Giáo trình VISI machining 2d

Ứng dụng công nghệ gia công tiên tiến nhất trên thế giới VISIMachining (Lập trình gia công cho máy Phay CNC 3, 4, 5 trục) đã làm cho người sử dụng hài lòng việc ứng dụng VISISeries vào trong thiết kế và gia công khuôn mẫu… Việc tích hợp VISIFlow (phân tích và mô phỏng dòng chảy nhựa) là một giải pháp kết hợp hoàn hảo, giúp cho qui trình thiết kế khuôn gần như là khép kính. Chúng cho phép phân tích và tính toán vị trí bơm keo và phân bố đường nước sao cho hợp lý để cho ra sản phẩm như mong muốn. Đây là giải pháp giúp các doanh nghiệp tiết kiệm rất nhiều thời gian và chi phí cho một quá trình sản xuất khuôn.

2D CAM Training

geometry methods, too editing the toolpaths and geometry

Things that will be covered in this training document:

• Creating Manual Features

• Creating Toolpaths – Pocketing, Milling, Face milling

• Creating a Drilling operation

Manual Features

From the menu select file > Open

The file that were about to use is installed by default and can be used at any time

Navigate to the following location and open the file - Compass Technology.wkf

C:\Visi16\Workf\Sample\Cam

The file itself is made of solid models In version 16.0 of Visi It is now possible to directly machine in 2D from a 3D model

From the menu select Machining > CAM Navigator

Inside of the CAM Navigator it is possible to define all of the Machining that is required This ranges from 2D all the way through to 5 axis, all of which uses this main interface Inside of the CAM Navigator you will see there are two pages, Feature and Operations The Features page is used to control all of the Model geometry that is being machined e.g Pockets, Profiles, Holes, Piece Material, Stock Model, Obstacles

The Operations page is where all of the toolpath data is stored Inside of this window it is possible to edit the machine tool that is being used and which tool crib is being used,

modify the toolpath parameters e.g Step over and step down, Tool that is being used, post processor that is being used

The first thing that we will do is to define a pocket to be machined out

From inside the Feature page right hand click on the Model Manager option and select

Add manual Feature

A manual feature can be a combination of things, face, point, circle, arc, profile and set of points This will allow you to pick any of these items and create a blind hole, through hole, closed pocket, open pocket and a boss

With this option selected the system will ask you to pick a face or element Ensure the face

selection icon is active and pick on the green face as shown bellow

Once this face has been selected the system will open a new dialog box displaying the information about what has been picked

Inside of this dialog box it is possible to add and remove geometry that has been selected

or miss-selected

Select this Face

Select Ok to the dialog box

With the model selection now confirmed the system will now open the Feature parameters dialog box

Inside of this dialog box it is possible to define what kind of manual feature you wish to create by changing the feature subtype drop down box

Selecting this icon will

allow you to add more

geometry to the selection

This icon will allow you to pick an item from the selection tree and remove this from the selection

Please note that this list can vary in length depending on the shape of the feature that has been picked e.g

Cylindrical Hole or Point =

Inside of this dialog box it is also possible to define a variety of parameters for the feature

that has been chosen e.g diameter, tip angle, thread diameter These parameters are

feature sensitive, so if that particular parameter does not have an affect on that feature it

will be greyed out

In this dialog box it is also possible to directly interact with the feature Manager if a

cylindrical hole or Point has been selected by picking on the “Feature attribute icon” this will allow you to assign a feature such as tapping, counter boring, drilling to a hole

Ensure the feature subtype is set to pocket and the height is 20 and select OK to the

dialog box

Once the Feature parameters have been confirmed you will now see a feature has been added to the Model Manager tree

With the feature now added it is possible to add our first toolpath

N.B All parameters for features, toolpaths, models etc are all controlled from the right hand mouse menu

Right hand click on the newly created feature and select

“Add Operation”.`

The system will now open the Operations dialog box

Inside of this dialog box it is possible to select the toolpaths that is required The system is will filter out any operations that cannot be applied on the feature that has been chosen

