5. Contents
5
Contents
1. General
1.1 New User Interface for Operations 12
1.2 Support of the 3D Connexion SpaceNavigator 13
1.3 Operation summary in SolidCAM Manager 14
1.4 Summarizing the part data in the tool sheet documentation 15
1.4.1 Definition of tool sheet parameters 15
1.4.2 The output PDF file 16
1.5 Opening of PRT files by double-clicking 18
1.6 3D geometry selection 19
1.7 Templates 20
1.7.1 Operation Template 20
1.7.2 Process template 26
1.7.3 Manage Operation/Process Templates 29
1.7.4 Defaults & Settings 32
1.8 Defining Transform position by picking on the model 36
1.9 Automatic synchronization and calculation 37
1.10 Changing the tool and tool data directly from SolidCAM Manager 39
1.10.1 Changing tool 39
1.10.2 Changing tool data 40
1.11 Support of SolidWorks 64-bit 41
2. Geometry
2.1 Closing geometry chains by extending chain entities 44
2.2 Geometry modification for specific operation 46
2.3 Automatic closing of open geometries for Pocket operations 52
2.4 Synchronization when design model configuration changes 53
2.5 Changing the sequence of drill positions 56
6. 6
3. Tools
3.1 End Mill / Bull nose mill / Ball nose mill 59
3.1.1 End mill 59
3.1.2 Bull nose mill 60
3.1.3 Ball nose mill 60
3.2 Drill tool 62
3.3 Bore tool 63
3.4 Center drill tool 64
3.5 Chamfer drill 66
3.6 Dove tail mill 67
3.7 Taper tool 68
3.8 Engraving tool 71
3.9 Face Mill tool 72
3.10 Lollipop mill 73
3.11 Reamer tool 74
3.12 Slot tool 75
3.13 Spot Drill 76
3.14 Tap tool 77
3.15 Thread Tool 78
3.16 Taper Thread Tool 79
3.17 Choosing the tool type 80
3.18 Tool Units 81
3.19 Angular dimensions 83
3.20 Rough tools 84
3.21 Link to the Vardex software for thread milling tool selection 86
4. Milling
4.1 3D Depth type in Profile Milling 88
4.2 Contour 3D operation 90
7. Contents
7
4.3 T-Slot operation 93
4.3.1 Second offset number 93
4.3.2 Technological parameters 94
4.4 Face Milling Operation 96
4.5 Vertical zigzag passes in Profile operation 104
4.6 Equal step down in Profile and Pocket operations 106
4.7 Final cuts machining in Profile and Pocket operations 108
4.8 Wall Draft angle in Profile and Pocket operations 110
4.9 Profile floor machining 112
4.10 Pocket Wall finishing 114
4.11 Open Pocket machining 115
4.11.1 Open Pocket Geometry definition 115
4.11.2 Open pocket machining parameters 116
4.12 Adjacent tool paths connection in Profile operations 119
4.13 Complete Z-level in Pocket operations 121
4.14 Movements between cutting passes 122
4.15 Minimal machined area in Floor Constant Z machining 123
5. Automatic Feature Recognition and Machining (AFRM)
5.1 Drill Recognition operation 126
5.1.1 Geometry definition 127
5.1.2 Drill Depth definition 133
5.1.3 Technological parameters 138
5.2 Pocket Recognition operation 139
5.2.1 Geometry definition 139
5.2.2 Geometry modification 146
5.2.3 Milling Levels 148
5.2.4 Technological parameters 149
5.3 Using color information in AFRM 150
5.4 Dividing deep holes for machining from both sides 152
9. Contents
9
8.2.3 Part Settings 229
8.3 Rest Material calculation for Milling Drilling operations 230
8.4 Generation of the Material boundary solid 231
8.5 Tool direction and imaginary tool nose 232
8.6 TX/TZ parameters for Machine Simulation 235
8.7 Clamp and Material boundary synchronization 236
8.8 Envelope calculation enhancements 238
8.9 Turning geometry definition by picking model entities 239
8.9.1 Associativity and Geometry Synchronization 242
8.10 Rough turning at angle 243
9. Mill-Turn
9.1 CAM-Part definition 247
9.1.1 CNC-controller definition 247
9.1.2 Coordinate System definition 248
9.1.3 Stock and Machining boundary 251
9.1.4 Clamp definition 251
9.1.5 Target definition 251
9.2 Existing CAM-Parts conversion 252
9.3 Additional Turning Coordinate Systems 254
9.4 Pre-processor customization 257
9.5 Post-processor customization 258
9.5.1 Milling post-processor adaptation 258
9.5.2 Turning post-processor adaptation 259
9.5.3 Turn-Mill post-processor adaptation 261
9.6 Geometry wrapped around axes for 4-axis machining 263
10. Wire Cut
10.1 Improvements of the 4-axis Geometry definition 266
10.2 Sharp corner machining in Profile and Angle operations 271
10. 10
11. Simulation
11.1 SolidVerify support in Machine Simulation 274
11.2 Machine Simulation for Turning, Turn-Mill and Mill-Turn 275
11.3 Fixtures support within Machine Simulation 276
11.4 Solving self-intersections and noise problems in solid verification 278
11.4.1 Checking and fixing self-intersections 278
11.4.2 Rounding of input data 279
11.5 Improving the simulation performance in the SolidVerify mode 280
12. 12
New User Interface for Operations1.1
SolidCAM2008 R12 offers you a new enhanced interface for milling and turning
operations.
In the new interface the single-page dialog box of the previous interface is divided
into a number of pages, each handling a specific set of parameters (e.g. Geometry,
Tool, Levels, Technology, etc.). The list on the left side of the dialog box enables you to
switch between the different parameters pages.
You may switch between the new and the
previous single-page interface by using the
User Interface page of the SolidCAM Settings
dialog box. To work with the single-page
interface, choose Single-Dialog. To switch
to the multi-page interface, choose Multi-
dialog. In this mode, you may also set a
keyboard shortcut for switching between
pages in the multi-page dialog box; click
on the Switch Items Hotkey box and press a
required key or a combination of keys you
want to use as hotkeys for switching.
Technology
Geometry parameters
Parameter illustration
Parameters page
Info
Tool parameters
Machining levels
parameters
Link parameters
Operation name
Operation buttons
Template
Technological parameters
Miscellaneous parameters
13. 1.General
13
Support of the 3D Connexion SpaceNavigator1.2
SolidCAM2008 R12 provides you with the support of SpaceNavigator 3D mouse by
3Dconnexion (www.3dconnexion.com).
This device enables you to rotate, pan and zoom the CAD model during all the stages of
the CAM-Part definition. Using the SpaceNavigator enables you to significantly speed
up the geometry definition process and simplifies the model and tool path viewing
during such simulation modes as: HostCAD, Rest Material, SolidVerify, RapidVerify
and Machine Simulation.
14. 14
Operation summary in SolidCAM Manager1.3
SolidCAM2008 R12 provides you with the possibility to
obtain the summary of a specific operation directly
from the SolidCAM Manager, without opening of the
operation.
The Info command located in the right-click menu,
available on a specific operation in the SolidCAM
Manager, displays the Info dialog box.
This dialog box displays the summary information of the selected operation: Tool
information (diameter, corner radius, taper angle and lengths); Operation Tool data (feeds
and spin) and Levels (Upper level, Depth and Step down).
The icon located in the title bar enables you to pin/unpin the Info
dialog box.
15. 1.General
15
Summarizing the part data in the tool sheet documentation1.4
SolidCAM2008 R12 provides you with an advanced option to summarize the CAM-Part
information by generating a tool sheet documentation in PDF format.
Definition of tool sheet parameters1.4.1
The Tool Sheet command is available for the
complete CAM-Part (in the right-click menu
available on the CAM-Part header) or for separate
operations (in the right-click menu available on the
operations). The Tool Sheet Extra Parameters dialog
box is displayed. This dialog box enables you to
manage the content of the documentation PDF
file.
In this dialog box, you can attach a logo file (in BMP format) to your tool sheet, define
your own variables and values that will be inserted into the tool sheet, add comments
and notes relative to your part, and decide whether you need the full version of the
information sheet or only particular sections, such as Operations summary or Tool
Table.
The Show Last Tool Sheet command enables you to display the last generated tool sheet
for the current part, instead of generating it anew. The Tool Sheet Extra Parameters
dialog box is displayed so that you can define which sections of the last tool sheet you
want to display.
16. 16
The output PDF file1.4.2
The output PDF file consists of the following sections:
Main page
This section summarizes general information about the CAM-Part, including its picture
and the comments and notes you have added.
Tool table
This section displays the list of the tools used for
the operations of the current CAM-Part, with their
parameters and illustrations.
Part picture
Part notes
Company logo
Part definition
Part properties
Comment entered
in the Parameters field Part name
17. 1.General
17
Operations summary
This section summarizes the operations defined for the current CAM-Part.
Fixtures
This section shows how the part must be fixed on
the CNC machine table.
18. 18
Opening of PRT files by double-clicking1.5
In the previous versions of SolidCAM, it was only possible to open a PRT file by using
the SolidCAM submenu in the main menu of SolidWorks, i.e. to open a CAM-Part file,
you needed to load SolidWorks, click SolidCAM, Open, and then choose the required
file from the CAM-Parts browser. SolidCAM2008 R12 provides you with a time-saving
possibility to open a PRT file by double-clicking on the file name in any location where
it is saved.
19. 1.General
19
3D geometry selection1.6
In previous SolidCAM versions the Select/Unselect radio button was used in dialog
boxes for 3D geometry selection (solids, surfaces and faces). This radio button switches
the system between selection and unselection modes.
SolidCAM2008 R12 provides you with an improvement
of the selection/unselection of the 3D geometry.
This improvement is based on automatic toggling
between modes: a click on the model entity selects
it, while the next click on the selected entity clears
the selection.
The Select/Unselect radio buttons are therefore
removed from the relevant dialog boxes (3D Geometry
dialog box, 3D Box dialog box, Select faces dialog box
etc.)
