Alexsys V4 Mill Operator Manual

Overview

 ALEXSYS is a programming system for CNC machining centers. That combines features of CAD / CAM systems with typical features of conversational programming.

It is not necessary to be experienced with CAD/CAM systems to use this software.

Alexsys Features

This features below are in every Alexsys package.

• Import from DXF/DWG
• Generate GCode
• CAD Editor
• Toolpath Simulation
• G-Code Customization
• Thread Tables
• 3D Stock Preview
• Integrated calculator
• Advanced profile selection
• Timeline
• Manual G-Code Input
• Stock Materials

Part Origin(Part Zero)

The reference point or part origin is where you zero the part offset on the machine. New setups in Alexsys by default have the part zero set in the middle of the stock.  Sometimes, it makes it easier to get an accurate touch off if you move the reference point to a corner or edge of the stock.

To alter this, adjust the reference coordinates to match your setup. Below are compare and contrast shots to show how the reference point will move.

Example of Default settings, part 0 set to center of stock/part

Here is an example with part 0 moved to the corner. 

Face Milling

Safe Z : It's the z coordinate where the tool is safe , where it can't collide with anything ( fixture , stock , ..)

Reference Z Plane : Is the reference z coordinate. Usually it's the zero part Z0

Parallel strategy ( traditional ) :

Further reference Z plane detail from the software author:

The reference Z plane is the final surface plane after facing is complete.
The material to remove, is the raw material to remove from the reference plane in the Z+ direction.
Thus the software can calculate the starting level and how many passes are required.
If you are cutting other profiles as part of the same Alexsys project, you will need to adjust the start Z point for each of those profiles.

Direction Auto : The direction is calculated automatically

Direction Horizontal : The direction is parallel to X axis

Direction Vertical : The direction is parallel to Y axis

Child operations available

1) Roughing

It process multiple passes in z direction to remove all the material to remove.

The passes depth is determined by the tool cutting data parameter. ( Max Cut Height )

Material to remove : Measured from Reference Z Plane to Z+ direction

Roughing Mode : It's the selected strategy

2) Finishing

It perform the last finish pass on the part face.

Finishing allowance : It's the material left by the roughing operation

3) Chamfering

Contour and Pocket operations

Under the Mill menu, you can find Contour and Pocket operations.

This 2 machining operations are identical except the fact , by default ,  contour will work the outer area of selected profiles, and pocket will work the inner area of selected profiles.

Switch profile side

Is possible switch the side of selected geometry.

You can both click on the double sided arrow in geometry list box or click the yellow arrow in viewpoint . When you hover the yellow arrow with mouse cursor , the arrow will turn red. Click on it to change working side.

The highlighted area in viewpoint , will be the area machined away by the operation.

Open Profiles

Contour and Pocket operations need a closed profile to work with.

If you select an open profile instead, Alexsys will try to close it with the outer stock profile.

See image.

Also in this case you can switch working side .

Z Levels

Safe Z : is the Z Plane where the tool approach in rapid movement

Start Z : Is the z plane where the tool start remove material

Depth : Is the thickness of material to be removed , measured from Start Z

By default these values are applied to all associated geometries.

But if you enable the " DEFINE Z LEVELS FOR GEOMETRY" , these value are applied only to current geometry. The current geometry is highlighted with red strokes in viewpoint and active in geometry list box

Groove Width

With a 0 value in WIDTH property , the region area is filled .Like this

But if i set a value in WIDTH the working area is created by offseting the source profile , like this.

This property is set just to the selected profile in geometry list box.

Overhang

Overhang feature is useful to create the side slots with this tool.

You need to enable [Is Overhang Active] and set the [Slot Height]

The bottom part of the slot is determined by the [Start Z] and [Depth] values. The Slot height is measured from the bottom part to Z+ direction.

By default , the outer overhang area is defined by the stock outer contour. 

Roughing plunge points

To force plunge point position for roughing operation, enable "Select Plunge Point" to pick to position with mouse.

Use [Clear Points Selection] to remove all defined plunge points.

Finishing Start Points

Is also possible define finishing start points. Use [Define starting points] under finishing operation.

