the user interface for setting the drilling parameters.

Drilling positions can either be entered manually in a list or selected directly on the 3D model using various selection tools and transferred to the list. Alternatively, it is possible to take over the drilling positions from another job.

Note

As long as the job dialog is open, a preview of the drilling positions is displayed in the render window. This preview shows lines that represent the drilling axes to provide visual orientation about the planned drill holes.

Precision

The values of the point list are transferred to the voxel grid during calculation. This means that the coordinates of the points in the exported NC file may differ from the entered coordinates of the point list. The accuracy of the drilling positions is determined by the project resolution.

Source

Specifies the source from which the drilling positions are obtained.

Point list

The point list contains the XY coordinates of the drilling positions, starting from the workpiece origin. Each line of the list defines a drilling position and consists of two values (position X and Y).

As soon as the input focus leaves the text field or the F5 key is pressed, the list is automatically formatted, cleaned and checked for errors. The drill axes displayed in the render window are also updated.

Set Drill Position

This function allows you to select drill positions directly in the render window with a single click. To exit the selection mode, right-click in the render window and open the context menu or press the Esc key. The points set are added to the point list.

Set and center drilling position

This function allows you to set drilling positions in the center of automatically recognized shapes in the render window. You can end the selection mode by right-clicking in the render window and opening the context menu or by pressing the "Esc" key.

To successfully select a shape, left-click the side face of the desired shape (e.g., the vertical inside of a hole). The shape must not intersect the model boundary.

Delete Points List

This function removes all points entered in the text field.

Reference

The drill positions are taken from the selected reference.

If the drilling positions of the reference change, they will be updated automatically when the job is recalculated. Any job of the type "Drilling" is allowed as a reference and must be located above the job in the project hierarchy.

Z Setting

This section is used to configure the automatic detection of the drill start points and the drill depths.

Start [drillModeTop][drillTop]

Defines the mode for determining the start points for drilling.

Mode	Remarks
Top plane	All drill holes start on the same plane. The value entered determines the height of the plane starting from the workpiece origin.
Geometry	The starting point in direction Z of all drill holes is determined automatically. The surface of the geometry references, the tool and the radius compensation are taken into account. An optional offset shifts the starting points by the specified value.

Depth [drillModeFloor][drillFloor]

Defines the mode for calculating the drilling depths.

Mode	Remarks
Floor-Plane	All drillings end on the same plane. The value entered determines the height of the plane based on the workpiece origin.
Drilling depth	All holes have the same depth. The depth is calculated from the starting point and the specified value. A negative value must be specified.

Miscellaneous parameters

This section contains additional settings for drilling.

Vertical infeed [stepAp]

After the tool reaches the specified vertical infeed, it performs a retracting movement to break the chip. It prevents chip congestion by lifting out of the hole and repositioning itself in the hole. This process is repeated until the drilling depth is reached.

Retraction

Defines the feed mode with which the tool lifts out of the hole after each infeed and repositions itself in the hole for multiple infeeds.

Resulting blank

After the job has been successfully calculated, a resulting workpiece is added to the job as a sub-element.

This can be selected and displayed in the project tree. This way, the end result can be visually checked immediately.

It can also be used as a follow-on blank for the next job. This way, a chain of inheritable parts can be created so that each job takes into account the result of the previous job.

The resulting blank is calculated from the referenced blank, the tool and the toolpaths. It is automatically deleted as soon as the job is recalculated or reset.

Collision Check [collision]

During the calculation of a job, a collision between the tool and the stock can be detected. In such a case, the system creates an object named "*_COLLISION" as a sub-item for the job. This object indicates the contact points of the non-cutting tool geometry with the blank and is automatically shown together with the resulting blank. If the job is recalculated or reset, the collision object is automatically deleted.

For a collision check to be performed, the following conditions must be met:

The collision check must be enabled in the job.
A tool must be referenced in the job.
A stock must be referenced in the job.

A collision is detected if the tool makes contact with the blank during a rapid movement or if the non-cutting geometry of the tool makes contact with the blank.