1 Search – this command will allow you to type in the name of the toolpath you are looking

for in the text box provided

2 Clear Search – this will remove any search that has been applied

3 Add to favourites – this will allow you to select a toolpath and copy it into the favourite’s

folder This will allow you to develop a list of frequently used commands

4 Style – this changes the layout style of the dialog box

5 Delete – this command will allow you to remove a toolpath from the favourites section

Select the pocket operation and select ok

With the toolpath now defined, the next step is to select which tool we wish to use from the tool crib

1 Add tool from DB – This will allow you to select a tool from the VISI Tools database

2 Add tool manually– This option will allow you to create a tool manually from scratch

3 Edit Record – This option will allow you to edit the parameters of a tool

4 Duplicate Tool – This option will allow you to make a copy of a previously defined tool

5 Change Tool position – This option will allow you to edit the tool position in the crib

6 Edit tool holder – This option will allow you to add or edit a tool holder

7 Delete Record – This option will allow you to delete a tool from the crib

Select the 10mm Endmill from the tool crib and press OK

1 2 3 4 5 6 7

Pocketing

The system will now build the toolpath automatically based upon the system defaults

Note you will also now notice that in the Model manager tree the pocket feature text has gone from green to black This is to indicate that a toolpath has now been applied to that feature

We can now modify the toolpath parameters from with the operations page

Select the operations Page

Inside of the operations page you will now see the pocketing Spiral operation we have just created on the feature

Inside of the operations tree, it is possible to control all of the parameters of the toolpath and simulation options

Right hand click on the Pocketing Spiral operation

Operation tree – RHM

• Editing cutting conditions – Toolpath parameters

• Model geometry editing – Change or edit model

• Editing tools – Change or edit tools

• Editing boundaries – Machining Boundaries

• Editing User Priority – Operation Priority

• Copy – Copy toolpath

• Build Toolpath – Batch build Toolpath

• Re-set Toolpath data – Reset the toolpath data

• Save operation as a Template

• Cam Setup Shift factor – G54/55 Shift factor

• Toolpath Laboratory – Simulate toolpath

• Kinematic Simulation – Machine tool Simulation

• Toolpath Checker – Collision Point checking

• Posting – Post processing

• Toolpath report – Tool sheet

• Show/hide toolpath

Select the properties option from the right hand mouse menu

You will now be presented with a new dialog box that will contain all of the operation

parameters for the toolpath

Side allowance – Stock to be retained on the side of the part

Bottom allowance – Stock to be retained on the bottom of the pocket

Island Top allowance – stock to be retained on top of any island detected

Stepover method – this option will allow you to choose the different stepover methods

available Spiral Out, Spiral In, ZigZag, Oneway

Stepover – This is the Value or percentage that the toolpath will stepdown

Stroke angle – this option is only active when the stepover method ZigZag or one way and

will change the stroke angle on the passes

Corners method – this option will allow you to either have a sharp corner or add a set

radius to any sharp corners found to help avoid dwell marks

High speed radius – this option is only on when the corner method is set to round and will

allow you to define a radius for the sharp corner movements

Reduce retract movements – this option will try and remove any un-necessary retract

rapid movements where possible

Max Stepdown – this value define the maximum stepdown between passes

Last Stepdown – this option will allow you to specify a stepdown value to clear up the

bottom of the pocket

Machine island top – this option will allow you to profile machine the top of an island if

one has been found

Generate left overs – this option will build 2D profiles in the areas that the cutter cannot

get into

Cut Method – this will define the cutting direction to be climb or conventional

Profiling method – this option will add finishing passes at either the beginning or end of

the passes

Cut direction Method – this option will allow you to reverse or invert the stepover direction

N.B [%] – where any percentage value icon is present, it is possible to select this icon and allow you to use physical value instead of a percentage value