Use [Clear Points Selection] to remove all defined plunge points.

Keep Tool Down

By default, after every pass in Z direction, the tool move to [Safe Z] level . The reason is to keep the maximum safety in toolpath creation.

But if you see there is no issue with stock collision, you can enable [Keep Tool Down] . In this way the tool goes directly to next z level , without moving to [Safe Z] after every pass. 

You have 2 different [Keep Tool Down] options, one under roughing operation and one under finishing operation. So you can have active in one operation and disabled in the other.

Finishing Offset

Is possible apply a negative or positive offset value to profile. With this you can remove more or less material from stock with finishing tool.

Override Geometries

In this image, only a square is defined in geometry selection box. The stock profile is defined by the stock setup. The toolpath is calculated in order to remove all the material from stock until it reach the defined profile.

Is possible override stock profile by :

1. Adding a new entity to geometry selection, in this case a circle
2. Setting it as [Stock Profile] from the dropdown menu.

With the new stock profile defined , the toolpath in calculated in order to remove just the material from custom stock profile.

Trim By Stock

Let's say this is your current stock model.

Then you need to machine a squared shape . By default this is the generated toolpath. You clearly notice the tool is working on already machined area. The toolpath is not optimal.

You can enable [Trim toolpath by current stock] .

The toolpath engine will calculate the stock model resulting from previous operations, and will use that model to skip the already machined area.

This will be the optimized toolpath. Now the tool works only where there are material to remove.

The [Trim By Current Stock] feature is computationally expensive.

Where applicable, use the override geometries method, which is more light to process.

Engraving

With ENGRAVING machining operation is possible to engrave text and geometries.

For text is available :

• Single Line font
• True Type font type , with any font family installed on PC.

You can define text on circular or linear pattern, mirrored around X or Y axis and you can apply many alignment options.

And of course all the selected geometry can be engraved.

Cut Operation

This is the machining you need to use when you want cut 2D Profile from material sheet.

Just select the geometries of the profile you want to cut.

Select the relative position of the tool :

• Internal
• Central
• External

Holding tabs

Holding tabs are needed in order to keep your cut part stable after the machining.

In this way the machine or tool are not damaged.

You need to manually remove the cut part from sheet

.

Check the property ADD HOLDING TABS.

To create this holding tabs, the tool need to raise in some points. 

You have to define the thickness and length of this holding tabs.

To define the position you can proceed manually or use the automatic method.

Automatic Mode

With automatic method, you need to define how many holding tabs you want to add.

The positions are calculated automatically.

Manual Mode

If you want to set the holding tabs in precise point, you need to select [Manual Mode].

Then click on [Pick Point], and click with mouse in desired points.

Thread Milling

Common parameters

Select Tool : You need to choose a thread mill tool. In case of internal thread , is necessary a tool diameter a bit smaller than predrill diameter.

Select Thread Category : Choose the thread family from dropdown field

Threading : Select the thread dimension you need. If you need to add a new row or edit some default data , open thread table and edit related property. To open the thread table you can click on the button at side of this field. Or from menu -> edit -> thread table.

Pitch : It's one of the field that will be defined automatically after choosing thread row. You can edit it manually

External Threading : Check this if you need to create an external threading.

Depth : Thread depth measured from [Start Z] level.

Thread Mode : You can choose between :

1. Right Handed - Climb
2. Right Handed - Conventional
3. Left  Handed - Climb
4. Left  Handed - Conventional

The suggested working method is Climb

Compensation Mode : See related page for more info.

Step Count : For larger thread , it's better create the thread with multiple axial pass.

First Step % : Available when you select for the one pass to create the thread. It indicated the % of material removed from the first pass.

Internal Thread

After selection of thread dimension. All the thread related property are filled with data from thread table.

Diameter : It's the diameter of thread helix. In case of [Computer] or [Tool Wear] compensation . it will be reduced by tool diameter.

Predrill Diameter : It's used as start approach diameter. The tool will reach touch this diameter and then will approach the helix diameter with a arc tangent movement.

