Machine Menu

Machine Menu
	Chapter 5. Mill

Figure 5.52. Machine Menu

Abstract

The main milling menu in Mill and is used to create and send toolpaths to the machinery. The machining process utilizes the tools defined in the Setup menu and allows you to define and create toolpaths (Face Mill, Slot, Profile, Area Clear and Drill Cycles). Toolpaths can then be sent directly to the machine, or saved as a file.

Machine → Machine

Start the Machine wizard that will proceed with a step-by-step guide to complete your job. The list below describes the order of the Machine Wizard:

The wizard starts with the billet setup dialog box, which enables you to define the billet’s material, dimensions and location.
Choose groups and surfaces with which you want to create toolpaths.
The tool library dialog box is then displayed for selecting the tools to use in your job.
The technology dialog box creates a toolpath with tool compensation.
Select the required toolpath strategy – Profile, Area Clear, Slot, Face or Drill Cycles.
The final stage, where applicable, is creating a reference to surfaces.

Figure 5.53. Example Machine Wizard Screen

While working through the Wizard you can edit or add parameters in any of the four tabs: Tool, Technology, Strategy and Surface. In addition to the tabs placed at the top of the wizard screen, there is a row of six buttons that exist in all tab modes:

	Goes back to the previous tab.
	Starts the calculation of the inserted parameters.
	Cancels the Machine Wizard.
	The command is added to the script but not executed.
	Will start the machine wizard process for the next operation.
	Opens the help menu.

Tool .

Figure 5.54. Tool

Tools define the tools to be used in the machining process. An engraving tool may have a conical cross section with a nose tip radius and a corner radius. Many kinds of shaped or tapered engraving tools can be defined including flat, ball, and tapered tools.

Technology . Creates a toolpath with tool compensation.

Figure 5.55. Technology

Depth of cut (Z)	Final depth you want to reach in the material with respect to the Z Top value.
Z Increment (I)	Input the increment by which the milling should occur on the Z-axis.
Z Retract(R)	Sets the safe retract plane above the material and clamps or other objects so that the cutter moves about freely. This value is absolute.
Z Top (T)	Sets the local zero plane (the level at which the material surface top plane was set). Usually Z Top is set at zero.
Increment by Group	Executed over groups according to the value in the window; therefore the Z level is uniform. This method is time-consuming.
Increment by Chain	Applied on chains according to the value in the window. The cutting tool finishes a chain and then passes to the next chain. This method is more efficient than the By Group method because less machine time is needed.
XY Feedrate	Enter the machine's feed rate (units/min) for the horizontal (XY) plane.
Z Feedrate	Enter the machine's feed rate (units/min) for the vertical (Z) axis. This defines the speed of entry into material.
Spindle speed	The cutting tool's rotation speed is rated in revolutions per minute (RPM).
Spindle Mode	Select the cutting tool's rotation direction: `CCLW` – Counter-clockwise. `CCW` – Clockwise. `OFF` – The direction of rotation is determined manually on the cutting machine.
Coolant	Select the applied cooling method: `Flood` – for a steady flow of cooling solution. `Mist` – for a spraying flow of cooling solution. `Off` – for none.
Plunge Angle	Entrance angle of the tool to the material.
Tool Compensation	`Off` – Create toolpaths without compensation, only with the tool’s center geometry. `On` – Control the G-code output so that G41/G42 will be output together with the tool center geometry.
Optional stop	Machine will pause each time the machining process completes a single marked group and waits for the operator to resume command on the machine panel.
Machine Groups Separately	Machine each marked group on its own. This feature is useful for groups created by the GraphiCAD stack function (serial numbers, nameplates, etc.).
Optimize Jumps	Optimize the rapid motions. The system default is off in order to enable the system to machine from inside out. If it is necessary to minimize the jumps, you may turn the switch on, so that the shortest way is calculated.
Cut in climb mode	Unless checked, cutting is done in normal mode.

Strategy . There are five toolpath strategies to select from – Profile, Area Clear, Slot, Drill or Face.

Profile .