Transition Method – this option determines how the tool moves from one area of passes

to another

Rapid Distance – this Z value is the level in which the tool will go to before returning to the

machining level

Return between Levels – if this option is ticked, the tool will return to the clearance plane

or rapid distance after every level

Clearance plane – this value is the Z value when the tool is moving from one area to

another

Feed distance – this value is the amount feed movement created before the toolpath

moves in rapid

Transition Distance – this option defines the amount to lift up when moving from one

pocket to another

Entry Method – this option defines how the tool will approach the part

Angle – this option defines the ramp angle when the approach method is set to

descending

Increment – if the approach method is Zigzag this value is active and will allow you to

define the height in between each ZigZag movement

Generate Hole Feature – this option will allow you to pick a drill point to start machining

from

Face Mill Z Start – If possible the system will add a extra stock thickness and face milling

path to the top of the pocket

Maximum absolute Z – This option will allow you to change the machining Z top according

to an absolute Value

Minimum absolute Z - This option will allow you to change the machining Z bottom

according to an absolute Value

Max/min feature depth –

Max feature Z / extra Z+ - this option will allow you to add extra stock to the top of the

pocket

Min feature Z / extra Z- - this option will raise the base of the pocket if a plus value is

entered and lower the base if a minus value is entered

Min side / bottom radius – this option will allow you to add a radius to the bottom of the

pocket

Pocket / island draft angle – this option will allow you to add draft to any islands that have

been found

1 Model Manager – this option will allow you to check, add, remove the geometry that is

being used to produce the toolpath Inside of this option it is also possible to change start, approach, retract and end points

2 Tolerance – this option will display the tolerances used in the toolpath

3 Auto Rebuild – if selected this option will automatically rebuild the toolpath as soon as

you select ok to the operations parameters dialog box

4 Create Custom operation – this option will allow you to save all of the operation

parameters you have defined as an external file without any of the tool information

5 Load Custom operation – this will allow you to load the “snapshot” file as explained

above

6 Save defaults – this option will save the parameters as they stand as default

7 Compass settings – this option will allow you to access all of the variables that can be

used with the compass technology

Use the following parameters in the pocketing

Select ok to the dialog box

The toolpath should now have been built with

the parameters that you have defined

We can now simulate the toolpath with the

Toolpath Laboratory option

Right hand click on the Pocketing Spiral

operation and scroll down the option list and

select on the Toolpath laboratory option

1 2 3 4 5 6 7

The system will now open the new Toolpath Laboratory dialog box From inside of here it is possible to simulate the toolpath, view the type of geometry that makes up the toolpath, view the speeds and feeds at specific points on the toolpath or at a given level

1 Play – This icon will start the simulation

2 Move point backward – This option will allow you to step back through the toolpath

points

3 Move point forward – This option will allow you to step forward through the toolpath

points

4 Stop Simulation – This icon will stop the simulation

5 Level Backwards – This icon will allow you to step backwards through the toolpath level

6 Level Forwards - This icon will allow you to step forwards through the toolpath level

7 (See bellow) (7a)

8 Simulation Speed – This slider bar will allow you to speed up or slow down the

simulation

9 Invert direction – This is icon will reverse the toolpath direction for the simulation only

10 (See bellow) (10a)

4 5

6 7

8

9

10.

11

1 No criteria – this option will remove any visualisation option that has been set

2 By element type – this option will show the type of elements that make up the toolpath

e.g segments, arcs, and helixes in a colour band option

3 Same Feed – this option will colour band the toolpath relating to different speeds and

feeds across it

4 Show points – this option will show the physical toolpath points

5 Show Rapids – this option if enabled will show the rapid movements on the toolpath

6 Show links – this option will show all linking moves in the toolpath

7 Show normals – this option will show the toolpath normal points

8 Show helixes – This option will show all helixes in the toolpath

9 Set Colours – this option will allow you to control all of the colours that’s are used for all

of the banding options, feed rate ranges, etc

10 Show diameter compensation – this option will add the cutter compensation to the

simulation if it has been added in the operation parameters

11 Set tool transparency – this option will control the toolpath transparency of the tool

and the holder itself when the transparent shading is enabled

1 Edit entry/exit – this option will allow you to edit the entry and exit plane Z height

2 Sub path trimming – this option will allow you to delete levels of the toolpath

3 Tool path trimming – this option will allow you to trim an area of a toolpath back to a

profile

4 Edit toolpath – this option will allow you to edit or delete a specific point on a toolpath

5 Move tool on point – this option will allow you to move the tool to a specific point on the

toolpath and also see the XYZ position and speed and feed at that specific point

6 Draw modality – this option will display all of the parameters as explained above

7 Show Links – this option if enabled will show the linking movements of the toolpath

Ensure the Model is shaded, highlight the pocketing Spiral operation from the operations page and select the play icon to begin the simulation