20. 20
Templates1.7
SolidCAM2008 R12 provides you with the functionality of templates that is useful for
simplifying the repetitive tasks in the CNC programming. SolidCAM enables you to
save the operation data as a template and load it into a new operation of the same type.
SolidCAM enables you also to specify the default operation template that is used for
each newly created operation of the appropriate type.
SolidCAM enables you also to define and use a Process Template, which is a template
of a series of operations that executes a specific machining task.
Operation Template1.7.1
SolidCAM enables you to create an operation template by saving an already defined
operation. The saved template can be later used for a new operation definition. The
saved template data does not include the geometry which must be defined after loading
the template. The saved template can optionally include the tool data.
The Template section is added into each SolidCAM Operation dialog box. This section
provides you with the following functionality:
21. 1.General
21
Save Template
The button enables you to save all the
data (except the geometry) of the current
operation as a template.
The Template Manager dialog box is displayed.
This dialog box enables you to choose the
name for saving the template. The template
is saved in the location defined by the
SolidCAM Templates Directory parameter in
the Part Settings dialog box (see topic 1.7.4).
The Operation Templates table displays all the
Operation Templates located in the SolidCAM
Templates Directory and their types.
The Include tool data check box enables you to include the tool data in the saved
template.
Type the name in the Template edit box and click on the OK button to confirm. If
a template with the defined name already exists in the current location, SolidCAM
displays the following warning message:
When you confirm this warning by the Yes button, SolidCAM overwrites the existing
template with the new one. When you press the No button, the Template Manager dialog
box is activated again providing you with the possibility to choose a different name for
the template.
22. 22
SolidCAM enables you also to save
an existing operation as Operation
Template from the SolidCAM
Manager, using the Create Template
command from the right-click menu
available on single operations.
This command displays the Template
Manager dialog box which enables
you to save the template data as
described earlier.
23. 1.General
23
Load Template
The button enables you to load a specific
template into the current operation. The
Template Manager dialog box is displayed.
This dialog box offers you the templates
located in the SolidCAM Templates Directory
determined by Part Settings (see topic 1.7.4).
The Template Manager dialog box displays
only the templates whose type is suitable for
the current operation.
Choose the necessary template and click on the OK button to confirm the operation.
When the template is loaded, all the current operation data are substituted with the
data from the template.
When a template is loaded into the operation, its name is
displayed in the edit box in the Templates section. A tool tip
message is available when you place the mouse cursor over
the edit box; the tool tip message displays the full name of
the loaded template.
When any of the operation data is modified after a template
is loaded, the template name in the edit box is marked by an
asterisk sign (*).
24. 24
SolidCAM enables you also to create a
new operation from an existing template,
directly from the SolidCAM Manager using
the Add Operation from Template command
from the right-click menu available
on the operations header or on single
operations.
This command displays the Template
Manager dialog box which enables you to
choose an existing template as described
earlier. In this case the Template Manager
dialog box displays all the templates
existingintheSolidCAMTemplatesDirectory
regardless of its type.
When the dialog box is confirmed by the
OK button, SolidCAM inserts the chosen
Operation Template into the SolidCAM
Manager tree.
The inserted operation is incomplete since
the operation has no defined geometry
and no tool (if the initial Operation
Template used for the operation creation
had no tool). The incomplete operations
are marked with red color.
Since the incomplete operation has
no geometry, its tool path cannot be
generated. In order to completely define
the operation, you have to define its
machining geometry and tool (if necessary).
During the creation of a new operation from an Operation Template, SolidCAM
assigns the Machine Coordinate System #1 (Position #1) for the newly created operation.
During the operation editing this Coordinate System can be changed.
25. 1.General
25
Tool search
When an operation template is loaded, SolidCAM checks the existence of the tool data
in the template; if the tool data was saved in the operation template, the tool search is
performed according to the following rules:
• When the operation template uses a tool defined as Permanent, the tool search
for this tool is performed using the tool number only. At the first stage, the
tool search is performed in the Part Tool table. If the tool with the defined
number is not found in the Part Tool Table, SolidCAM performs an additional
search in the Current Tool Table. If a tool with the defined tool number is
found in the Current Tool Table, it is copied into the Part Tool Table and chosen
for the operation. If the tool is not found in the Current Tool Table, SolidCAM
displays the following error message:
When you confirm this message with the OK button, SolidCAM returns you
to the operation dialog box in order to define a tool.
• When the tool in the operation template is not defined as Permanent,
SolidCAM performs the tool search using the tool parameters. The tool
parameters used for the tool search are defined in the SolidCAM Settings in
the Tool search page. The tool search is performed in the Part Tool table. If
a tool with the same definition as in template is not found in the Part Tool
Table, SolidCAM performs an additional search in the Current Tool Table. If a
suitable tool is found in the Current Tool Table, it is copied into the Part Tool
Table and chosen for the operation. If a tool is not found in the Current Tool
Table, a new tool with the parameters defined in the template is created in
the Part Tool Table. SolidCAM automatically assigns the first not used tool
number for the new created tool.
When you load a template containing tool data into an operation that already
has a defined tool, SolidCAM displays the following message:
When you confirm this message, SolidCAM replaces the tool already defined
in the operation with the tool defined according to the template.
26. 26
Process template1.7.2
SolidCAM2008 R12 enables you to define and use a Process Template, which is a template
of a series of operations that executes a specific machining task. Such capability enables
you to store a complete sequence of operations as a Process template and apply it for
the machining of similar cases.
Define Process Template
To create a Process Template, select in the
SolidCAM Manager all the operations intended
to be included in the Process Template and
choose the Create Template command from
the right-click menu available on single
operations.
This command displays the Template Manager
dialog box which enables you to save the
chosen operations as a Process Template.
ThisdialogboxdisplaysalltheexistingProcess
Templates in the SolidCAM Templates
Directory; the Process Templates names are
listed in the Template Folders section under
the Process Templates header. The sequence
of operations comprising the template is
displayed in the Operation Templates table.
27. 1.General
27
The Include tool data check box enables you to include the tool data into the saved
Process Template.
To save the selected operations as a new Process Template, type the name in the
Process Template edit box and click on the OK button to confirm the operation. If
a Process Template with the defined name already exists in the current location,
SolidCAM displays the following warning message:
When you confirm this warning by the Yes button, SolidCAM overwrites the existing
Process Template with the new one. When you press the No button, the Template
Manager dialog box is activated again providing you with the possibility to choose a
different name for the Process Template.
The Template Manager dialog box
provides you with the capability to
create an empty Process Template
and copy to it a number of Operation
Templates from different Process
Templates. See topic 1.7.3 for more
details.
Use Process Templates
SolidCAM enables you to insert the Operations
Templates contained in a Process Template
into a CAM-Part, converting them into regular
SolidCAM Operations. To insert a Process
Template into the CAM-Part choose the Add
Process Template command from the right-click
menu available on operations header or single
operations in the SolidCAM Manager.
28. 28
This command displays the Template Manager dialog box which enables you to choose
an existing Process Template to be inserted.
During creation of a new operation from the Process Template, SolidCAM displays
the CoordSys selection dialog box, which enables you to choose the Coordinate System
to be used in the created operations.
The inserted operations are incomplete; this means that the operations have no defined
geometry and no tool (if the initial Operation Template used for the operation creation
had no tool). The incomplete operations are marked with red color.
Since the incomplete operations have no geometry, their tool path cannot be generated.
In order to completely define the operation, you have to define the machining geometry
and tool (if necessary) for each operation.
29. 1.General
29
1.7.3 Manage Operation/Process Templates
The Manage Templates command located in the SolidCAM
menu enables you to manage your Operation Templates and
Process Templates using the Templates Manager dialog box.
The Templates Folders section contains Templates and Process Templates.
When the Templates header is selected, all the Operation Templates located in the
SolidCAM Templates Directory are displayed in the Operation Templates table.
All the Process Templates located in the SolidCAM Templates Directory are listed under
the Process Templates header. When a Process Template is selected, all the Operation
Templates included into this process are displayed in the Operation Templates table.
30. 30
SolidCAM enables you to manage
the Process Templates with the
right-click menu which is available
on the Process Templates header or
single Process Templates. This menu
provides you with the following
commands:
• New Process Template. This
command enables you to
create a new empty Process
Template.
• Rename. This command
enables you to rename an
existing Process Templates.
• Delete. This command enables you to delete an existing Process Template.
SolidCAM enables you to manage Operation Templates with the right-click menu
which is available on the Operation Templates in the Operation Template table. This
menu is available for the standalone Operation Templates located in the SolidCAM
Templates Directory and for Operation Templates included into Process Templates.
31. 1.General
31
The menu provides you with the following commands:
• Create Process Template. This command enables you to create a new Process
Templates; the current Operation Template is added to this process.
• Copy. This command enables you to copy the current Operation Template
into the clipboard.
• Paste. This command enables you to paste the Operation Template from the
clipboard. TheOperation Templateisinsertedintothechosenlocation(either
into the active Process Template or as a standalone Operation Template into
the SolidCAM Templates Directory).
• Edit. This command enables you to load the chosen Operation Template
for editing. When a template is loaded, SolidCAM displays an appropriate
operations dialog box with the template data.
SolidCAM enables you to edit all the parameters and options of the template,
except the geometry and coordinate system.
The button enables you to save the template data using the Save template
dialog box.
• Delete. This command enables you to delete the active Operation template.
32. 32
1.7.4 Defaults & Settings
SolidCAM Settings
The Templates and Defaults page is added to the SolidCAM Settings dialog box.
Thispageenablesyoudefinethedefaultlocationof theOperationTemplates/Template
Groups and to specify the default templates that are used for each new operation.
SolidCAM Template Directory
The SolidCAM Template Directory section enables you to define the default
location for SolidCAM Operation Templates/Template Groups. You can
define the path by typing it in the combo-box or by using the Browse
button. In case the chosen folder does not exist, SolidCAM displays the
following message:
• The Create button enables you to create the folder with the
specified location and set it as the SolidCAM Template directory.
33. 1.General
33
• The Browse button displays the browser dialog box that enables
you to choose another location for the SolidCAM Templates
directory.
By default, the Templates directory location is ..TablesMetricTemplates for
Metric units and ..TablesInchTemplates for Inch units.
