anafranil online
IPB

Welcome Guest ( Log In | Register )

 
Reply to this topicStart new topic
> Tool End 5D Machining operation, SprutCAM 2007 Tool End 5D Machining operation tips and tricks
Live
post Mar 10 2009, 06:54 PM
Post #1


Member
**

Group: Members
Posts: 21
Joined: 10-February 09
Member No.: 2,767



= The Tool End 5D Machining operation =

The Tool End 5D Machining operation can be used for 3 axis and 5 axis isoline machining, as well as for swarf machining, 3 axis and 5 axis curve engraving, fillet machining, chamfer machining and slot machining, as well for 5 axis trimming and 4 axis rotary machining. By now there is no gouge and collision checks for the Tool End 5D Machining operation, so it is crucial to check the machining result for gouges and collisions in the Simulation mode.

== Job Assignment of the Tool End 5d Machining ==

=== Drive Faces item ===

Drive faces in the Job Assignment of a Tool End 5D Machining operation define the geometry that should be machined by the operation. Drive faces control as well the flow of the toolpath. Machining is fulfilled along isoparametric lines of the drive faces.


==== Drive Faces Item properties ====

Drive faces have the following properties:

1. The Alternate front side option defines the machining side of drive faces: front or back. The front side is colored lime while the back side is colored black.
2. The Alternate streamlines option defines the flow of toolpath: along surfaces U-curves or along surfaces V-curves.
3. The Step Method drop down list defines the way isoparametric curves are distributed on a drive face. This option can take following values: Number, Distance.
4. The Step amount field defines the number of isoparametric curves on a drive surface. If the Step Method is set to Number then The Step amount is simply the number of curves on a drive surface. If the Step Method is set to Distance then the Step amount is the geodesic distance between two neighboring surface isoparametric curves.
=== Project Curves feature ===

It is possible to project curve entities onto the part geometry of a Tool End Machining operation. This kind of geometry can be used as the job assignment for the 5Axis and 3 Axis curve engraving. Curves are projected onto the part faces by shortest distance.

==== Project Curves Item properties ====

The Project Curve Item properties include the following options:
1. The Alternate direction option defines the direction of curve machining: forward or backward.
2. The Alternate front side option defines the front side of the machining.

=== Using the part edges in the Job Assignment of a Tool End 5D Machining operation ===

It is possible to add part edges as well as edge chains into the job assignment of a Tool End 5d Machining operation. This feature can be used for Swarf, Chamfer, Fillet and Slot machining.
To add an edge chain into the job assignment select it in the view and press the Project curves button. Projected edges have the same properties as general projected curves.


== Parameters of the Tool End 5D Machining operation ==

=== Contact tool type ===

The Contact tool type parameter defines the method of tool axis control. There are three types of tool contact methods: Face milling, Flank milling and Roll milling.

• By face milling the tool is placed normal to a machined surface. It is possible to set the additional Tilt and Incline angles to tilt the tool axis. The tilt angle is measured relative to the tool motion direction. In other words, this is the lead angle. The Incline angle is measured perpendicular to the tool motion direction. In other words, this is the lean angle.

• By Flank milling the tool is placed in such a way to contact a part surface by tool side. This option is used for Swarf milling, chamfer milling and slot milling. The tilt and incline angles can be specified to tilt the tool axis from the default position. The Inverse tool axis direction option can be checked to alternate the orientation of the tool axis to opposite direction.

• By Roll milling the orientation of the tool axis does not depend on the surface normal and stays the same for all toolpath points. The tool axis orientation is determined by two angles: Rotation around X axis and Rotation around Y Axis. This kind of machining can be used for Isoline 3d machining.


== Safe Axis ===
By a five axis machining the tool axis orientation varies continuously so it is impossible to specify a distinct safe plane where rapid movements can be made safety without a damage of collisions of machine tool parts with a workpiece. So in SprutCAM 2007 the Safe Axis parameter is used in Tool End 5D Machining operation to define the space of safe tool transitions.

