Hướng dẫn sử dụng phần mềm Mastercam-X4 - P10

Đây là hướng dẫn sử dụng phần mềm Mastercam-X4. hướng dẫn có các hình ảnh và ví dụ cụ thể

TABLE OF CONTENTS

PageLesson 1:

Advanced Pocket Toolpaths

Manual Drill Toolpaths

Lesson 10: FBM Mill Toolpaths

Lesson 11: 3D (HST) High Speed Toolpaths—Part 1

Lesson 12: 3D (HST) High Speed Toolpaths— Part 2

Lesson 13: Assembly Toolpaths: Configurations

Lesson 14: Assembly Toolpaths: Replacing Parts

LESSON 3 CONTOUR TOOLPATHS PART 2

INTRODUCTON:

This lesson builds on the basic procedures you were introduced to in the first Contour lesson You will gain ex

perience in additional geometry selection (Chaining) techniques that will allow you to cut most Contour shapes

you come across The toolpaths will consist of several new types of contours

Overview of Exercise:

In this lesson we will machine the part shown by first Facing the 5.0 X 8.0 stock, then machining the yellow

areas shown by using several different types of 2D contour toolpaths and tools

NEW CONCEPTS COVERED IN THIS LESSON:

Facing rough stock

Multi pass contour to cut an open pocket shape

Removing excess stock

Chamfer contour toolpath

Multiple techniques for contour chain selection

Chain Manager options

Review of basic Mastercam for SolidWorks general workflow procedures

Contour Toolpaths Additional Reference Information:

REFERENCE INFORMATION:

2D GEOMETRY SELECTION OPTIONS

Single Edge: Click the edge.

(The Mastercam Chain Manager gives the option to

automatically propogate along tangencies.)

Multiple Edges: CTRL-Click each edge.

(The Chain Manager will display all individual edges.

The CHAINS tab will show how Mastercam has

connected continuous edges into a single Chain.)

Select Tangency: Right Click on Edge and choose

the option from the menu

(This will select all of the edges tangent to the one

highlighted and put them in the Selection list in the

Chain Manager.)

option from the menu.

(This will select every connecting edge on a face,

whether tangent or not If the wrong Loop is chosen

by SolidWorks, click the yellow arrow to toggle to the

other option.)

Partial Loop: Click the first entity, then CTRL-RIGHT

Click on the second entity to choose the option from

the menu NOTE: When CTRL-RIGHT Clicking on

the second entity, you must select on the end of the

entity nearest the direction you want to close For

more information, see the SolidWorks Help menu.

(This will allow a faster method of selecting a large

number of individual edges on complicated contours.)

Select Face: Click on a Face.

(This will select every individual edge on a face,

including interior edges, whether tangent or not The

Chain Manager gives the option to use only outer loop

on faces This is useful if you only want to cut the

outer shape.)

CONTOUR TOOLPATHS PART 2 TUTORIAL

Process Step 1: Prepare and Orient Model for

Machining

In this task you will choose the view to machine from

and locate part on the machine Due to the shape of

the model, there is no good location for the origin We

will use SolidWorks to create the origin location first.

1 Open the part “CONTOUR 2.SLDPRT”

2 From the SolidWorks Drop Down View Menu, make

sure View Sketches is selected.

(We will need to see Sketches in a later step.)

3 Select this face and select Insert Sketch from the

pop up icons or from the SolidWorks Insert menu.

(This will start a new sketch on this top face The

following steps will have us create a single point at

the theoretical sharp corner of the stock So we can

locate the machining origin where we want it.)

4 Rotate the model similar to the view shown and

select both of the edges by pressing the Control key

and selecting these two edges

5 Select the Point icon from the SolidWorks Sketch

toolbar or from the drop down menu Tools – Sketch

Entities – Point, to create a point entity at the

intersection of the two lines

(Note: You must select the (2) edges first to get

the point at the intersection.)

6 Exit the Sketch.

(Right Mouse Click and Select Icon.)

7 From the Mastercam drop down menu, select

View Manager.

8 View Manager Dialog settings:

9 Select the Geometry button.

10 Rotate the model as needed so you can pick the top

Solid Face to be the Machine View.

11 Rotate XY as desired for Direction

(We will leave at 0° in this example.)

12 Click OK to accept.

13 Give the new view a Name

(“2D Machining View” in this example.)

14 Set the Current View and Origin equal to this new

view by clicking the “EQUALS” button.

15 Select button to choose the desired Origin Point.

16 Select the sketch point previously created

as shown

(In order to see this sketch Point,

View Sketches must be on See Step # 2)

17 Click OK to accept.

18 Click OK to Accept again to exit and save the View

Manager settings dialog

(The Mastercam Origin should be located on the

point entity as shown.)

Process Step 2: Create the Job Setup

In this task you will supply Mastercam with information

about tool information and stock size prior to beginning

the machining operations.