Operation default templates
The Operation default templates section enables you to assign default
templates for operations.
The templates are divided between four tabs:
• The 2.5D Milling tab contains the 2.5D milling operations.
• The 3D Milling tab contains the 3D milling operations.
• The HSM tab contains the HSM operations.
• The Sim. 5-Axis tab contains the Sim. 5-Axis operations.
Each tab contains a table
that enables you to define
the default templates of
each SolidCAM operation.
When the default template
use is activated for a specific
operation, the Template
column enables you to use
the suitable template with
the combo-box. When the
template use is activated for
an operation type, each new
operation of this type will
be started with the data of
the specified template.
34. 34
Templates activation/deactivation
When user deactivates template use for an operation, the Template column
combo-box is disabled.
When you activate template use for an operation type, SolidCAM searches
in the SolidCAM Template Directory for suitable templates of this type. The
combo-box is filled with the names of the found templates; the first of
them is automatically chosen. In case of absence of suitable templates,
SolidCAM deactivates the use of templates for this operation.
Changing SolidCAM Template Directory
When you change a SolidCAM Template Directory, SolidCAM performs a
search for suitable templates for all the operations with the activated default
template use. When a template for some operation is not found, SolidCAM
deactivates the default template use. Found templates are inserted into the
related combo box. The first found template name is displayed.
The templates search is not performed for the operations where
the templates use is deactivated.
Creating templates sets (working style)
Consider a folder containing a set of templates. This set contains only one
template for each specific operation; all the operations are thus covered
by templates. This set is customized for a specific application (e.g. Mold
machining). Consider an additional folder containing a set of templates for
another application.
By switching between these folders for SolidCAM Template Directory,
SolidCAM switches templates for all the operations. This enables you to
quickly choose a templates set for a specific application.
35. 1.General
35
Part Settings
SolidCAM enables you to customize the default and templates settings for a specific
CAM-Part using the Templates and Defaults page of the Part settings dialog box.
During the CAM-Part definition the Part settings for Templates and Defaults are copied
from the SolidCAM Settings.
The behavior of this page is similar to the behavior of the Templates and Defaults page
of the SolidCAM Settings dialog box.
36. 36
Defining Transform position by picking on the model1.8
SolidCAM2008 R12 enables you to define the positions for operations transformation
by picking on the model. This functionality is implemented for Move and Translate by
List options.
When you choose the Move item from the Transform menu in SolidCAM Manager, the
Move Operations dialog box is displayed. This dialog box enables you either to define
the move position by entering the offset values along the axes or to define the move
position by picking on the model.
To define the move position by
picking on the model, activate the
Move Operations dialog box and click
the necessary position on the design
model. The coordinates of the
picked position are displayed in the
offsets edit boxes.
The picked positions are not associative to the solid model.
The behavior of the
Translation list dialog box
is similar; the coordinates
of the picked position are
displayed in the Offsets value
edit box. The Enter button
enables you to confirm the
picked position and includes
it into the positions list.
The picked positions are not associative to the solid model.
37. 1.General
37
Automatic synchronization and calculation1.9
In previous versions, SolidCAM provided you with the possibility to automatically
perform the synchronization check. During this check the unsynchronized geometries
and operations based on them are detected. SolidCAM2008 R12 provides the additional
capability to perform the synchronization and tool path calculation automatically for
detected unsynchronized operations.
The Synchronization page of the SolidCAM Settings dialog box has two new options. The
Automatically synchronize geometries and Calculate operations after the synchronization
options are added under the Check synchronization always option (this option enables
you to perform the synchronization check automatically).
38. 38
Automatically synchronize geometries
The Automatically synchronize geometries option enables SolidCAM to perform the
geometries synchronization automatically.
This option is enabled only when the Check synchronization always option
is chosen.
When the Automatically synchronize geometries option is activated, SolidCAM performs
the synchronization check and then automatically synchronizes all the unsynchronized
operations and geometries. When the synchronization fails for certain operations or
geometries, SolidCAM marks the operations/geometries with an exclamation mark
and deletes the operations tool paths; such operations are marked with the asterisk.
Calculate operations after the synchronization
The Calculate operations after the synchronization option enables you to automatically
perform the calculation of the synchronized operations.
This options is enabled only when the Automatically synchronize geometries
option is activated.
When the Calculate operations after the synchronization option is activated, SolidCAM
automatically calculates all the synchronized operations; the operations marked with
the exclamation mark are not calculated.
39. 1.General
39
Changing the tool and tool data directly from SolidCAM Manager1.10
Changing tool1.10.1
In previous SolidCAM releases, changing the tool for
a particular operation could be performed only via
the operation dialog box. SolidCAM2008 R12 enables
you to change tools directly from SolidCAM Manager.
The Change Tool option is added into the right-click
menu available on the operation entries in the tree.
This option displays the Tool dialog box that contains
the parameters of the current tool and enables you
to choose another tool for the operation.
40. 40
Changing tool data1.10.2
In previous SolidCAM versions, the data of
the tool used in a particular operation could
be edited only via the operation dialog box.
SolidCAM2008 R12 enables you to change the
tool data directly from SolidCAM Manager.
The Change Tool data option is added into the
right-click menu available on the operation
entries in the tree.
This option displays the Operation Tool Data
dialog box that enables you to edit the data
related to the current tool. The All checked
operations as selected one check box enables
you to define the listed tool parameters in all
operations identically to the first operation.
41. 1.General
41
Support of SolidWorks 64-bit1.11
SolidCAM2008 R12 provides you with complete support of the 64-bit version of
SolidWorks working under the Windows XP Professional x64 Edition.
44. 44
Closing geometry chains by extending chain entities2.1
The Curve option commonly used for geometry chains selection enables you to select
a continuous geometry chain by picking its successive entities. During the geometry
definition SolidCAM detects the gaps between selected entities and provides you with
the capability to close them, taking into account the Gap Minimum and Gap Maximum
parameters defined in the SolidCAM Settings.
If the detected gap is smaller than the Gap Minimum tolerance, SolidCAM automatically
closes the gap by extending/shortening chosen entities up to their virtual intersection
point. If the gap is greater than the Gap Minimum tolerance but less than the Gap
Maximum tolerance, SolidCAM displays a prompt message asking you if you want
to close the gap. When you confirm, SolidCAM automatically closes the gap by
extending/shortening chosen entities up to their virtual intersection point; if you
cancel, SolidCAM does not close the gap and unselects the last entity.
When the gap is larger than the Gap Maximum tolerance, SolidCAM does not accept the
chosen entity and displays a warning message.
SolidCAM2008 R12 provides you with the Curve + Close
Corners option of the chain geometry selection. This
option enables you to close the gaps between successive
chain entities irrespective of the Gap Minimum and Gap
Maximum values.
45. 2. Geometry
45
When a gap is detected between two successively selected entities, SolidCAM continues
the chain by virtually extending the selected entities, according to the direction of the
first entity, up to a virtual intersection point between the two entities.
In case several possible intersection points exist, the point closest to the
last vertex of the first selected entity is chosen.
If an intersection point cannot be found by extending
either one or both selected entities, the following message
is displayed.
Splines and arcs are extended by lines tangential to the arc/spline at its end point.
Associativity and synchronization
When the model used for the geometry definition is modified, SolidCAM enables you
to synchronize the geometry with the updated model. During the synchronization
SolidCAM handles the gaps areas (closed using the Curve + Close Corners option) by
regenerating the extension of the chain elements so as to close the gaps.
First selected entity
Next selected entity
46. 46
Geometry modification for specific operation2.2
SolidCAM enablesyoutosharegeometriesbetweenanumberof SolidCAM operations.
SolidCAM2008 R12 provides you with the additional capability to modify a shared
geometry, specifically for each operation; this includes assigning different values to the
geometry Extension, Offset and Define Start. The geometry modification also includes
choosing which geometry chains are active in the operation (in case of multiple chain
geometry). The modification is relevant only for the current operation and does not
affect other operations where the geometry is shared. The geometry modification is
supported for the Profile, T-Slot and Translated Surface operations.
The Geometry button is added to the Modify section of the Technology page of the
operation dialog box.
This button displays the Modify Geometry dialog box. This dialog box
enables you to perform the geometry modification for the current
operation.
Tool side
The Tool side option enables you to define the tool
position relative to the geometry. For more details about
this option, refer to SolidCAM Milling User Guide.
47. 2. Geometry
47
Chains
This section displays the list of all the geometry chains participating in the
current geometry. The check box, located at the side of the geometry chains
in the list, enables you to include/exclude the chain from the geometry of
the current operation.
A right click menu is available on the elements of
the list. This menu enables you to perform the
following actions:
• Check all. This command enables you
to check all the chains.
• Uncheck all. This command enables
you to uncheck all the chains.
• Invert check states. With this command the state of the check
boxes of all the chains will be reversed.
• Reverse. This command enables you to reverse the direction of
the chain.
• Reverse All. This command enables you to reverse the direction
of all the chains.
48. 48
Extension
The Extension section enables you to define the extension for the selected
chain. The Start and End parameters define the start and end extension
lengths. The extension is performed tangentially to the chain entities at the
start and end points of the geometry chain. The start and end elements are
determined according to the chain direction.
When a negative value is defined, SolidCAM shortens the chain by a
distance, measured along the chain elements.
SolidCAM enables you to define the Start and End parameters either by
typing in the values or by picking on the model (when the focus is placed
in the edit box).
The Apply to all button enables you to apply the extension, defined for the
selected chain, for all the chains of the geometry.
Geometry chain
Start extension
End extension
49. 2. Geometry
49
Modify offset
The Modify offset section enables you to define the offset for the selected
chain. Machining is performed at the specified offset.
SolidCAM enables you to define the Modify offset parameter either by
typing in the value or by picking on the model (when the focus is placed
in the edit box).
The Apply to all button enables you to apply the Modify offset, defined for
the selected chain, for all the chains of the geometry.
The direction of the Modify Offset
for the open contours is defined
according to the chain direction.