External Thread

After selection of thread dimension. All the thread related property are filled with data from thread table.

External Diameter : It's used as start approach diameter. The tool will reach touch this diameter and then will approach the helix diameter with a arc tangent movement.

Inner Diameter: It's the diameter of thread helix. In case of [Computer] or [Tool Wear] compensation . it will be increased by tool diameter.

Multi Teeth Tool

From tool geometry screen , is possible define multiple teeth .

The generated toolpath will be compensated in order to use all the teeth, resulting in shorter toolpath. 

Toolpath created with single tooth tool.

Toolpath created with multiple teeth tool.

Adaptive Toolpath Strategy

It's considered a high efficiency because it can easily extend your tool life using a different path compared to the traditional OFFSET strategy.

This is the common default OFFSET toolpath. In indicated point the tool work almost at full cut and there is a big engagement angle.

This one is the toolpath generated with ADAPTIVE strategy . You can see the tool works with constant load and never exceed a high engagement angle. In this way you can use deeper passes in order to distribute the force all along the flute.

• https://www.harveyperformance.com/in-the-loupe/8-ways-youre-killing-your-end-mill/ , in particular to section "Using Traditional Roughing" 
• https://www.cnccookbook.com/thinking-about-high-speed-machining-corners-stepover/
• https://www.cnccookbook.com/high-speed-machining-trochoidal-milling-hsm-speeds-and-feeds

How to change feed value to link moves ?

From version 4.1.0.111

You can edit the default feed in link moves from post processor dialog.

1) Select the Machine Properties tab

2) Search "adaptive"

3) Insert your custom value. Leave 0 to use the fabric default value.

Chamfering Operation

You can find the chamfering operation in almost all the milling machining.

It's used to create a chamfer on the material with a tapered tool.

Chamfer Depth : It's the dimension of the desired chamfer

Step Count : Sometimes it's preferable create the chamfer with multiple passes, with this property you decide how passes you need. The tool depths are calculated keeping constant the volume of removed material .

Additional tool depth : This property allow to move the tool down in Z- direction , but keeping the same chamfer depth .

Useful if you want to move the contact point away from tool tip.

Tool Diameter Compensation

In Alexsys there are 3 compensation mode available :

1. Computer Mode
2. CNC Mode
3. Tool Wear Mode

Computer Mode

This is the most compatible mode, since the final path is calculated automatically. The output code don't contains any command related to compensation ( usually G41 - G42 )

It's not possible adjust the toolpath from the machine tool table. You don't have to worry about setting tool diameter in Tool Diameter register.

It's not indicate if you have to keep tight tolerances in your workpiece.

See info about output code .

Computer Compensation Mode:

CNC Mode

This the least compatible mode. The output path reflect exactly the geometry profile. All the offset distance and effective toolpath are calculated by cnc machine.

With this mode is necessary define tool diameter in cnc machine tool table. Is possible adjust tool wear value in order to compensate possible tool deflection.

CNC Compensation Mode:

Tool Wear Mode

The offset diameter is calculated by the computer, but you can also adjust the toolpath editing the machine tool wear table .

This permits to have less incompatibility issues with cnc.

Tool Wear Compensation Mode:

Both in CNC Compensation and Tool Wear compensation, if toolpath engine can't create proper lead in / lead out movement, an error is raised.

If this happen, try to reduce the approach radius value , under the finishing operation

Output Code

To help the machinist have clear what compensation is enabled and what values has to insert in cnc tool registry, in the output code are visible all this information.

Both in tool summary and when the tool is actually called.

Computer Compensation Example :

In Tool Summary :

(#7 - END MILL D 8MM COMP COMPUTER - RADIUS COR VALUE 0)

On Tool Called :

N5 (POCKET - FINISHING) (COMP COMPUTER - RADIUS CORRECTOR VALUE 0) (END MILL D 8MM)

CNC Compensation Example :

In Tool Summary :

(#7 - END MILL D 8MM COMP NCCONTROL - RADIUS COR VALUE 4)

On Tool Called :

N5 (POCKET - FINISHING) (COMP NCCONTROL - RADIUS CORRECTOR VALUE 4) (END MILL D 8MM)

Tool Wear Example :

In Tool Summary :

(#7 - END MILL D 8MM COMP TOOLWEAR - RADIUS COR VALUE 0)

On Tool Called :

N5 (POCKET - FINISHING) (COMP TOOLWEAR - RADIUS CORRECTOR VALUE 0) (END MILL D 8MM)

In this way , directly from gcode , you can see what compensation mode is going to be activated , and what value have the machinist have to insert in the machine tool table.