To define a safe axis you should specify the safe axis coordinate. It is a linear motion coordinate: X, Y, Z etc. You also should specify the Safe level amount in current system units (mm or in).
The safe axis feature works as follows. When the tool reaches the terminate point of a tool pass a multigoto instruction MULTIGOTO <Safe Axis Coordinate> <Safe Axis Distance> is inserted into the MCD tree, than the tool is moved to the next tool pass on rapid feedrate.

=== Stock ===

The Stock parameter is used to leave uncut material on the part.

=== Levels ===

The Levels panel on a strategy tab is used to specify machine levels of a roughing Tool End 5D Machining toolpath. The levels are defined by the Top and the Bottom level as well as the Step between levels.

== Tool End 5D Machining practices ==

=== 1. Five Axes Face Milling ===

To create a Five Axes Face Milling operation:

1. Create a new Tool End Machining operation.
2. Add Drive faces into the job assignment of the new operation. Define the drive faces properties: the machining side, the drive curves flow, the drive curves step.
3. Open the operation parameters dialog. On the Strategy tab Set The Contact Tool Type to Face, define the Safe Axis, specify the machining stock and the roughing levels.
4. Generate the toolpath.

=== 2. Five Axes Swarf Milling ===

To create a Five Axis Swarf Milling operation:

1. Create a new Tool End Machining operation.
2. Add drive faces into the job assignment of the new operation. Adjust the drive faces properties.
3. At the Strategy tab of the Operation Parameters Dialog set the Contact Tool Type to Flank.
4. Generate toolpath. If the tool axis is inversed check the Alternate tool Axis Option at the Contact Tool Type panel of the Strategy tab and regenerate toolpath. You may have to define addition axial displacement to machine through features.

=== 3. Five Axes Slot Milling ===

1. In the 3D Model mode activate the part folder and press the Sew button. The Sew dialog should appear. Press Ok to introduce part edges into the Geometry Model.
2. Switch to the Machining tab. Create a new Tool End 5D Machining operation.
3. Select the Job Assignment item of the operation. Ensure the Edges button at the Filters toolbar is checked. Select the Slot bottom edges chain in the view. Press the Project Curves button at the Job Assignment panel.
4. The Slot faces should highlight lime. If they do not, double click on the edges item at the Job Assignment toolbar and check the Alternate Front Side option, than press OK.
5. Open the operation parameters dialog. At the Strategy tab set the Contact tool type to Flank.
6. Generate toolpath. If the tool axis is inversed check the Alternate tool Axis Option at the Contact Tool Type panel of the Strategy tab and regenerate toolpath. You may have to define addition axial displacement to machine through slots.

=== 4. Five Axes Chamfer Machining ===

1. Create a new Tool End Machining operation.
2. Add the chamfer faces into the job assignment of the new operation. Adjust the drive faces properties: the isoparametric curves flow, the machining side and the curves step.
3. At the Strategy tab of the Operation Parameters Dialog set the Contact Tool Type to Flank.
4. Generate toolpath. If the tool axis is inversed check the Alternate tool Axis Option at the Contact Tool Type panel of the Strategy tab and regenerate toolpath. You may set an addition axial displacement to machine a chamfer with some axial shift.

=== 5. Three Axes Fillet Machining ===

1. Create a new Tool End Machining operation.
2. Add the fillet faces into the job assignment of the new operation. Adjust the drive faces properties: the isoparametric curves flow, the machining side. Set the Step method to Number and the Step Amount to 1.
3. At the Strategy tab of the Operation Parameters Dialog set the Contact Tool Type to Roll.
4. Generate toolpath..

=== 6. Three Axes Isoline Machining ===

1. Create a new Tool End Machining operation.
2. Add drive faces into the job assignment of the new operation. Adjust the drive faces properties: i.e. the machining side, the curves flow and the curves step.
3. At the Strategy tab of the Operation Parameters Dialog set the Contact Tool Type to Roll.
4. Generate toolpath.
Go to the top of the page
 
+Quote Post

Reply to this topicStart new topic
1 User(s) are reading this topic (1 Guests and 0 Anonymous Users)
0 Members:

 



Lo-Fi Version Time is now: 17th July 2019 - 12:20 PM