A positive Modify Offset value
offsets the chain to the right side
(according to the chosen chain
direction). A negative value
offsets the chain to the left side
(according to the chosen chain
direction).
Geometry chain
Modify offset
Modified chain
Positive Offset
Negative Offset
Geometry Chain
50. 50
For closed contours, a positive Modify Offset value offsets the geometry
to the outside; a negative Modify Offset value offsets the geometry to the
inside.
The Take 1/2 from selected offset option enables you to offset the chain by
half of the defined offset value.
In the part shown below the central pads should be machined by a single
straight cutting pass, located at the middle of the pad. After defining the
geometry at the edge of the pad, the geometry is offset using the picked
position at the opposite edge and the Take 1/2 from selected offset option.
Positive Offset
Negative Offset
Geometry Chain
Modified geometry
Geometry
Picked offset position
51. 2. Geometry
51
Define Start
The Define start section enables you to shift the start position of the closed
chains. For open chains, this section is disabled. The shifting of the start
point is defined as a percentage of the chain length. SolidCAM enables
you to define the start position shifting either by typing in the Shift value or
by picking the position on the model.
The Apply to all button enables you to apply the Shift value defined for the
selected chain for all the closed chains of the current geometry.
The Auto next button enables you to define the start points successively,
for all the closed chains, by picking the positions on the model. When this
mode is activated, the first closed chain is highlighted, enabling you to pick
the start position for it. When the position is picked, SolidCAM switches
to the next closed chain and so on. The Resume button enables you to
finish the Auto next definition of the start positions.
The Set default button enables you to return the start position of the
current chain to its initial state. When the Apply to all check box is activated,
the Set default button returns the start positions of all the chains to their
initial state.
52. 52
Automatic closing of open geometries for Pocket operations2.3
SolidCAM2008 R12 provides you with the possibility to automatically close the open
geometry chains for Pocket operations.
When you confirm an open chain definition for a Pocket operation in the Geometry
Edit dialog box with the button, SolidCAM displays the Close Chain message box.
When you confirm this dialog box with the OK button, SolidCAM closes the chain
with a line connecting the start and the end points of the chain. The Mark line as open
edge check box enables you to mark the connecting line as an open edge to perform
Open Pocket machining (see topic 4.11).
When you click on the Cancel button, SolidCAM returns to the geometry definition
and enables you to close the chain manually, by the model element selection.
Selected chain
Connecting line
53. 2. Geometry
53
Synchronization when design model configuration changes2.4
In previous SolidCAM versions, SolidCAM provided you with a constant link between
the geometry and the design model configuration which was used for the geometry
definition (parent configuration). With such a link, switching between configurations of
the design model does not affect the defined geometry; the geometry can be updated
(through synchronization), only in case the parent configuration is modified.
SolidCAM2008 R12 provides you with an additional functionality that enables you to
synchronize the geometry, when the configuration changes; SolidCAM discontinues
the link between the geometry and its parent configuration and establishes a new
link between the geometry and the new current configuration. Such functionality
enables you to automatically update SolidCAM geometries according to the current
configuration of the design model.
This functionality enables you for example to perform, in a single CAM-Part, the
machining of a family of similar parts, based on a single design model and managed by
configurations. The geometries of this CAM-Part are automatically updated for each
current configuration, providing you with an updated tool path.
SolidCAM Settings
The Synchronization when
design model configuration
changes section is added to
the Synchronization page of
the SolidCAM Setting dialog
box. This section enables
you to define SolidCAM
behavior in case when the
configuration is changed.
The SolidCAM Settings are
used as the default for the
Part Settings of each newly
defined CAM-Part.
54. 54
Part Settings
The Synchronization page is added to the Part Settings dialog box. This page enables
you to define SolidCAM behavior in case when the configuration is changed for the
current CAM-Part. The Synchronization when design model configuration changes section
provides you with the following options:
The Keep the geometry associative with the parent configuration option enables you to
keep the link between the geometry and the parent configuration. SolidCAM always
keeps the geometry linked to the parent configuration (the configuration used for the
geometry definition). When you switch between the model configurations, this does
not affect the geometry; synchronization is required only in case when the parent
configuration is changed.
55. 2. Geometry
55
The Associate the geometry with the current configuration option enables you to establish
the link between the geometry and the current configuration and perform the
synchronization according to the current configuration.
After such synchronization the geometry is linked to the current configuration until
you switch to another one.
Geometry
Configuration #1
Geometry
Configuration #2
Geometry
Configuration #1
Geometry
Configuration #2
56. 56
Changing the sequence of drill positions2.5
In previous SolidCAM versions, editing the sequence of drilling positions was possible
only in the operation dialog box. SolidCAM2008 R12 enables you to change the order of
positions in the sequence by dragging and dropping them in the list section of the XY
Drill Geometry Selection dialog box.
59. 3. Tools
59
End Mill / Bull nose mill / Ball nose mill3.1
The End/Rough Mill tool type, used is previous SolidCAM versions, is reclassified into
three separate tool types: End mill, Bull nose mill and Ball nose mill, according to the
Corner radius value.
End mill3.1.1
A tool of this type is defined by the
parameters shown in the image. Note
that the Corner radius parameter, used for
the tool definition in previous versions,
is not used any more for the End Mill tool
definition.
The cylindrical tool arbor is added to
the tool definition. The arbor diameter
and length are defined by: Arbor Diameter
and (Total Length - Shoulder Length). The
Shoulder Length should be greater than or
equal to the Cutting Length, and equal to
or less than the Outside Holder Length.
When a new tool is created, the default value of the Arbor Diameter is equal to the
Diameter value. The default value of the Shoulder Length is equal to the Cutting Length.
Outside
Holder
Length
Cutting
Length
Arbor Diameter
Diameter
Total
length
Shoulder
Length
60. 60
Bull nose mill3.1.2
A tool of this type is defined by the
parameters shown in the image. The
Corner radius of a tool of the Bull nose
mill type should be in the range from 0
to half the Diameter value.
The cylindrical tool arbor is added to
the tool definition, same as for the End
mill tool.
Ball nose mill3.1.3
A tool of this type is defined by the
parameters shown in the image.
The Corner radius of a tool of the Bull
nose mill type is equal to half the Diameter
value and cannot be changed.
The cylindrical tool arbor is added to the
tool definition, same as for the End mill
tool.
Outside
Holder
LengthCutting
Length
Corner Radius
Arbor Diameter
Diameter
Total
Length
Shoulder
Length
Outside
Holder
LengthCutting
Length
Corner Radius
Arbor Diameter
Diameter
Total
Length
Shoulder
Length
61. 3. Tools
61
Tools conversion
SolidCAM automatically converts tools of the End/Rough Mill tool type, created with
previous SolidCAM versions, into one of the three tool types described above. The
tools conversion is performed according to the Corner radius value:
• Tools with zero Corner radius are converted into End mill tool type.
• Tools with Corner radius equal to half the Diameter are converted into Ball
nose mill type.
• Tools with Corner radius in the range from 0 to half the Diameter value are
converted into Bull nose mill type.
When an existing tool (created in a previous SolidCAM version) is converted into
End mill / Bull nose mill / Ball nose mill tool, the value of the Arbor Diameter is defined
as equal to the Diameter. The value of the Shoulder Length is defined as equal to the
Cutting Length.
62. 62
Drill tool3.2
The cylindrical tool arbor is added to
the tool definition. The arbor diameter
and length are defined by: Arbor Diameter
and (Total Length - Shoulder Length). The
Shoulder Length should be greater than or
equal to the Cutting Length, and equal to
or less than the Outside Holder Length.
When a new tool is created, the default
value of the Arbor Diameter is equal to
the Diameter value. The default value of
the Shoulder Length is equal to the Cutting
Length.
During the conversion of tools defined in previous SolidCAM versions, the tool arbor
is added with the following values:
• Arbor Diameter is equal to the Diameter value.
• Shoulder Length is equal to the Cutting Length.
Outside
Holder
Length
Cutting
Length
Diameter
Angle
Total
Length Shoulder
Length
Arbor Diameter
63. 3. Tools
63
Bore tool3.3
SolidCAM2008 R12 provides this
new tool type for boring using
the Drill operations.
The image illustrates the
parameters used for the Bore tool
definition.
Parameter limitations
• Corner Radius should be equal to or less than the Cutting Length.
• Angle should be greater than 0° and less than 90°.
• Cutting Length value should be equal to or less than the Shoulder Length
value.
• Shoulder Length value should be equal to or less than the Outside Holder Length
value.
• Outside Holder Length value should be equal to or less than the Total Length
value.
Outside
Holder
Length
Total
Length
Shoulder
Length
Arbor
Diameter
Diameter
Cutting
Length
Corner Radius
Angle
64. 64
Center drill tool3.4
This new tool type is used for center
drilling in Drill operations.
The image illustrates the parameters
used for the Center drill tool
definition.
When this tool is used in combination with the Use chamfer option,
SolidCAM calculates the drilling depth according to the following
formula:
Drilling depth = Tip length + Arbor Diameter /2 + cotan(Shoulder angle / 2)
Outside
Holder
Length
Tip Diameter Tip
Length
Total
Length
Shoulder
Angle
Cutting
Length
Angle
Arbor
Diameter
Tip Diameter
Chamfer Diameter
Shoulder angle
Arbor diameter
Cutting length
Tip length
Chamfer Diameter
Drilling depth
65. 3. Tools
65
Parameter limitations
• Tip diameter should be less than the Arbor Diameter.
• Tip Angle should be greater than 0° and less than 180°.
• Shoulder Angle should be greater than 0° and less than 180°.
• The length of the conical part defined by Tip diameter and Tip angle should
be equal to or less than the Tip length value. The length of conical part can
be calculated with the following formula: Cone Length = Tip diameter / (2*tan(
Tip angle /2))
• Tip length should be equal to or less than the Cutting Length value.
• Cutting Length should be equal to or less than the Outside Holder Length
value.
• Outside holder length should be equal to or less than the Total Length value.
66. 66
Chamfer drill3.5
This new tool type is used for
chamfering.
The image illustrates the parameters used
for the Chamfer drill tool definition.