N.B it is possible to simply select an individual level of the toolpath and start the simulation from this level rather then starting from the very beginning

Once the simulation has been run, Close the Toolpath laboratory

We have now successfully defined a closed pocket, we will now define an open pocket and also look at modifying the start and end points of the toolpath

1

3 4

5 6 2

7

Machining an Open Pocket

Move back into the features page of the CAM Navigator

Right hand click on the Model Manager and select the option Add Manual Feature

Ensure the face icon is selected and select the face as shown bellow

Select OK to the features dialog box to confirm the face selection

The system will once again open the Feature Parameters dialog box

Select this face

As you will see, the system will automatically detect the depth of the pocket and also that the pocket is open

Select OK to this dialog box

You will now see that the open pocket has been added to the Model Manager page

Even though the pocket is open it is possible to modify the geometry in order to close the open sides and convert this into a pocket if needed

Right hand click on the Open Pocket feature and select Properties

The system will now open the Geometry Features dialog box This dialog box will show all

of the geometrical information about the feature that has been picked It will also contain vital information about compass(*) settings and machining cycle that is being used for this particular feature

(*) Please ask your instructor for an explanation of compass options

From the geometry features dialog box select the Edit Open/Closed Sides icon

The system will now open the Edit geometry dialog box

Inside of this dialog box, it is possible to see what

elements are set to be open and what elements are set to

be closed By default the system will always split the

longest element or open side into two segments, this is

used by the system to define the start and end point for

machining The system will also display closed elements

in orange and open elements in green

If you right hand click on a item from the list it is possible

to change an open element to be closed

Cancel the Edit geometry dialog box without making any changes to the element status

and return back to the CAM navigator

The next step is to create a roughing and finishing toolpath on the open pocket

As we did before, select the open pocket from the Model manager tree, and right hand click and select and Add operation

Select the Pocketing operation and select OK

The system will now open the tool selection dialog box

This time we will pick a tool from the Visi tools database

Select the Add tool from DB icon

The system will display all tool from the VISI tools database To make selection of the correct tool easier we can use the filter options at the top of the dialog box

Change the filter drop down boxes at the top of the dialog box to be the same as the ones shown bellow

Select the following tool and select Ok

The system will now build the toolpath

We can now add some toolpath parameters

From inside of the operation page, right hand click on the second pocketing spiral

operations and select properties (or alternatively double click on the second toolpath

operation)

Add a Value of 1mm for Side and Bottom Allowance and select OK

With the roughing cut now taken on the pocket we can add a finishing cleaning pass on the pocket

Once again right hand click on the open pocket feature from the model manager tree, and select Add Operation

This time we will add a Milling operation to the pocket

From the Global Tooling database select the following tool and select OK

Your Operations tree should now look like so:

We will now add some entry and exit parameters for our toolpath Open the toolpath

parameters,

Side allowance – Stock to be retained on the side of the part

Bottom allowance – Stock to be retained on the bottom of the pocket

Stepover – This is the Value or percentage that the toolpath will stepover

Number of passes – this option will allow you to add extra passes for roughing if needed Round corners – this option will remove sharp corners and replace these with arcs

Zigzag Mode – if the passes are greater then 1, the system will allow you to apply ZigZag

machining between the passes

Max Stepdown – this value define the maximum stepdown between passes

Last Stepdown – this option will allow you to specify a stepdown value to clear up the

bottom of the feature

Generate Left overs – this option will create profiles in the areas that could not be

machined with the defined cutter

Overlap Method – these 3 options will allow you to machine past the start and end point

by a given amount in different styles to remove any possible cusps that might have been created when leading in and out of the model