Figure 5.56. Strategy - Profile

Skeleton	Tapered tool will travel to the maximum allowed depth in cases of close proximity entities.
Ramps only	Only active if Skeleton is checked. By-passes the profile milling process of Skeleton. Thereby saving time if the tapered tool has already fulfilled its milling operation.

Area Clean .

Figure 5.57. Strategy - Area Clean

Figure 5.58. Parallel

Select Hatch Angle to clear the area in parallel sweeps, and enter the angle (in degrees) at which the area clear (X-hatch) operation will take place. A value of 0° defines the horizontal X-hatch lines; a value of 90° defines the vertical hatch lines. Spiral/Parallel is calculated for all the marked groups as if the groups are one object.

Optimized – for a smart bi-directional move, with minimum movement of the tool in the Z- level.
Uni-Directional – for machining in only one direction.
Bi-Directional – For machining in two directions.
Laser mode – as Optimized, without connecting the moves in order to avoid double burn by the laser.

Figure 5.59. Laser mode | Bi-Directional | Uni-Directional | Optimized

Profile pass

Select one of the following mode:

Every Z Level – default, generates a profile path after the area clean operation path for every increment.
Final Pass Only – generates a profile path after the area clean operation for only the last increment.
No Profile – no profile path after area clean operation.

Figure 5.60. Spiral

Clear the area in a spiral pattern.

Smart clear

When side step value is set to more than 50% of the tool’s diameter size. When selected, the program creates a supplementary toolpath - Smart clear to cover the unmachined areas remaining due to the large side step selected. Use of this option for less than 50% side step will not create the Smart clear toolpath. This is a powerful tool and vital for creating pockets and other area cleaning assignments in a fast and accurate manner.

Outside in

Change the usual milling direction of inside out.

Profile / Area Clean Common .

Side Step

	Note
	Area Clean only!

Defines the distance (in units) between two adjacent tool moves.

Additional Offset Extra stock in addition to the original geometry stock, necessary for finishing.

Mold Sets the procedure to create a toolpath on the contour projected at the Z depth value. This option is effective when a tapered tool is used.

Sharp Corners Corners consist of straight lines unless there is an intersection between two entities. In that case, the corners will be chamfered. Enter the desired offset in the adjacent text box.

Mark Unmachined area

There are often unmachined areas after cutting because the selected tool was too large to clean the entire area. This option creates a new group consisting of the unmachined area. Select a smaller tool, mark the unmachined group, and activate the Profile (or Area Clear) option again.


Machined and unmachined area.	Unmachined area.

Shaped Walls

Figure 5.61. Tool

By dragging on the circular control points you can manually design the shape of a wall.

	Note
	The shape of the wall has to be compatible with the tool you are using.

You are able to save and load previously created shaped wall. Resetting returns the shaped wall back into its original position.

	Paste a shape from the system’s clipboard.
	Figure 5.62. Shaped Wall, Slope Insert the desired angle in the text box.
	Figure 5.63. Shaped Wall, Ellipse Insert the desired ellipse points in the text boxes.
	Determines that the wall will adopt the shape of the tool.

Entry Mode

Select one of the following three entry modes:

None – vertical entry.
Linear – perpendicular entry.
Circular – radial entry.

Helical – enables a plunge into the material in a down spiraling motion.

	Note
	Area Clean only!

Entry Value Defines the distance between the middle of the first entity chosen and the first tool entry location. Circular entry mode - the distance is the radius of the half circle. If the value is larger than the geometry width, the Entry Value is set automatically to optimal value – the entry point will not move to another location.

Pitch

	Note
	Area Clean only!

Defines the down step on every complete circle. The helical motion is similar to the action of inserting a screw, with a fixed pitch.

Machining side Sets the offset side with respect to the marked groups. This value is calculated for all the marked groups as if the groups are one object. Select Internal to apply the offset on the inner side of the object, External to apply the offset on the outer side of the object, or Manual Pick to apply the offset manually on the screen. If the marked geometry consists of open contours, Left and Right options replace the Internal and External options.