Parameter limitations
• Angle should be greater than 0°
and less than 180°.
• Cutting Length should be equal
to or less than the Shoulder
Length value.
• Shoulder Length should be equal to or less than the Outside Holder Length
value.
• Outside Holder Length should be equal to or less than the Total Length value.
Outside
Holder
Length Cutting
Length
Arbor Diameter
Diameter
Total
Length
Shoulder
Length
Angle
67. 3. Tools
67
Dove tail mill3.6
This new tool type is available for dove
tail slot machining.
The image illustrates the parameters used
for the Dove tail tool definition.
Parameter limitations
• Angle should be greater than 0°
and less than 90°.
• Corner radius should be equal
to or less than half the Diameter
value.
• Cutting Length should be equal
to or less than the Shoulder
Length value.
• Shoulder Length should be equal to or less than the Outside Holder Length
value.
• Outside Holder Length should be equal to or less than the Total Length value.
Outside
Holder
Length
Cutting
Length
DiameterCorner Radius
AngleTotal
Length
Shoulder
Length
Arbor
Diameter
68. 68
Taper tool3.7
The cylindrical tool arbor is added to
the tool definition. The arbor diameter
and length are defined by: Arbor Diameter
and (Total Length - Shoulder Length). The
Shoulder Length should be greater than or
equal to the Cutting Length, and equal to
or less than the Outside Holder Length.
The image illustrates the parameters used
for the Taper tool definition.
Tools conversion
During the conversion of existing tools,
the tool arbor is added with the following
values:
• Arbor Diameter is equal to the
tool Shank Diameter
• Shoulder Length is equal to the Cutting Length + (Outside Holder Length – Cutting
Length)/2
Outside
Holder
Length
Cutting
Length
Angle
Diameter
Tip
Diameter
Corner
Radius
Arbor
Diameter
Total
Length Shoulder
Length
Cone
Length
Shank diameter
Corner
radius
Diameter
Taper angle
Cutting
Length
Outside
Holder
Length
Total
length
Cone length
Diameter
Corner
radius
Tip Diameter
Taper angle
Shoulder
Length
Outside
Holder
Length
Total
Length
Arbor Diameter
Cutting
Length
Old definition New definition
69. 3. Tools
69
In previous SolidCAM releases the flutes were considered to be only on the conical
face (flutes length and cone length were defined by the Cutting Length value). In
SolidCAM2008 R12, the cone length and flutes length are defined by separate parameters.
The Cone Length is determined by the Diameter, Taper angle and Tip diameter parameters.
The Cutting Length parameter defines the length of flutes. The flutes can be located at
the conical and cylindrical faces of the tool.
You choose one of the check boxes, at the side of the Tip Diameter and Cone Length
edit boxes, in order to define the taper tool using either the Tip diameter or the Cone
Length.
When the Tip Diameter check box is selected, the Cone Length check box is unselected
and the relevant edit box is disabled; the Cone Length value is thus automatically
calculated.
When the Cone Length check box is selected, the Tip Diameter check box is unselected
and the relevant edit box is disabled; the Tip Diameter value is thus automatically
calculated.
70. 70
Note that the Tip Diameter is the diameter of the virtual intersection of
the conical shape with the bottom plane.
Parameter limitations
• Tip diameter should be less than the Diameter value.
• Angle should be greater than 0° and less than 180°.
• Corner Radius should be equal to or less than half the Tip Diameter value.
• Corner Radius should be less than the Cone Length value.
• Cutting Length should be equal to or less than the Shoulder Length value.
• Shoulder Length should be equal to or less than the Outside Holder Length
value.
• Outside Holder Length should be equal to or less than the Total Length value.
Tip Diameter
71. 3. Tools
71
Engraving tool3.8
This new tool type is used for
engraving.
The image illustrates the parameters
used for the Engraving tool
definition.
Parameter limitations
• Tip diameter should be less than the Diameter value.
• Angle should be greater than 0° and less than 90°.
• Corner Radius should be equal to or less than half the Tip Diameter value.
• Corner Radius should be less than the automatically calculated Cone Length
value (the Cone Length is calculated using the Diameter, Tip Diameter and
Angle values).
• Cutting Length should be equal to or less than the Shoulder Length value.
• Shoulder Length should
be equal to or less than
the Outside Holder Length
value.
• Outside Holder Length
should be equal to or less
than the Total Length value.
Outside
Holder
Length
Cutting
Length
Tip Diameter
Diameter
Corner Radius
Angle
Total
Length
Shoulder
Length
Arbor Diameter
72. 72
Face Mill tool3.9
This new tool type is used for
facing.
The image illustrates the parameters
used for the Face Mill tool definition.
Note that the Cutting Length edit box
is disabled, this edit box displays
the automatically calculated Cutting
Length value.
Parameter limitations
• Tip diameter should be less than the Diameter value.
• Angle should be greater than 0° and less than 90°.
• Corner Radius should be equal to or less than the Cutting Length value.
• Corner Radius should be equal to or less than half the Tip Diameter value.
• Shoulder Length should be equal to or less than the Outside Holder Length
value and greater than or equal to the automatically calculated Cutting Length
value.
• Outside Holder Length should be equal to or less than the Total Length value.
Outside
Holder
Length
Cutting
Length
Arbor Diameter
Diameter
Tip Diameter
Total Length
Shoulder
Length
Angle
73. 3. Tools
73
Lollipop mill3.10
The cylindrical tool arbor is added to
the tool definition. The arbor diameter
and length are defined by: Arbor Diameter
and (Total Length - Shoulder Length). The
Shoulder Length should be greater than or
equal to the Cutting Length, and equal to
or less than the Outside Holder Length.
The image illustrates the parameters used
for the Lollipop mill definition.
During the conversion of existing
tools, the tool arbor is added with
the following values:
• Arbor Diameter is equal to
the tool Shank Diameter
• Shoulder Length is equal to
the Cutting Length
Parameter limitations
• Cutting Length has to be
equal to or less than the following value: (Diameter+sqrt( Diameter^2-Arbor
Diameter^2 ))/2
• Cutting Length has to be equal to or less than the Shoulder Length.
• Shoulder Length has to be equal to or less than the Outside Holder Length.
• Outside Holder Length has to be equal to or less than the Total Length value.
Outside
Holder
Length
Cutting
Length
Arbor Diameter
Diameter
Total
Length
Shoulder
Length
74. 74
Reamer tool3.11
The cylindrical tool arbor is added
to the tool definition. The arbor
diameter and length are defined by:
Arbor Diameter and (Total Length -
Shoulder Length). The Shoulder Length
should be greater than or equal to
the Cutting Length, and equal to or
less than the Outside Holder Length.
The image illustrates the parameters
used for the Reamer tool definition.
During the conversion of existing
tools, the tool arbor is added with
the following value:
• Arbor Diameter is equal to
the Diameter
Parameter limitations
• Chamfer Length should be equal to or less than the Cutting Length value.
• Cutting Length should be equal to or less than the Outside Holder value.
• Outside Holder should be equal to or less than the Total Length value.
Outside
Holder
Length
Cutting
Length
Chamfer Length
Diameter
Total
Length
Arbor Diameter
75. 3. Tools
75
Slot tool3.12
The Shank Diameter used in previous
SolidCAM versions, is renamed into
the Arbor Diameter in SolidCAM2008
R12, to be consistent with the other
tools.
The image illustrates the parameters
used for the Slot tool definition.
Outside
Holder
Length
Cutting
LengthDiameter
Corner Radius
Total
Length
Arbor
Diameter
76. 76
Spot Drill3.13
This new tool type is used for center
drilling and chamfering.
The image illustrates the parameters
used for the Spot Drill definition.
The Cutting Length edit box is
disabled. This edit box displays the
Cutting Length value, automatically
calculated by SolidCAM according
to the Diameter and Angle values.
Parameter limitations
• Angle should be greater
than 0° and less than 180°.
• Shoulder Length should be equal to or greater than the automatically calculated
Cutting Length value.
• Shoulder Length should be equal to or less than the Outside Holder Length
value.
• Outside Holder Length should be equal to or less than the Total Length value.
Outside
Holder
Length
Cutting Length
Diameter
Angle
Total
Length
Shoulder
Length
Arbor Diameter
77. 3. Tools
77
Tap tool3.14
The cylindrical tool arbor is added
to the tool definition. The arbor
diameter and length are defined by:
Arbor Diameter and (Total Length -
Shoulder Length). The Shoulder Length
should be greater than or equal to
the Cutting Length, and equal to or
less than the Outside Holder Length.
During the conversion of existing
tools, the tool arbor is added with
the following values:
• Arbor Diameter is equal to
the tool Thread Diameter
• Shoulder Length is equal to
the Cutting Length
Outside
Holder
Length
Cutting
Length
Tip Diameter
Chamfer
Length
Diameter
Total
Length
Arbor Diameter
78. 78
Thread Tool3.15
The Shank Diameter used in previous
SolidCAM versions, is renamed into
the Arbor Diameter in SolidCAM2008
R12, to be consistent with the other
tools.
The image illustrates the parameters
used for the Thread tool definition.
Outside
Holder
Length
Total
Length
Thread
Cutting
Length
Shoulder
Length
Arbor
Diameter
Thread Diameter
79. 3. Tools
79
Taper Thread Tool3.16
The Shank Diameter used in previous
SolidCAM versions, is renamed into
the Arbor Diameter in SolidCAM2008
R12, to be consistent with the other
tools.
The image illustrates the parameters
used for the Taper Thread tool
definition.
Outside
Holder
Length
Total
Length
Thread
Cutting
Length
Shoulder
Length
Arbor
Diameter
Thread Diameter
Angle
80. 80
Choosing the tool type3.17
The process of the tool type definition in SolidCAM2008 R12 is as follows: when you
start a new tool definition, SolidCAM displays the Tool Type dialog box in order to
choose the tool type.
For an existing tool, the tool type can be changed with the Change Tool type command
from the right click menu as shown.
81. 3. Tools
81
Tool Units3.18
In previous SolidCAM versions, the tools in the tool library were saved without the
units data. When a tool was loaded into a CAM-Part, its dimensions were interpreted
according to the CAM-Part units; therefore it was impossible to use tools with different
units than the units of the CAM-Part.