Length – this is the amount extra length you wish to apply to the toolpath

Toolpath Offset – this option will control if the tool is offset from the profile in anyway Diameter Compensation – this option will allow you to turn diameter comp on and off

Transition Method – this option determines how the tool moves from one area of passes

to another

Rapid Distance – this Z value is the level in which the tool will go to before returning to the

machining level

Return between Levels – if this option is ticked, the tool will return to the clearance plane

after every level

Clearance plane – this value is the Z value when the tool is moving from one area to

Leadin Method – This option will define how the tool will approach the feature e.g circular,

perpendicular, Helicoidal, and direct

Axis movement method – the will define the method and direction in which the tool

moves from one pass to the next e.g 3D move in XYZ or simply XY-Z

Entry angle – this is the angle in which the cutter will approach the feature

Distance – this is the distance the cutter feed into the feature

Radius – this will define the radius of the entry arc if the leadin method is set to circular or

helical

Leadout Method – This option will define how the tool will “roll off” the feature e.g circular,

perpendicular, Helicoidal, and direct

Axis movement method – the will define the method and direction in which the tool

moves from one pass to the next e.g 3D move in XYZ or simply XY-Z

Exit angle - this is the angle in which the cutter will approach the feature

Distance - this is the distance the cutter feed out when leaving the feature

Radius – this will define the radius of the exit arc if the leadout method is set to circular or

helical

Maximum absolute Z – This option will allow you to change the machining Z top according

to an absolute Value

Minimum absolute Z - This option will allow you to change the machining Z bottom

according to an absolute Value

Max/min feature depth – This value define the depth of the feature

Max feature Z / extra Z+ - this option will allow you to add extra stock to the top of the

pocket

Min feature Z / extra Z- - this option will raise the base of the pocket if a plus value is

entered and lower the base if a minus value is entered

Min side / bottom radius –

Set the following parameters in the operation parameters dialog box

With the parameters now confirmed select OK to the dialog box

The toolpath should now be built to reflect the changes that have been made

With the toolpath now complete we now need to adjust the current feeds and speeds that have been already set

Right hand click on the Milling operation and select Edit cutting conditions

Using this dialog box it is possible to define all of the speeds and feeds, coolant to be used etc

Please change the speeds and feeds to be the same as the ones bellow and select ok

We have now machined an open and closed pocket, used pocketing and milling operations, used existing tools from the library and also selected a tool from the VISI tools database the next step is to look at face milling and creating our own tool manually

We now need to create a profile feature of the outer shape of the model in order to facemill the part successfully

From the menu select Wireframe > Profile > Profile from face

N.B Use the Select visible entities command to help with the selection

Ensure the face icon is selected and pick the bottom face of the model as shown

Confirm the profile default attributes

We now need to add profile CAM attributes to the profile that we have just created

From the menu select Machining > Profile CAM attributes

The system will now ask you to select the profile

Select the profile The system will now ask you to

define the material side Using the spacebar

toggle the arrow so that it is pointing inwards

towards the model

Confirm the direction with M2

The system will now display the Z height of the profile

We now need to enter the Z value for the top of the model, this will then move the profile up

to this Z height and graphically show the pocket

The best way to do this is to use the point selection icons from the left hand side of the screen

Highlight the Z top value 230 and select the icon Point in Z and select the top point as shown bellow

Length of a Segment\Arc Distance from Origin

Point in Y Distance between point to point

Between 2 points in Y Between 2 points in Z

Between 2 points in X Point in Z

Point in X Angle of two elements

The Z value should now be Z 286 and select OK

You should now see the top of the profile has been moved to the corresponding Z value and the graphical representation of the pocket

With the pocket now defined we can facemill the model

Re-open the CAM navigator

You will now notice that in the Model manager tree, an extra directory has been created If the system finds any 2D profiles with CAM attributes assigned to them, they will

automatically be added to a CAM repository folder

When dealing with 2D profiles it is possible to convert them into manual features This gives the added benefit of being able to use the compass technology (*) and also greater information about the feature itself e.g Volume, height