Accurate/ Fast Controls the calculation speed – as opposed to the calculation accuracy. The default value assures very high accuracy. However, in some cases, such as very small objects, higher accuracy is required. A good practice is to machine the rough toolpath with low accuracy (fast), in order to reduce processing time.

Slot .

Figure 5.64. Strategy - Slot

Toolpath that cuts directly on a contour.

Cut One Pass	Slot machines the geometry once only.
Cut to End and Back (Bi-Directional)	Slot the geometry from start-to-end of each contour and then repeat from end-to-start, thereby ensuring high quality.

Drill .

Figure 5.65. Strategy - Drilling cycles

Create drilling toolpath. The entry windows for Retraction and Dwell parameters will appear according to the parameters that were requested for the specific drill method.

End Entities	Drilling the end edges of the entity.
Arc Centers	Drills the center of each arc that belongs to the marked group.
Chain Starts	Drill a preparation hole for the milling tools after using Area Clean. The location of the hole depends on the Area Clean method (Spiral, Parallel).

Figure 5.66. End Entities | Arc Center | Chain Starts

Table 5.1. Drill method

Method	Drilling (-Z direction)	Operation at the bottom of the hole	Retraction (+Z direction)
High-speed peck drill	Intermittent feed (forward and backwards drilling).		Rapid traverse rate (the rate of fast traverse movement).
Left-hand tapping	Continuous feed (with no stopping)	Spindle CW (rotation clockwise)	Continuous feed
Fine boring	Continuous feed	Oriented spindle stop^[a] + Dwell	Rapid traverse rate
Spot drill	Continuous feed		Rapid traverse rate
Counter boring	Continuous feed	Dwell	Rapid traverse rate
Peck drill	Intermittent feed		Rapid traverse rate
Tapping	Continuous feed	Spindle CCW (rotation counterclockwise)	Continuous feed
Boring	Continuous feed		Continuous feed
Boring with stop	Continuous feed	Spindle stop	Rapid traverse rate
Back boring ^[b]	Continuous feed	Spindle stop	Rapid traverse rate
Boring with dwell	Continuous feed	Dwell + Spindle stop	Rapid traverse rate
Feed and dwell boring	Continuous feed	Dwell	Continuous feed
Rigid tapping	Continuous feed		Continuous feed
^[a]Because a spindle-oriented stop is performed at the bottom of the hole, and the spindle retracts after shifting in the direction opposite the cutter direction, high precision and efficient boring is performed without scratching the machined part surface. ^[b]In this method, after the tool is positioned along the X and Y-axes, the spindle stops at the orientation position. The spindle is then shifted in the direction opposite the tool and is positioned at the bottom of the hole at the rapid traverse rate. At this position, the tool returns only for the shift value, and the spindle rotates clockwise.

All the drill cycles conform to the ISO standard as defined by Fanuc™ Ltd.

Retraction	Sets the retraction distance for the cutting tool moves. Use this option to simplify chip disposal and perform efficient machining. Retraction is performed at the rapid traverse rate.
Dwell	Enter the delay time at the bottom of the hole (in seconds).

Face .

Figure 5.67. Strategy - Face milling

Create a cleaner and smoother area on the billet.

Parallel .

Figure 5.68. Parallel

Please refer to Area Clean for information.

Parallel .

Figure 5.69. Radial

Select Round or Square to get a snail like toolpath.

Width/ Height	Radial dimensions.
Snail Center point X/ Y	The X/ Y coordinate of the radial center.

Please refer to Area Clean for information.

Parallel/ Radial Common .

Side Step	Please refer to Side Step.
Margin	Adds an offset to the billet size.

Surface .

Figure 5.70. Surface

Select the desired reference to surfaces.

Ignore - does not refer to the surfaces in the job, if any.
Rough - leaves a rough surface finish (fast machining). The machine movement is with straight Z levels, and no jumps.
Equal Z - engraves between the border of a protruding surface and the border of a billet with minimal jumps.
Finish - leaves a fine surface finish. The machine movement follows the surface shape.
5 Axis - this option creates a 5-axis toolpath. The toolpath contains also the i,j,k normal values at the tool tip. These values are available when posting the file to a 5-axis machine.

