Alexsys V4 Turn Operator Manual
ALEXSYS is a programming system for CNC turning 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.
The lathe module support all the most common turning operations.
- Face Turning
- External / Internal Turning
- External / Internal / Face Grooving
- Central Drilling
- External / Internal Threading , also tapered threads
Diameter Mode - Auto : Start and end diameter value are defined by stock dimension
Diameter Mode - Manual Values : Start and end diameter value are defined manually
Start Z : Reference Z , usually it's always 0
Corner Mode : Choose between chamfer or fillet
Init Chamfer : It the chamfer/fillet value.
1) Roughing Operation
Material to remove : Is the material width to remove , measure from Start Z to Z+ direction
Finishing allowance : Is the material width left to finishing operation by the roughing operation
2) Finishing Operation
No options for this operation.
External Cycle : The tool moves from the outside the inner part of the component.
Internal cycle : The tool moves from the inner part of the component to outside.
Before proceed with internal cycle is necessary create a central hole in the component.
In important also use a tool with dimension compatible with this hole diameter.
You can find this information in tool catalog.
To add this operation, from [MENU] -> Lathe -> External or Internal Turning , depending on your needs.
Here the screen related to external / internal turning machining.
Generic turning accept as geometry both open profiles and closed profiles.
It's suggested to link just a single profile in geometry list.
Turning direction - Traditional : Tool direction it's from Z+ to Z-
Turning direction - Reverse : Tool direction it's from Z- to Z+ , you need to select a compatible tool when you change this property.
Profile Start/End Extension : A tangent extension will be added to start/end of selected geometries
Apply Fillet on sharp corner : Where applicable, a fillet will be created in sharp corner.
Toolpath Limit : With this you can define the limits of working area.
Without Limit :
With Limit :
Operation 1 of 2 : Roughing
Finish Allowance X / Z : It's the material thickness left by the roughing tool for the finishing operation.
Roughing Macro : Where applicable , it will print G71 macro code in output code instead of simple movements
Finish with same tool : Finishing allowance material will be removed by the roughing tool
Operation 2 of 2 : Finishing
Reverse direction on vertical wall : When enable , the turning direction will be inverted in 90° profile element. In some context , this may reduce tool vibration.
Vertical wall threshold : Will be considered only elements with length bigger than this value.
Multiple finishing passes : It create multiple finishing passes. The distance between passes is determined by finishing allowance thickness.
example : If you have a 0.3mm of finish allowance and 3 finish passes. Toolpath will generate 3 passes with a 0.1mm distance between them.
Lathe Central Drilling
To add a drilling machining , from Menu -> Lathe -> Central Drilling
This is the machining property screen.
Here you can enable these sub-operations :
- Center Drill
You can change the sub operation order manually from treeview. See related link at the bottom of this article.
When a drilling operation is selected, is possible see also "ghost tool model" at the minimum reached z.
This is useful to check the tool path correctness at glance.
Safe Z : It's the Z Level of approach . The tool arrives at this level in rapid.
Start Z : This is the effective start working level. Usually it's 0
[Drill Operation] Add Drill Tip Length : It calculate the drill tool tip length and add it to inserted depth.
The drill tip length is calculated by tool diameter and tool angle. You can edit this properties from tool edit screen. See related link below.
[Chamfer] Define Chamfer Diameter : In chamfer operation is possible define the plain tool depth to execute or desired chamfer outer diameter.
If you select to define the outer chamfer diameter, the effective tool depth will calculated automatically based on selected chamfer tool geometry.
To add an threading machining operation , from MENU -> LATHE -> select EXTERNAL or INTERNAL Threading.
In the screen below you can see requested parameter.
You can pick thread default data by selecting a thread category and then selecting desired thread row from the drop down property.
After selecting desired thread, all related field are filled with default data from thread table.
To open thread table window , you can click on button indicated in following image, or from MENU->EDIT-> THREAD TABLE
Lathe cut-off operation
When is necessary cut away turned part from bar, you need the Cut operation .
Pick Point : Let you select outer diameter and Length with mouse cursor.
Outer Diameter : It's the start diameter of cut cycle
End Diameter : It's the end diameter of cut cycle. This diameter is compensated with tool nose radius in gcode.
Length: It's the desired length of part.
Chamfer : You can create a chamfer or fillet in cut corner.
Chip Breaking Movement : When enabled, it create a chip breaking movement instead of a plain work movement to cut the part. This help to create smaller chip.
Basic Lathe Tutorial - Bullet Shape
- 1 - Overview
- 2 - Import Cad Geometries
- 3 - Add First Setup
- 4 - Stock Definition
- 5 - External Turning
- 6 - Play Simulation and Generate G-Code
1 - Overview
This tutorial will cover the basic to import a simple DXF / DWG 2d drawing and apply a turning cycle.
Here the sample dxf for this tutorial.
2 - Import Cad Geometries
It a good practice clean the dxf files and leave only the profiles you want to import.
You can remove all unnecessary entities from Alexsys, but to keep thing easy , it's suggested do this cleaning process directly with the cad software.
To import the dxf file, from Menu -> File -> Open , select the dxf file with the file selection dialog.
After cad import, Alexsys screen will be like this :
The tool screen "Adjust Imported Geometry" is called automatically.
This screen contains all the common modifier usually applied to imported geometry. Like rotate , scale , mirror and so on.
We need to create a turned part, so the profile must lie in the XZ plane. Under the CHANGE PLANE section, click on Move to XZ Plane.
The current geometry is very much not centered with the coordinate origin, So maybe after calling change plane, the geometry will be off screen. Just recall the 2D view to zoom to fit the scene.
You can also see the label in top of 3D viewpoint now indicate PLANE XZ
If you move the cursor around the 3D viewpoint, you can see huge coordinate values.
The geometries are in a not well precised position in 2D space.
We need to move it to X0 Z0 position. To do so , scroll down the side screen and click on PICK ORIGIN.
After that, click on the indicated point in the image below.