SolidCAM2008 R12 provides you with the possibility to assign units data for each tool in
the tool library. The tool library can store tools of different units. Such functionality
enables you to use tools, defined in different units than the units of the CAM-Part,
without converting the tool parameters into the CAM-Part units. You can choose the
units for the tool diameter values and tool lengths separately.
The Mm/Inch radio buttons are also added to the Default Tool data page. These radio
buttons enable you to define the units used for the speed/feed definition. In the Part
Tool Table, these radio-buttons are disabled; the units of the CAM-Part are used.
82. 82
When a tool library created in a previous SolidCAM version is loaded in SolidCAM2008
R12, the Assign Units dialog box enables you to assign units for tools.
83. 3. Tools
83
Angular dimensions3.19
In SolidCAM2008 R12, the button is added to each angular dimension edit box.
When the button is clicked, the angle is displayed in the degrees/minutes/seconds
format. The edit box becomes disabled.
When the button is clicked again, the edit box becomes enabled, with the angle
value in decimal format.
84. 84
Rough tools3.20
In previous versions, SolidCAM provided you with a separate tool type to define rough
end mill tools. SolidCAM2008 R12 enables you to define rough tools of all the following
types:
• End mill • Bull nose mill
• Ball nose mill • Face mill
• Taper mill • Slot mill
• Drill • Bore
• Dove tail mill
The Rough check box is added to the Tool topology page for the tools of types listed
above; this check box enables you to mark the tool as suitable for rough milling.
85. 3. Tools
85
The Rough tools only and Do not
display rough tools options are added
to the Range dialog box. These
options enable you to handle rough
tools during the tools sorting.
The Rough tools only option enables
you to display only rough tools in the
tools list.
When the Do not display rough tools
option is activated, the tools marked
as Rough are not displayed.
86. 86
Link to the Carmex and Vardex thread milling tool libraries3.21
SolidCAM2008 R12 provides you with a link to the Carmex (www.carmex.com) and Vardex
(www.vardex.com) thread milling tool libraries. This link enables you to choose the
appropriate thread milling tool from the Carmex or Vardex library and import it for
use inside the SolidCAM Thread Mill Operation.
The installations of the Carmex (Carmex_Setup.msi) and Vardex
(VardexTMGen11.0.26-Full.exe) tool libraries are located in the /Util folder under the
SolidCAM installation directory.
To import a tool from the Carmex or Vardex thread milling tools library, choose the
Carmex or Vardex item from the standard tables list for Thread Mill and Taper Thread Mill
tools.
The Carmex or Vardex tool library
wizard is launched. The wizard
guides you through the steps to
define the parameters of the tool
you are looking for, selects a number
of tools from the library that fit
these parameters and enables you to
choose one of these tools. When the
tool is chosen, it is imported into the
SolidCAM tool library.
88. 88
3D Depth type in Profile Milling4.1
In the previous versions of SolidCAM, you could
define the depth for the variable-depth profiles only
manually with the Define depth option. SolidCAM2008
R12 provides you with the new 3D option for
machining 3D profiles. This option facilitates
the depth definition by determining the depth-
change points automatically according to the model
geometry.
To define the profile depth with this option, choose
the 3D option in the Depth type area of the Profile
Operation dialog box.
With the 3D option, the Operation
Upper Level at each point along the
profile, is defined automatically by
the 3D Profile varying depth.
Profile Depth
89. 89
4. Milling
The Delta Z parameter enables you to
offset the Operation Upper Level in
the Z-axis direction.
If you want to edit the depth-change points defined automatically with the Profile 3D
option, choose the Define depth option and click on the Pick button.
The depth-change points are displayed on the model. The Define depth dialog box
displays the data of these points and enables you to edit the profile depth definition by
picking points manually on the model.
Delta Z
90. 90
Contour 3D operation4.2
SolidCAM2008 R12 provides you with the new Contour 3D operation which enables you
to utilize the power of the 3D Engraving technology for the 3D contour machining.
In this operation SolidCAM enables you to prevent the gouging between the tool and
the 3D contour.
The Contour 3D operation performs the machining of the defined 3D contour geometry
using the following technology parameters:
Tool reference
This option enables you to define the point on
the tool which is in contact with the machined 3D
contour.
• Tip. With this option, the tool tip is in
contact with the 3D contour; SolidCAM
prevents the gouging between the tool
and the 3D contour. Note that the tool
axis always crosses the geometry.
91. 91
4. Milling
• Center. With this option, the tool center
is in contact with the 3D contour. In
this case, SolidCAM does not check
the gouging between the tool and the
contour.
Technology
When the Tip option is chosen for the Tool Reference definition, SolidCAM provides
you with the following technology parameters:
Type
This option enables you to perform the semi-finish and/or finish of the
3D contour.
• Semi-finish performs the machining of the 3D contour in several steps
along the Z-axis. The vertical distance between two steps is defined by
the Step down parameter.
• Finish will machine the 3D contour to its final dimensions in one step
down.
• Both is used to machine the 3D contour first with a semi-finish cut
and then with a finish cut.
92. 92
Step down
This value defines the vertical distance between two successive steps
during the Semi-finish machining of the 3D contour.
• From Upper level. With this option, SolidCAM performs a number of
horizontal semi-finish passes at each down step, from the Upper Level
up to the defined Contour depth.
• From surface. SolidCAM performs a number of 3D semi-finish passes
at each step down, from the chosen 3D contour to the defined Contour
depth.
Contour depth
3D Contour geometry
Contour depth
Upper Level
3D Contour geometry
93. 93
4. Milling
T-Slot operation4.3
SolidCAM2008 R12 provides you with a new type of Milling
operation that enables you to machine slots in vertical walls
with a slot mill tool.
The definition of the T-Slot Operation is mainly similar to the regular Profile operation,
except for a number of parameters related to the milling of the ceiling face of the
slot.
Second offset number4.3.1
At the stage of the tool data definition, a
new parameter related to the tool offset
is available. The Second offset number
parameter defines the register number of
the upper cutting face offset, in the offset
table of the CNC machine. This option
enables SolidCAM to automatically take
into account the minor size differences
between the defined tool and the one
actually used for cutting the workpiece, if
there are any. You may choose not to use
this option by clearing the check box.
94. 94
Technological parameters4.3.2
Ceiling offset
For rough machining of the slot, you can define the offset
for the ceiling as well as for the walls and the floor.
You may choose to remove this offset with the finish pass by
selecting the Ceiling check box in the Finish section.
Cutting depth overlap
This parameter defines the overlap of each two adjacent tool
paths, in both the rough and finish machining of the slot.
Ceiling
offset
Cutting depth
overlap
Cutting depth
overlap
95. 95
4. Milling
Cutting direction
For both rough and finish cuts, you may define the direction of machining. The slot
can be milled from top to bottom or from bottom to top.
96. 96
Face Milling Operation4.4
In previous SolidCAM versions, face milling
(the machining of large flat surfaces with
face mill tools) was performed by utilizing
the Clear strategy of the Pocket Operation.
SolidCAM2008 R12 provides you with a new
Face Milling Operation which includes the
functionality of the Clear strategy and new
advanced functionality.
To create a new Face Milling operation, choose the
Face command from the Add operation submenu. The
Face Milling operation dialog box is displayed.
97. 97
4. Milling
Geometry definition
SolidCAM enables you to define the geometry for the Face
Milling operation with the Face Milling Geometry dialog box.
Name
Thiseditboxenablesyoutodefinethegeometry
name.
Geometry is based on:
This section enables you to choose the method
of the Face Milling geometry definition.
• Model. With this option a rectangle, located at the XY-plane and surrounding
the Target model, is generated and chosen for the Face Milling geometry.
The rectangle chain is displayed in the Chains List section.
Face Milling Geometry
98. 98
• Faces. This option enables you to define the Face Milling geometry by face
selection. The Define button and related combo-box enable you either to
define a new faces geometry with the Select Faces dialog box or to choose an
already defined geometry from the list. When the model faces are selected,
SolidCAM generates a number of chains surrounding the selected faces.
These chains are displayed in the Chains List section.
• Profile. This option enables you to define the Face Milling geometry by a
profile. The Define button and related combo-box enable you either to define
a new profile geometry with the Geometry Edit dialog box or to choose an
already defined geometry from the list. The defined chains are displayed in
the Chains List section.
Face Milling Geometry
Selected faces
Face Milling Geometry
99. 99
4. Milling
Chain List
This section displays all the chains chosen for
the Face Milling geometry.
The Merge button enables you to merge all the Face Milling geometry
chains into a single chain. The Separate button enables you to divide a
merged chain into its initial separate chains.
Modify
This section enables you to offset the chain
currently selected in the Chain List section. The
Apply to all button enables you to apply the
specified offset value to all the chains.
Separate chains Merged chain
Offset
100. 100
The definition of the Face Milling Operation is mainly similar to the regular Pocket
operation, except for a number of parameters related to face milling.
The Technology page of the Face Milling Operation dialog box provides you with the
following parameters:
Technology
SolidCAM enables you to choose the following technologies for the face milling:
• Hatch
With this strategy the machining is performed in a linear pattern. The Data
button displays the Hatch data dialog box which enables you to define the
hatch parameters.
The Hatch parameters used for the Face milling
are similar to the parameters used for the Hatch
strategy of the regular Pocket operation.
101. 101
4. Milling
During face milling the tool path is extended over the edges of the
machined face. The Extension section enables you to define the extension
both along the tool path (the Along section) and across the tool path (the
Across section). The extension can be defined either by percentage of the
tool diameter (the % of tool diameter option) or by value (the Value option).
• Contour
With this strategy the machining is performed
in a number of equidistant contours. The Data
button displays the Contour data dialog box which
enables you to define the contour parameters in
the same manner as for the Contour strategy of
the Pocket Operation.
The Contour parameters used for Face milling are
similar to the parameters used for the Contour
strategy of the regular Pocket operation.