Expand out the CAM Repository folder and right hand click on the profile itself

From the menu select Add Manual feature

The system will now convert the 2D profile into a manual feature

With the feature now defined we can now add the toolpath that we require

Right hand click on the toolpath and select Add operation

Once again we will use the pocketing operation in order to facemill the feature Please note that we can only facemill the feature if it is defined as a Boss

From the toolpath selection dialog box, select the pocketing operation

The system should now open the tool crib dialog box Instead of

Selecting a tool from the crib or the Visi tools database, this time we will create a new tool from scratch

Select the Add tool manually icon

From inside this dialog box we can define all of the tool parameters that we will need Change the manual tool dialog box to be the same as the one bellow

Once the dialog box matches the one above, select OK

You will now see the tool you have defined in the tool crib If you wish to add a tool to the tool crib please ask you instructor to show you how to achieve this

Select the tool again from the tool crib and select OK

The toolpath will now be built

With the toolpath now complete we forgot to add something to the tool when we were making it….a toolholder

Right handclick on the pocketing toolpath, and select Edit tool

At this point If needed we could change the current tool that is being used for the toolpath but what we are going to do is to add a toolholder to the tool

Select the edit tool holder icon

1 Assembly Description – This text box is the description of the assembly

2 Holder Database – this icon will allow you to pick a pre defined toolholder

3 Holder Extension Database - this icon will allow you to pick a pre defined extension

4 Holder Adaptor Database - this icon will allow you to pick a pre defined adaptor

5 Edit – This icon will allow you to edit a defined holder, extension or adaptor

6 Load Assembly – This icon will allow you to load a full assembly

7 Remove Assembly Component –This option will allow you to remove a holder

component

8 Remove all Components – this icon will remove any and all defined holder components

9 Max diameter – This value shows the maximum extreme size of the tool holder

10 Gouge Length – This value defines the distance that the tool protrude from the

machine head

11 Compute Presetting – allows you to calculate the required tool length

12 Overhang – this value you allows you to define the distance the holder protrudes from

the machine tool head

13 Presetting length - is to calculate the ideal length of tool required for currently applied

toolpath

14 Description – this window will display a list of the holder components

15 Graphic Window – this window will dynamically show you a preview of the holder and

The system will now open a new dialog box and display all of the default holders

Select the ISO 40 holder and select OK

The holder will now be added to the description list and you will now also see the preview

of the holder

Add an Assembly Description called “Holder1” and select ok to the holder dialog box

N.B Please note that you might need to move the gauge line to the correct position before simulating – please ask your instructor to explain this

Re-confirm the tool parameters to take you to the main CAM navigator window

If you wish, run the toolpath laboratory in order to simulate the toolpath with the new tool holder

We will now look at the other 2.5D machining strategy’s that are also available

Open the file ‘Profile and section2.wkf’

The file will consists of one ‘closed’ shape profile and one ‘open’ section profile which will define the 2.5D shape

N.B No profile CAM attributes have to be defined for this operation

Open the cam navigation

As you will see the Model manager tree will be empty, this is because the profiles

themselves do not have any CAM attributes assigned to them As there are no profiles added to the model manager tree we cannot add an operation in the same fashion as we have done previously

To add and operation we must do this directly from the project itself

Open the Operations page of the CAM Navigator

As you will see, we have already got a project defined

Right hand click on the Project itself and select Add operation

The system will now open the toolpath selection dialog box

As you will see, 90% of the toolpaths strategies are missing from the 2.5ax Operations section This is because we do not have any features or profiles with CAM attributes

defined This dialog box is contextual sensitive and as such will filter out any toolpath that cannot be used on the corresponding geometry

We do however have the option that we need to use “Profile & Section” Select this

strategy and select ok

Please select the 6mm Ball nose tool from the crib and select ok

The system will now prompt for the geometry to be selected Use the Select All icon

to pick the geometry

The system will now display the selected geometry dialog box

You will notice that only one profile has been added to the list, this is because it is the profile that is lying on the XY plane Select ok to the dialog box

N.B If you right hand click on the Profile from with in the Selected geometry dialog box, it is possible to modify the Start and End Machining point, cut direction, section profile, and section direction

The toolpath will now have been built but we must first change some toolpath parameters