It is preferable to start with the Rough option while giving some extra offset for the tool and then continuing with the Finish option until the required height is achieved.

Machine from Z

Defines the Z level in which the machine starts to engrave. This is a top level limitation as well. The default value is the billet top. For surface milling, verify that this value is above the marked surfaces. Otherwise only parts of the intended toolpath may be visible and active.

Surface Offset

Extra stock in addition to the original geometry stock.

Surface Step

Defines a grid sampling rate on the surface that represents the tool movement. Smaller values create a denser grid that results in a better surface quality; this however, also increases the calculation period.

Model Accuracy

	Note
	Applicable for Equal Z only.

Grid accuracy for calculating the border of a protruding surface and the border of a billet.

Gouge Check

If marked, the toolpath is calculated with the compensation of the tool’s shape. If not marked, all the toolpath calculations are with respect to the tool’s tip. The default value for Gouge Check may be set in the system options.

Figure 5.71. Gouge Check marked | Gouge Check unmarked

Machine → Set Machine Zero

Change the coordinate system origin location. Use the mouse to move the cursor to the desired location and press the left button to set the new origin (for details on precision clicking, see Clicking Around with Cursors in the introduction chapter). The coordinate system can be moved in three dimensions, and the new location will serve as the new machine zero for toolpath calculations.

Machine → Output to Machine

In order to machine the tool path created in the Machine operation, the toolpath must be post-processed in the code required to drive the machine. Any group on the layout may be marked to be sent to the machine and cut. The communication may be implemented directly or by file transfer. The G-Code parameters are set in the Create Machine Program dialog box.

Figure 5.72. Create Machine Program, Machine Tab Dialogue

Machine This list presents the post processor files (*.PPC) that are located in the post directory at the time of starting the program. Select one of them to be either the active post processor or for editing.

Edit

Switch to the edit window to display or change the selected post processor file. Before changing your post file, read the appendix about handling the post processor.

	Note
	Back-up your files prior to making any changes.

Direct to machine Sends the processed file directly to the Windows default spooling device.

Axis Control

3 Axis	Translates the final CNC code to a 3-axis machine. 3 Axis is the default option for translating.
4 Axis Land + R	Translates the final CNC code to a 4-axis machine to engrave the geometries on a cylinder and maintain a constant angle. Enter the cylinder radius in the box.
4 Axis Width + R	Translates the final CNC code to a 4-axis machine to engrave the geometries on a cylinder and control the width of geometries (cutting roller dies). Enter the cylinder radius in the box.
5 Axis (Normal to Surface)	Translates the final CNC code to a 5-axis machine to engrave the geometries on a cylinder or sphere. Enter the cylinder or sphere radius in the box.
Use Machine Optimization	The Use Machine Optimization option was made in order to solve the following problem. In the picture below, the grid represents the machine accuracy. The Red line is the tool path that was made in Mill module and with Mill accuracy (which is bigger, then the machine has). The Green line is the real tool path on the machine. As you can see because Cimagraphi accuracy is bigger then the machine accuracy the tool paths are not equal. In order to solve this problem we added two parameters in Cimagraphi post processors that define the machine accuracy in three coordinates (`DEFXACCURACY`, `DEFYACCURACY`, `DEFZACCURACY`). This parameters combined with the activation of the Use Machine Optimization will make the two tool paths be equal. Figure 5.73. Use Machine Optimization

Output File Select an existing or enter a new *.CNC file in order to save the G-Code produced.

Figure 5.74. Create Machine Program, Repetition Tab Dialogue

Cartesian

If geometry is to be produced several times, it is possible to form a matrix. Select this option to create an XY matrix. The parameters of the repetitions matrix are defined by the number of rows (Repeats X) and columns (Repeats Y) to be produced and the Distance between each sequential job origin along the X and Y-axis. The default values are one row and one column (a single job).

Polar

To create a polar matrix for the option of repetitions. The entry windows below changes, enabling you to define: the repeats radius number (Repeats R), the matrix angle (Repeats A), and the distance from the center (Radial step) and the Delta Angle .