Extension along
the tool path
Extension across
the tool path
102. 102
Similar to the Hatch strategy, the Contour tool path can also be extended
over the machined face edges. The Extension section enables you to define
the extension of the tool path, same all around. The extension can be
defined either by percentage of the tool diameter (the % of tool diameter
option) or by value (the Value option).
• One Pass
With this option, SolidCAM performs the face
milling in one pass. The direction and location of
the pass is calculated automatically, taking into
account the face geometry, in order to generate
an optimal tool movement with the tool covering
the whole of the geometry.
The Data button displays the One Pass data dialog
box which enables you to define the machining
parameters.
Extension
103. 103
4. Milling
The Extension section enables you to define the tool path extension over
the face edges. The extension can be defined either by percentage of the
tool diameter (the % of tool diameter option) or by value (the Value option).
The Overlap section enables you define the tool overlapping between two successive
passes. This section is enabled for Hatch and Contour strategies only.
Offsets
The Offsets section enables you to define the value of the Floor offset, the machining
allowance that is left unmachined on the face during the rough machining.
The Finish check box enables you to remove the remaining offset with the last cut (if
the check box is selected) or leave the offset unmachined for further operations (if the
check box is unselected).
Sort cut order
The Complete Z-level option enables you to define the order of the machining Z-levels,
in case more than one face is machined. The behavior of this option is similar to its
behavior in the Pocket Operation.
Extension
104. 104
Vertical zigzag passes in Profile operation4.5
In previous SolidCAM versions the linking of the
profile machining passes, located at successive
Z-levels (defined with the Step down parameter), was
performed by rapid movement up to, at and down
from the Clearance level. At the end of each pass the
tool performs a retreat movement to the operation
Clearance level, a horizontal movement at rapid feed
to the beginning point of the next pass and then
descends to the Z-level of the next pass. With this
method SolidCAM keeps the same cutting direction
(either climb or conventional) along the whole tool
path.
SolidCAM2008 R12 provides you with the possibility to
connect the passes, located at two successive Z-levels,
directly from the end of a pass to the beginning of
the next pass. With this connection method the
machining is performed in a zigzag manner; the
machining changes to the opposite direction from
one pass to the next.
The Depth cutting type section is located in the
Technology page of the Profile operation dialog box.
This section enables you to switch between the One
way and Zigzag options.
When the One way option is chosen, the cutting passes are oriented in the same direction
and connection between them is performed through the operation Clearance level.
When the Zigzag option is chosen, the tool path is performed in a zigzag manner, with
the tool path direction changing from one pass to the next.
The Zigzag option cannot be used together with the Clear offset
technology.
105. 105
4. Milling
Lead in and Lead Out
When the Lead In/Out strategies are used
together with the Zigzag option, SolidCAM
calculates the lead in/out movements for
all the cuts according to the direction of
the first cutting pass, irrespective of the
direction of the other cutting passes. During
the tool path linking, SolidCAM connects
the cuts (containing lead in and lead out
movements) in a zigzag manner and changes
the direction of all even cuts to the opposite.
Therefore only for odd cuts, the Lead in
strategy is used for the lead in and the Lead
Out strategy is used for the Lead Out. For
even cuts the Lead In strategy is used for the
Lead Out and the Lead Out strategy is used
for the Lead In.
Tool side and compensation
When the Zigzag option is used, the
Tool side combo-box defines the tool
location for the first cut. For each
successive cutting pass, the tool
position, relative to the geometry
direction, is changed.
When the compensation is used
for the tool path linked using the
Zigzag option, SolidCAM takes into
account the machining direction
and the changes in the tool position,
relative to the geometry direction,
for each successive cut. The different
compensation commands are used
in the GCode output for even and
odd cuts.
Movements defined by Lead in strategy
Movements defined by Lead out strategy
106. 106
Equal step down in Profile and Pocket operations4.6
In previous SolidCAM versions, the
machining of the Profile and Pocket
operations started from the Upper level
and continued on a number of successive
Z-levels till the operation Depth (modified
with the Floor offset and Delta depth
parameters). The distance between two
successive Z-levels was determined by the
Step down parameter. If the machining
depth was not divisible exactly by the Step
down parameter, the depth of the last cut
was less than the Step down parameter.
SolidCAM2008 R12 provides you with the Equal step down option that enables you to
keep an equal distance between all Z-levels. With this option you have to specify the
Max. Step down parameter (instead of the Step down parameter).
Step down
Last cut depth
107. 107
4. Milling
According to the operation Depth (modified with the Floor offset and Delta depth
parameters), SolidCAM automatically calculates the actual step down to keep an equal
distance between all passes, while making sure not to exceed the specified Max. Step
down value.
Max. Step down
Actual
step down
108. 108
Final cuts machining in Profile and Pocket operations4.7
SolidCAM2008 R12 provides you with the option to divide the depth to be machined
into two regions, each with its own Step down, with the second region, close to the
depth bottom, having the smaller Down step.
The Final cuts button is added to the Technology page of the Profile/Pocket Operation
dialog box.
This button displays the Final cuts dialog box. This dialog box enables you to define
the parameters of the Final cuts machining.
When the Final cuts used check box is activated, the option is used.
The Number of steps parameter defines the number of Final cuts.
The Step down value defines the distance between two successive Final cuts.
109. 109
4. Milling
When the Final cuts option is used, the check box on the
Final cuts button is activated.
When the Final cuts option is activated, SolidCAM performs the machining with the
operation Step down from the Upper level till the depth calculated according to the
following formula: Depth - Number of cuts * Step down.
From this depth, the machining is performed in a number of cuts, determined by the
Number of cuts/ Step down parameters in the Final cuts dialog box. The machining in
such manner is performed till the full operation depth.
Step down
Final Cuts
Step value
110. 110
Wall Draft angle in Profile and Pocket operations4.8
In previous SolidCAM versions, it was possible to perform Profile and Pocket
operations on vertical walls only.
SolidCAM2008 R12 enables you to perform the machining of walls inclined with a
constant draft angle along all the geometry.
The Wall draft angle button is added to the Technology
page of the Profile and Pocket operation dialog boxes.
This button displays the Wall draft angle dialog box.
When the Wall draft angle check box is activated in the
dialog box, the inclined wall machining is performed.
The External wall angle parameter defines the draft angle of
the wall; the angle is measured from the Z-axis direction as
shown.
The Islands wall angle parameter defines the draft angle
of the island walls. This parameter is relevant only within
the Pocket operation; the angle is measured similar to the
External wall angle parameter.
111. 111
4. Milling
For the inclined wall machining, each cutting pass located
at a specific Z-level is generated according to the specified
External/Island wall angle parameter.
The External corner type option enables you to define how
the cutting passes will be connected during the external
corners machining. The following possibilities are available
for two possible types of corners in the geometry model:
If the geometry model has sharp corner there are two options for creating tool path at
the corner:
• Sharp Corner. With this option the tool
path is calculated in such a way so as to
perform the machining of a sharp corner.
• Conical fillet. With this option the tool path
is calculated in such a way so as to perform
the machining of the corner with a conical
fillet; the radius of the tool path rounding
increases from one pass to the next.
If the geometry model has filleted corner there is one option for creating tool path at
the corner:
• Cylindrical fillet. The tool path is calculated
in such a way so as to perform the
machining of the corner with a cylindrical
fillet; the radius of the tool path rounding
is the same for all the cutting passes.
Geometry
Geometry
Geometry
112. 112
Profile floor machining4.9
In previous SolidCAM versions, the Profile operation enabled you to define a
machining allowance in XY direction (Wall offset), leaving it unmachined during the
profile roughing and removing it during the finishing passes (within the same operation
or within another Profile operation).
SolidCAM2008 R12 provides you with the possibility to define a similar allowance in
the Z-direction (Floor offset). This Floor offset is left unmachined during the profile
roughing and removed during the finishing.
The Floor offset parameter is added to the Offsets section,
located on the Technology page of the Profile operation dialog
box.
The Floor offset parameter is available only when the Rough section is
activated.
When the Floor offset is specified,
SolidCAM performs the machining
by the Z-levels defined with the Step
down parameter. The machining
is performed up to the Floor offset
from the Profile depth.
The Clear offset section enables you
to define the parameters of the Clear
offset machining for the roughing
and finishing passes.
Floor offset
Step Down
Profile Depth
113. 113
4. Milling
The use of the Clear offset option for the Profile
finishing enables you to perform the machining of
both the Wall and Floor offsets. In this case, SolidCAM
performs first the machining of the floor area and
then the walls.
The floor area is machined with a single cutting pass
at the Profile depth. This cutting pass is calculated
using the Clear offset strategy (with the specified
Offset and Step over parameters) and taking into
account the specified Wall offset.
The wall finishing is performed from
the Upper level till the Profile Depth in
a number of steps defined with the
Step down parameter.
Offset
Wall offset
Step Over
Step Down
Profile Depth
114. 114
Pocket Wall finishing4.10
In previous SolidCAM versions, the
pocket walls finishing was performed
with a single cut at the whole Pocket
depth.
SolidCAM2008 R12 enables you also
to perform the finishing of the walls
in a number of successive cuts, with
the distance between them defined
by the Step down parameter.
The Depth section is added to the Finish section of
the Pocket operation dialog box.
This section enables you to choose how the wall
finish will be performed: either at the whole depth
(Total depth option) or in a number of steps at each
step down (Each step down option).
The options of the Depth section are available only when the wall finishing
is performed in the operation (the Wall or Floor option is used for the
Finish).
When the Wall draft angle option is used in the operation, the Depth options
are disabled and the Each step down option is used for the Wall finishing.
Finish passes
Single Finish pass
115. 115
4. Milling
4.11 Open Pocket machining
SolidCAM2008 R12 provides you with the functionality to
performthemachiningof apocketwithacombinationof
open edges and closed walls. This functionality generates
optimized tool path and lead in movements.
Open Pocket Geometry definition4.11.1
SolidCAM enables you to define the geometry for the
Open Pocket Machining by defining open edges on the
conventional Pocket geometry.
The Mark open edges command is added to the right click menu
available on chain items in the Chain List section of the Geometry
Edit dialog box. This command displays the Mark Open Edges
dialog box. This dialog box enables you to mark the open edges
on already chosen pocket chains by picking on them.