19 Select the Mastercam Toolpath Manager Icon from

the Property Manager page

20 Expand the Properties in the Toolpath Manager.

(Click the plus (+) sign if the Files, Tool Settings

and Stock Setup icons are not visible.)

21 Select the Tool Settings icon

22 Change or confirm the highlighted parameters as

shown:

REFERENCE INFORMATION

For further information on other settings, see the

Mastercam Help file by clicking

Program # Identifies the program in the output NC

machine code

Feed Calculation from tool uses the feed rate,

plunge rate, and spindle speed directly from the tool

definition

Assign tool numbers sequentially assigns the next

available tool number This option overrides the tool

numbers stored in the tool definition

Warn of duplicate tool numbers informs you when

a duplicate tool number is entered and displays a

description of the duplicate tool

Override defaults with modal values When

selected, the default values for any of the checked

items will be the value from the previous operation

These override the values found in the toolpath

defaults file

23 Select the Stock Setup tab.

24 Select the icon and then set the Stock View to the

previously created view (“2D Machining View”)

25 Select the Bounding Box button.

26 Accept the default Bounding Box values as shown:

(In this example, the Stock size will be defined as

the extents of the solid model.)

27 Click OK to accept and close the Machine Group

Properties.

Process Step 3: Toolpath Selection and

Generation

During this section you will select the portions of the

solid model that CNC tool will cut We will generate 5

separate operations to machine the part in this process

step These will include:

Facing the Top of the Stock

Open Contour Toolpath with Multiple Passes

Partial Contour Toolpaths

Contour the Entire Outside Periphery

Chamfer the top edge

Facing the Top of the Stock

28 Select Facing Toolpaths from the Mastercam

Drop Down Menu or Command Manager

(Facing operations will machine the entire top

surface of the model to prepare for subsequent

operations.)

29 Rotate model as needed and select the top face as

shown:

(Note: In this example, the shape is simple enough

to allow selecting the top face In other cases,

additional sketching may be required to define the

stock shape for the facing operation.)

30 Click OK to accept and close the Chain Manager.

(In facing operations, the entire boundary must be

closed and the facing tool cuts inside the boundary,

so chaining direction and cut side is not required to

be set in this example.)

31 When prompted, enter a name for the NC program

we are going to create

(“CONTOUR 2” is used in this lesson.)

32 Click OK to accept and close the NC name dialog

box

33 Facing Toolpath Parameters Dialog Box Preview:

(In the following steps we will be setting the

parameters to make our Facing toolpath.)

34 Toolpath Type:

Facing

35 Tool:

Select Library Tool

(We will choose a 2” Face Mill from the Library of

tools provided by Mastercam.)

36 Select the Filter button.

(The Filter button will allow searching through the

tool library for a specific tool type to make it easier

and quicker to find the desired tool.)

37 Select the None button.

(This will de select all tool types to clear the filter.)

38 Select the Face Mill tool type.

(You can hover your cursor over the icons to see

what tool type is represented by each icon.)

39 Confirm that the rest of your settings match the

screenshot as shown and click OK to accept.

40 Select the 2” Face Mill from the filtered list and

click OK to accept.

41 Other Tool settings:

(Tool numbers should be automatically assigned

from our Job Setup settings.)

Rapid Retract = Selected

Comment: (Enter a description of what the toolpath

does This will be part of the NC program to assist

the operator of the machine identify what this part

of the program does.)

In this example we inserted “FACE OFF THE TOP OF

THE STOCK”

Move between cuts = High speed loops

43 Linking Parameters values:

Clearance = 2.0 (Absolute)

Retract = 25 (Absolute)

Feed Plane = 0.1 (Incremental)

Top of Stock = 0.0 (Absolute)

Depth = 0.0 (Absolute)

(Depth value is set from the value of the selected

faces In this case, Absolute depth of the top face is

46 Results of Facing parameters:

47 Select the Operation and Backplot and/or Verify

the toolpath operation to confirm your results

Open Contour Toolpath with Multiple Passes

(In this operation we will remove the cutout area using

Contour toolpath.)

48 Before starting the next operation, turn off the

toolpath display for the Facing operation

(This will remove selected toolpaths to make it

easier to view and select the model edges for the

next operation.)

49 Select Contour Toolpaths from the Mastercam X4

Drop Down Menu or from the Command Manager

50 Rotate the model as shown, then Right Mouse Click

on the edge Shown and choose Select Tangency.

(We are using the SolidWorks selection option to

select all of the entities that are Tangent to this

edge instead of selecting each entity individually.)

51 Results:

(You should have 5 edges in the selection list If you

do not have all 5, you may select the missing edge

from the model or Right Mouse click in the box and

Clear Selections to try again.)

52 Select Chains tab in the Chain Manager.

(Notice that all 5 edges have been combined into

one continuous chain automatically by Mastercam

for SolidWorks.)