Complete part

Finish the work on a complete part before going on to the next repetition.

Parts to Produce

First Part Only	Produce only the first part from the matrix. The first part is the original part you selected. Use this option combined with the next option to decide whether or not to continue with the rest of the matrix.
All Parts Except First	Produce all the parts in the matrix except the first one.
All Parts	Select this option to produce the entire matrix.

Figure 5.75. Create Machine Program, Processor Tab Dialogue

Indexes

Select one or all of the indexes to be sent to the post processor.

Tools

Select one or all of the tools to be sent to the post processor.

Produce Tool Table

Print a table of all the defined tools at the G-Code file.

Load 1st tool at EOJ

Load the first tool at the end of the job in preparation for the next job.

Pause at Tool Change

The machine pauses after each tool change and waits for user interaction.

Subprograms for

Index Change	Create sub-programs in the G-Code whenever there is an Index Change.
Tool Change	Create sub-programs in the G-Code whenever there is a Tool Change.
Repetitions	Create sub-programs in the G-Code when you define Repetitions in your job.
Z Increment	Create sub-programs in the G-Code whenever you define Z Increment in the Machine options.

Position At

Select Start of Program for locating the sub-programs at the beginning of the CNC file. Select End of Program for locating the sub-programs at the end of the CNC file.

No Sub-programs

Create G-Code without any sub-programs.

Save as Default

Save these settings as default options for later use.

Figure 5.76. Create Machine Program, Edit Tab Dialogue

Saves the file that is presented on the screen (CNC or PCC files).

Opens the Print dialog box and prints the displayed text to the selected printer. This option uses Windows spooling capabilities and data transfer protocols. For more details regarding communication and printer devices, see the Windows On-line Help.

Undoes the last editing change.

Removes the selected text from the document and places it on the clipboard.

Copies the selected text into the clipboard.

Inserts the contents of the clipboard at the insertion point, replacing any selection.

Finds the specified text or the specified formatting.

Finds the specified text or the specified formatting and replaces it.

Sends CNC code to a file or to the machine. Press Process or CR.

	Note
	When processing, the button acts as an Abort button!

Exits without making changes. Press Close or Esc.

	Note
	For direct communications, add the Generic/Text Only printer to the list of printers and select this printer as the default. Consult the Widows printer manager for further information regarding printer installation.

Machine → Order Toolpaths

Often it is necessary to re-organize the toolpath sequence before sending toolpaths to the machine. Cimagraphi provides several ways to order the toolpaths. Selecting this menu item will display the Order Toolpath dialog box.

Figure 5.77. Order Toolpaths Dialogue

By Tool	Re-orders all toolpaths according to the tool position in the tool holder. This means all toolpaths using tool #1 will be at the top of the list followed by tool #2, etc. Internally for each tool, the order is as follows: smart clear toolpath lead, area-clean (Face, Spiral, Hatch), profiles, Skeletons, Slots and Drilling cycles.
By Index	All toolpaths are grouped first by index and then ordered internally as in by tool.
By Script	Re-orders the toolpath by the order of the script. To order the script, select a script command and drag it to a new location within the script list.

	Note
	Toolpaths may be re-ordered manually from the Group Manager. To change a toolpath position within the Group Manager list, use the Move Up/Move Down pop up menu items or drag them using the mouse.

Machine → Set Tabs

In order to leave the part attached to the billet, little jumps in the toolpath are created - Tabs.

Figure 5.78. Tab Settings Dialogue

Width	The width of the jump (see diagram).
Height	The height of the jump (see diagram).
Slope	the slope angle in degrees of the jump (see diagram).
Tab Spacing	The distance between tabs. Every X mm/inch.
Automatic / Manual	If the Automatic is checked, the tab spacing and position is fixed automatically. If Manual is checked, after you press OK, you left click on the toolpath in the place you want the tab to appear, if there is enough place for the tab it will appear there.

	Note
	In Manual mode, Tabs will appear only if there is enough space and always in the middle of an entity.