The Mark as section of the dialog box enables you to choose the
selection mode. When the Open option is chosen, picking a pocket
geometry edge marks it as open. When the Wall option is chosen,
picking a pocket geometry edge marks it as closed (wall). With
the Toggle option, picking a closed edge marks it as open and vise
versa.
Open Pocket
Pocket geometry
Open edge
Closed edges
116. 116
The Select section enables you to choose the selection method. When the Single entity
option is chosen, SolidCAM enables you to pick single entities in order to mark them
in order to mark them as open/closed. When the From/To entities option is chosen,
SolidCAM enables you to mark a segment of the pocket geometry by picking the start
and the end entities.
The CAD Selection button enables you to perform the selection using the CAD tools.
Open pocket machining parameters4.11.2
The Open Pockets section is added to the Technology page of
the Pocket operation dialog box. This section is enabled only
when the pocket geometry contains open edges.
During the Open pocket machining the tool path is extended
beyond the open edges. The Extension section enables you
to define the overlapping between the tool and the open
edges; the overlapping can be defined either by percentage
of the tool diameter (the % of tool diameter option) or by
value (the Value option).
TheUse profile strategy optionenablesyoutoperform
the Open pocket machining in a Profile manner. The
tool path at a specific Z-level consists of a number of
equidistant profiles starting from outside the model
(at the distance defined by the Extension parameter).
The tool moves in parallel offsets to the pocket
geometry.
Extension
Open edge
117. 117
4. Milling
The One way/Zigzag options enable you to define the tool path direction and linking.
• With the Zigzag option, the tool finishes one profile pass and then directly
moves to the next pass. The machining is performed without leaving the
material, thus constantly switching between climb and conventional milling.
• With the One way option, the tool finishes one profile pass, then rapidly
moves (G0) to the safety distance and then to the start of the next cutting
pass. The cutting direction (either climb or conventional) is preserved for
each cutting pass.
The Approach from outside option enables the tool to approach from outside of the
material in the open pocket areas, if possible. Such an approach enables you to decrease
the tool loading when plunging into the material. This option enables SolidCAM to
perform the approach movement from an automatically calculated point outside of
the material. The tool moves to the necessary depth outside of the material and then
plunges into the material.
The Descend to cutting level with Rapid option enables you to avoid vertical non-
machining movements outside of the material performed with the working feed by
direct rapid movement down to the cutting level.
118. 118
When this check box is selected, the tool descends from the Clearance level outside of
the material directly to the cutting level (defined with the Step down parameter) using
the Rapid feed. Then the horizontal movement into the material is started with the
working feed.
When this check box is not selected, the tool descends from the Clearance level down to
the Safety distance with Rapid movement. From the Safety distance, the tool descends
down to the cutting level (defined by the Step down value) with the defined feed and
starts the horizontal cutting movements into the material with the working feed.
The Descend to cutting level with Rapid check box is available only when the
Approach from outside check box is selected.
Upper level
Safety distance
Cutting level
Rapid movement
Feed movement
Upper level
Cutting level
Rapid movement
119. 119
4. Milling
Adjacent tool paths connection in Profile operations4.12
SolidCAM2008 R12 provides you with the Adjacent tool paths connection option for the
Profile operation. This option enables you to choose the connection method for adjacent
cutting passes generated using the Clear offset method with Zigzag option.
The Adjacent tool paths connection section is added to the Links page of the Profile
operation dialog box.
The following options are available to define the passes connection:
• Linear. With this option, the tool
movement from one cutting pass to the
next, is a straight line connecting the end
point of the first pass to the start point
of the next pass.
120. 120
• Rounded. With this option, the tool
movement from one cutting pass to the
next is an arc, tangential to the adjacent
cuttings passes. The arc connects the
end point of the first pass to the start
point of the next pass.
121. 121
4. Milling
Complete Z-level in Pocket operations4.13
SolidCAM2008 R12 provides you with a new Complete Z-level option which enables you
to define the order of the machining Z-levels during the machining of several pockets
within a single Pocket operation. The option is located in the Technology page of the
Pocket operation dialog box.
When the Complete Z-Level check box
is not selected, SolidCAM machines
all the Z-levels of the first pocket
and then starts the machining of the
next pocket.
When the Complete Z-Level check
box is selected, the machining is
performedbytheZ-levels;SolidCAM
removes material at a specific Z-level
in all the pockets and then moves to
the next Z-level.
1
2
3
4
5
6
7
8
1 2
3 4
5 6
7 8
122. 122
Movements between cutting passes4.14
SolidCAM2008 R12 provides you with a new Keep tool down option that enables you to
reduce unnecessary rapid tool movements upto, at and down from the Clearance level,
during machining with Profile, Pocket, Pocket Recognition and Face Milling operations.
This option is added in the Link page of the operation dialog box.
If the Keep tool down check box is not selected, then after
the machining of a specific Z-level, the tool retracts up
to the Operation Clearance level. At this level the tool
horizontally moves to the start position of the next cut
and then descends to the next Z-level.
If the Keep tool down check box is selected, then after
the machining of a specific Z-level, the tool directly
moves to the start position of the next cut (without
retreating up to the Clearance level) and then descends
to the next Z-level.
Clearance level
123. 123
4. Milling
Minimal machined area in Floor Constant Z machining4.15
In the Constant Z floor machining of 3D models, SolidCAM2008 R12 provides you with
the possibility to define the minimal tool path segment length that will be machined.
The Min. cut area option is added into the Constant Z flat floor machining section of the
Constant Z Semi-Finish and Constant Z Finish dialog boxes.
126. 126
Drill Recognition operation5.1
SolidCAM2008 R12 providesyouwiththenew
Drill Recognition operation that combines
the power of automatic hole feature
recognition and the interactive control by
the user of the machining technology. This
operation provides you with two significant
advantages versus the current Drilling
operation:
• The Drill Recognition operation
performs powerful drill feature
recognition and automatic
Drill geometry creation using
SolidCAM AFRM module
functionality.
• While the Drilling operation enables you to define only one set of Milling
Levels parameters (Upper Level, Drill Depth, Delta Depth) that is common for all
the drill positions, the new Drill Recognition operation enables you to handle
separate sets of Milling Levels for each drill position. The initial values of the
Milling Levels sets are automatically recognized from the model and they can
be edited by the user.
The Drill Recognition operation dialog box enables you to define the geometry and the
technological parameters of the operation.
127. 5. Automatic Feature Recognition and Machining (AFRM)
127
Geometry definition5.1.1
SolidCAM2008 R12 enables you to define the geometry for the Drill Recognition operation
using the AFRM functionality. The geometry used for the Drill Recognition operation is
automatically recognized on the Target model. Therefore the Target model should be
defined in the CAM-Part before you define the Drill Recognition operation.
The geometry definition is performed using the HR Drill
Geometry Selection dialog box. This dialog box provides
you control over the parameters of the drill recognition
and enables you to select the specific hole features that you
want to machine in the current Drill Recognition operation.
The hole recognition is performed on the Target model in
a direction parallel to the Z-axis of the Coordinate System
chosen for the operation.
The major steps of the HR Drill Geometry selection are
follows:
• Choose the model configuration used for the
recognition.
• Set the selection filter options (Hole type, Hole
diameter, Hole Upper level and Hole Height).
• Perform the holes recognition and generate the
recognized holes tree.
• Choose from the holes tree those holes that you
want to include in the operation geometry.
• See a preview of the machining sequence.
Following is a detailed explanation of the all the sections and
parameters of the HR Drill Geometry Selection dialog box.
128. 128
Name
This edit box enables you to define the geometry name.
Configuration
This section enables you to select the SolidWorks model configuration to
be used for the geometry definition.
Hole type
This section sets the recognition filter that filters the hole features according
to their type.
The Through check box enables you to recognize the through hole features.
The Blind check box enables you to recognize the blind hole features.
When both of these check boxes are unselected, hole recognition
cannot be performed and the Find Holes button is disabled.
Hole Diameter (d)
When this section is activated, SolidCAM
enables you to filter the hole features according
to the Hole Diameter. With this filter, only the
hole features with the Hole Diameter within the
specified range are recognized.
The From and To values enable you to define the diameter range either by
typing in the values or by picking on the solid model. When the cursor
is located in the From/To edit box, SolidCAM enables you to specify the
diameter value by picking either a specific cylindrical surface or a circular
edge in the solid model. When a cylindrical surface / circular edge is
picked, its diameter is calculated and inserted into the relevant edit box (the
previous value is removed). The edit box becomes pink. When you remove
the automatically determined value, the edit box becomes white.
129. 5. Automatic Feature Recognition and Machining (AFRM)
129
The Thread only option enables you to recognize only hole features with
threads. When this option is checked, the From and To values define the
range of the Thread diameter values. When the Thread option is active the
From and To values can be defined by picking either a specific cylindrical
surface, cosmetic thread or circular edge in the solid model.
Hole Upper level (u)
When this section is activated, SolidCAM
enables you to filter the hole features according
to the Upper Level. With this filter, only the hole
features with the Upper Level within the specified
range are recognized.
The From and To values enable you to define the Upper Level range either
by typing in the values or by picking on the solid model. When the cursor
is located in the From/To edit box, SolidCAM enables you to specify
the Upper Level value by picking the solid model. When a model point
is picked, the Z-value of the picked position is calculated and inserted
into the relevant edit box (the previous value is removed). The edit box
becomes pink. When you remove the automatically determined value, the
edit box becomes white.
Hole height (h)
When this section is activated, SolidCAM
enables you to filter the hole features according
to the Hole Height. With this filter, only the hole
features with the Hole Height within the specified
range are recognized.
The From and To values enable you to define the Hole Height range either
by typing in the values or by picking on the solid model. When the cursor
is located in the From/To edit box, SolidCAM enables you to specify the
Hole Height value by picking the solid model. When a model point is picked,
the Z-value of the picked position is calculated and inserted into the
relevant edit box (the previous value is removed). The edit box becomes
pink. When you remove the automatically determined value, the edit box
becomes white.