53 Click on “Chain 1” in the Chains Selection box.

54 Verify the Direction of cut and Cut side of the

selected chain by selecting the icons

(Match screenshot shown to Climb Cut

the contour.)

REFERENCE INFORMATION

Change Sides changes which side of the

selected chain the cutter will travel

Delete Chain deletes the currently selected

chain(s) from the list

Analyze Chain provides technical information

about the selected chain

Reverse Chain changes the selected chain cut

direction

Rename Chain allows changing the name from

Chain #1, etc to a more meaningful name to

help user recall the purpose of the chain

Start Point allows user to change the start

point by scrolling through each possible chain

point

End Point allows user to change the end

point by scrolling through each possible chain

point

55 Click OK to accept the Chains and close the Chain

Manager

56 Contour Toolpath Parameters Dialog Box:

(In the following steps we will be setting the

parameters to make our toolpath.)

57 Toolpath Type:

Contour

58 Tool:

Select Library Tool

(We will choose a ½” Flat Endmill from the

Library of tools provided by Mastercam.)

59 Select the Filter button.

(The Filter button will allow searching

through the tool library for a specific

tool type to make it easier and quicker

to find the desired tool.)

60 Select the None button.

(This will de select all tool types to clear the filter.)

61 Select the Flat Endmill tool type.

(You can hover your cursor over the icons to see

what tool type is represented by each icon.)

62 Confirm that the rest or your settings match the

screenshot as shown and click OK to accept.

63 Select the 1/2 Flat Endmill from the

filtered list and click OK.

64 Other Tool settings:

Rapid Retract = Selected

Comment: “REMOVE THE OPEN POCKET AREA”

65 Cut Parameter Settings:

Compensation = Wear

Stock to leave on walls = 005

(We will leave 005 for final clean up contour

operation we will add later Confirm other settings

match the default values as shown.)

66 Lead In/Out Settings:

Lead In/Out = Selected

Entry = Selected

Entry Line Tangent = 30%

Entry Arc Radius = 30%

Select the Double Arrow to copy all values to the

Exit Values.

67 Set Break Through values as shown:

Break through = Selected

Break through amount = 0.05

68 Set Multi Passes settings as shown:

Multi Passes = Selected

Rough = 3

Spacing = 25

Finish = 0

Spacing = 0

Keep tool down = Selected

(Since there is no danger of cutting through the part

in this toolpath, it is more efficient to keep the tool

down.)

69 Set the Linking Parameters values as shown:

Clearance = 2.0 (Absolute)

Retract = 25 (Absolute)

Feed Plane = 0.1 (Incremental)

Top of Stock = 0.0 (Absolute)

Depth = 0.0 (Incremental)

(Depth value is set from the value of the chained

edges Incremental value is used in case there are

multiple edges are at different depths Incremental

values always display 0.0)

70 Set Coolant value:

Flood = ON

71 Click OK to accept the Contour Toolpath Parameters.

72 Results:

73 Select the Operation and Backplot and/or Verify

the toolpath operation to confirm your results

(If your verify does not look like this result, click the

Parameters icon under the Contour operation in the

Mastercam Operations Manager and confirm your

settings are correct Then Regenerate the toolpath.)

Partial Contour Toolpaths

(In this Contour operation we will remove the excess

material at the four corners of the stock.)

74 Before starting the next operation, turn off the

toolpath display for the Contour operation you just

completed

75 Select Contour Toolpaths from the Mastercam

Drop Down Menu or from the Command Manager

76 Rotate the model as shown and select the 3

individual edges as highlighted

77 Rotate the model so you can select 3 more edges

from the next angled corner of the model

78 Repeat rotating the model and selecting the edges

for all 4 angled corners When complete, you

should have 12 edges listed in the Selection list.

79 Select the Chains tab in the Chain Manager.

(Notice once again the Mastercam has combined

the 12 edges into 4 separate chains.)

80 Click on Chain 1 in the Chains Selection Box.

81 Verify the direction of cut and cut side of the

selected chain by selecting the icons

(Cut side and direction should match screenshot so

we Climb Cut the contours.)

82 Repeat for Chain 2, Chain 3, and Chain 4 Make sure

cut side and cut direction matches the screenshot

(We want to make sure the cutter is on the outside

of the part and moves in direction shown so we

Climb Cut the contours.)

83 Click OK to accept the Chains to close the Chain

Manager.

84 Contour Toolpath Parameters Dialog Box.

(Most settings should remain correct from the

previous contour operation.)

Confirm the following Settings All others set as in

screenshot or as desired:

85 Toolpath Type = Contour

86 Tool = ½ “ Flat Endmill

Rapid Retract = ON

Comment = “Remove excess stock from corners”

87 Cut Parameters:

Compensation type = Wear

Compensation Direction = Left

Contour Type = 2D