From this comments ,you have to set the tool diameter only with CNC Compensation, with the other two modes you have to set to 0 the tool diameter.

Operations Logical Sort

In home treeview toolbar, is visible the Logical operation sort button. 

When enabled , all the operation are keep sorted by logical flow of the machining logic.

So , for example, the centering operation comes before the drilling operation, the drilling operation comes before the tapping operation, the roughing operation comes before the finishing operation and so on.

Advanced Profile Selection

With [Chain Selection] is possible select contiguous entities. Entities be defined contiguous when they have a common endpoint. 

But sometimes we need to extract profiles from intersection geometries. See case below.

In this case , it comes useful another kind of profile selection. To add entities to selection you can :

• Keep pressed [CTRL] and keep pressed [Mouse Left Button]  and hover with cursor to ADD to selection group .
• Keep pressed [CTRL] and single Click on entity with [Mouse Left Button] to ADD to selection group .
• Keep pressed [SHIFT] and keep pressed [Mouse Left Button] and hover with cursor to REMOVE from selection group .
• Keep pressed [SHIFT] and Single Click on entity with [Mouse Left Button] to REMOVE from selection group.
• Press [ESC] to reset current selection

Appendix

Import 2D CAD File

Import DXF/DWG

With Alexsys you can import 2D geometries from DXF / DWG files.

1. First select the plane you want to import the geometries you can select the XY or the XZ planes.

   The XZ is the lathe plane.

   

2. From menu [FILE] -> [OPEN FILE]

   Choose the file you want to import.

   How to generate G-Code

   To Generate G-Code , press this button from main Menu or press F8 from keyboard.

   

3. This window dialog is the next step , here you can define gcode output filepath.

   Press G-Code or keyboard [ENTER] to generate GCode.

   After generation the generated machine code will be opened into select text editor.

   

   ---

   If may receive this error message : 

   

   This means that some operations toolpath are not valid.

   Look at tree view you have some operation with error icon.

   

   Hover with mouse cursor the error icon to read message error.
   You need to solve all the issue before call g-code generation.

Cad Editor

Alexsys is not intended to be a full CAD system, but with the available tools is possible draw basic profiles or do some little edits to imported geometries.

Under Menu -> Draw  , are available all the command below. See also the related links to get more information.

Toolpath Simulation

Is possible get the simulation of generated toolpath with the command "Simulation"

From Menu -> Simulation , or press F6 from keyboard.

Here the simulation side screen.

With simulation control you can single-step forward or backward.

Pause and continue simulation

With this control you can increment simulation speed. Drag the cursor with mouse

This slider stand for the current operation timeline, you can drag the cursor forward or backward.

Tool Mode : is possible show the tool with transparency or hide it completely

Continue with next operation : If checked, at the end of an operation simulation, the next operation is played. Otherwise the animation is stopped. Use the 2 button to go to next or previous operation manually.

Show complete toolpath : If checked, all the movements of current operation are shown .By default , just a the last part of the toolpath is visualized . The length of this visualized toolpath is determined by the property "Toolpath length".

Stock Simulation : If checked, the material removal simulation is shown. This option might impact on performance.

Stop on Collision : When a rapid collision is detected, the animation is paused on collision event. This option , is enabled only when the stock simulation is active.

Information : Current tool position and cut data parameter are visible in the lower part of the screen.

Basic Concepts

{EMPTY_LINE}
{LINE_N}
({OP_DESC})
{RADIUS_COMP_INFO}
({TOOL_LABEL})
T{TOOL_POS}M6
{NEXT_TOOL_POS}
{FEED_MODE}
S{SPEED_VALUE}{SPINDLE_ORIENTATION}
{ORIGIN}
{COOLANT_CODE}

LINE_N = N5
TOOL_POS = 15
NEXT_TOOL_POS = 10
FEED_MODE = G98
SPEED_VALUE = 2387
SPEED_ORIENTATION = M3
ORIGIN = G54
COOLANT_CODE= M8

N5
(CONTOUR - ROUGHING)
(COMP COMPUTER - RADIUS COR VALUE 10)
(R390 D 20MM)
T15M6
T10
G98
S2387M3
G54
M8
...

Thread Table

In Alexsys is available also a thread database for the most used thread tables.

This mean you don't need to search diameter or pitch values to create machining operation.

Just select the desired thread item from a list to compile all the necessary data.

To open thread table dialog , from menu click EDIT and then THREAD TABLE

Add custom data

This database can be expanded with custom data.

Open the thread table dialog.

• Select the desired thread family ( category)
• Insert the new values in the last row of the table.

To find reliable thread information , search directly from tool builder website. There you can find more information about everything . Suggested pass count,thread depth and angle , predrill and some useful tips about thread machining.

Edit Pitch

To edit pitch value , simply click on [Pitch Details]

Is possible to edit :

• External Thread Height
• External Passes Count
• Internal Thread Height
• Internal Passes Count

Edit Category

Also the thread category are editable.

Is possible to edit :

• Description
• Unique Id
• Select between TPI and Pitch values
• If is tapered or not
• Taper Angle

This information will be used in code generation.

If you want to hide the a category, check the "HIDE THIS CATEGORY FROM DROPDOWN THREAD LIST" field.

3D Stock Model

In Alexsys the 3D stock is modeled with defined machining operations.

From preference dialog you can choose how the model is created . From Menu -> Edit -> Preferences -> 3D Model Creation Mode

1 ) By Toolpath

The generated 3D model, is the effective result of the toolpath movements.

In this way you can see if there something wrong with generated toolpath.

For example, in the case below you can see the material left in the corner from the end mill machining. This is what you get on real machining.

[Simulation Stock Quality] is related to the stock in simulation context.

[Static Stock Quality] is related to the stock modeled in viewpoint context.

2 ) By Work Properties

This generation mode is usually faster , especially for simple 3D model, but it doesn't reflect the effective toolpath.

Some work machining like threading and engraving are not elaborated .

In the example below you can see the model is not considered the corner radius of the pocket. It's just used the profile and work parameter to model the stock.

Textbox integrated calculator

Every numeric textbox has an integrated expression solver.

This mean you can insert expression like " ( 6+6 ) * 2 ", and when you leave the textbox field, in the text box will convert it to 24 as result.

Unit Conversion

Is also possible unit conversion , from [mm] to [inch] and from [inch] o [mm] units.

Just insert [mm] or [in] suffix at te end of inserted value.

Example:

In a [mm] unit file instance, set as text " 1 in " or 1 inch in any numeric textbox .

The value will be converted in 25.4 mm .

Timeline

In the window application bottom , is visible the timeline control.

1) It's the time of current selected operations.

If you hover this label, you can see the timing grouped by setup, if you have multiple setup in your project.

2) Here it's a graphical representation of machining time of each operation.

The purpose of this graphic is too see at glance what operations are taking most of the machining time.

Every operation has a different color, if you hover it with mouse cursor you can see the related operation in the viewpoint.

Click on color bar to select related operation.

Manual Code

With [Manual Code] operation , is possible add manual text in output g-code program.

Load Template : Load existing gcode.

Description : It's the name of current template . It's used as identifier when you need to save , load or delete a template.

Insertion Mode :: Write only g-code : In output gcode related to this operation, you get the imputed text without any other command.

Insertion Mode :: Call Tool + Manual Code : In output g-code related to this operation , you get also the tool change and tool disengagement logic.

Save Template : Save the current text as template. You can find it in template list after this.

Delete Template : It will delete the related template from list.

G-Code Text : It's the manual g.code text you are going to add in output code.