SolidCAM Simultaneous
5-axis Machining
User’s Guide
©1995-2005 SolidCAM LTD.
All Rights Reserved.
5-axis MachiningSolidCAM2005 Milling Manual
Contents
1. Introduction ............................................................................................................................... 5
2. User Interface ........................................................................................................................... 6
2.1 Adding a 5-axis Operation ....................................................................................................6
2.2 5-axis Operation user interface ............................................................................................8
2.3 Stages of the Simultaneous 5-axis Operations parameters definition ............................... 10
3. CoordSys Page ...................................................................................................................... 11
4. Tool Page ................................................................................................................................ 12
5. Levels Page ............................................................................................................................ 14
6. Geometry Page ...................................................................................................................... 17
6.1 Drive surface selection ....................................................................................................... 18
6.2 Cut Controls: ...................................................................................................................... 20
6.2.1 Parallel cuts ..................................................................................................................
Exercise 1: .................................................................................................................... 23
Exercise 2: .................................................................................................................... 25
6.2.2 Cuts along curve ........................................................................................................... 26
Exercise 3: .................................................................................................................... 27
Exercise 4: .................................................................................................................... 28
6.2.3 Morph between two curves ........................................................................................... 30
Exercise 5: .................................................................................................................... 32
Exercise 6: .................................................................................................................... 34
6.2.4 Parallel to curve ............................................................................................................
Exercise 7: .................................................................................................................... 37
Exercise 8: .................................................................................................................... 38
6.2.5 Project curves ............................................................................................................... 40
Exercise 9: .................................................................................................................... 41
Exercise 10: .................................................................................................................. 43
6.2.6 Morph between two surfaces ........................................................................................ 45
Exercise 11: .................................................................................................................. 46
Exercise 12: .................................................................................................................. 48
6.2.7 Parallel to surface .........................................................................................................
Exercise 13: .................................................................................................................. 52
6.3 Flip Stepover ...................................................................................................................... 54
Exercise 14: .................................................................................................................. 55
6.4 Cutting Method ................................................................................................................... 56
6.5 Cut Order ...........................................................................................................................58
Exercise 15: .................................................................................................................. 60
20
36
50
2
5-axis Machining
SolidCAM2005 Milling Manual
6.6 Direction for One Way machining ......................................................................................62
Exercise 16: .................................................................................................................. 64
6.7 Cutting Area ....................................................................................................................... 65
Exercise 17: .................................................................................................................. 67
6.8 Start Point ..........................................................................................................................
69
7. Finish Parameters page: ........................................................................................................ 71
7.1 Tool Contact point ..............................................................................................................
72
Exercise 18: .................................................................................................................. 75
7.2 Lead in / Lead out ..............................................................................................................79
Exercise 19: .................................................................................................................. 82
Exercise 20: .................................................................................................................. 86
7.3 Round surface by tool radius .............................................................................................92
7.4 Stock to leave .....................................................................................................................94
7.5 Multi Passes .......................................................................................................................
95
7.6 Surface Quality ...................................................................................................................97
7.6.1 Chaining Tolerance .......................................................................................................
97
7.6.2 Cut tolerance ................................................................................................................ 98
7.6.3 Distance ........................................................................................................................ 99
7.6.4 Stepover ..................................................................................................................... 100
8. Gaps Page ............................................................................................................................ 101
8.1 Gap Along Cut ..................................................................................................................101
8.1.1 Gap Size as % of tool diameter .................................................................................. 102
8.1.2 Direct .......................................................................................................................... 102
8.1.3 Broken ........................................................................................................................ 103
8.1.4 Retract ........................................................................................................................ 103
8.1.5 Follow Surface ............................................................................................................
104
8.2 Gaps between cut (Gap Size as % Of Stepover) ............................................................. 105
8.2.1 Gap Size as % of Stepover ......................................................................................... 105
8.2.2 Direct .......................................................................................................................... 106
8.2.3 Broken ........................................................................................................................ 106
8.2.4 Retract ........................................................................................................................ 107
8.2.5 Follow surface .............................................................................................................
9. Tool axis control page ...........................................................................................................
107
108
9.1 Output format ................................................................................................................... 109
9.2 Maximum angle change ................................................................................................... 110
9.3 Tilting strategies (Toll axis direction) ................................................................................
9.3.1 Tool axis is not tilted and stays normal to the surface ................................................
9.3.2 Tool axis will be tilted relative to cutting direction ......................................................
9.3.3 Tool axis will be tilted with the angle ..........................................................................
111
111
112
114
3
5-axis MachiningSolidCAM2005 Milling Manual
9.3.4 Tool axis will be tilted with fixed angle to axis ............................................................ 114
9.3.5 Tool axis will tilted around axis ...................................................................................
9.3.6 Tool axis will be tilted through point ...........................................................................
9.3.7 Tool axis will be tilted through curve ...........................................................................
9.3.8 Tool axis will be tilted through lines .............................................................................
115
116
117
123
9.3.9 Tilted from point away ................................................................................................. 123
9.4 Side tilt definition .............................................................................................................. 124
9.5 Tool axis direction limit parameters ..................................................................................
125
9.5.1 XZ Limit ....................................................................................................................... 126
9.5.2 YZ Limit ....................................................................................................................... 126
9.5.3 XY Limit: ..................................................................................................................... 127
9.5.4 Conical angles from leading curve .............................................................................. 127
10. Gouge Check page ............................................................................................................ 128
10.1 Clearance ....................................................................................................................... 128
10.2 Check gouge between positions .................................................................................... 129
10.3 Gouge pages ..................................................................................................................131
10.4 Tool .................................................................................................................................
10.4.1 Tool Tip and Tool Shaft .............................................................................................
131
131
10.4.2 Check Arbor and Check Holder ................................................................................ 132
10.5 Strategy .......................................................................................................................... 132
10.5.1 Retracting tool along tool axis ................................................................................... 133
10.5.2 Moving tool away ...................................................................................................... 134
10.5.3 Tilting tool away with max angle ............................................................................... 141
10.5.4 Leaving out gouging points ....................................................................................... 143
10.5.5 Stop tool path calculation .......................................................................................... 143
10.6 Drive Surfaces ................................................................................................................144
10.7 Check Surfaces .............................................................................................................. 144
10.8 Stock to leave .................................................................................................................144
11. Stock Page .........................................................................................................................
12. Additional parameter Page .................................................................................................
145
146
13. Appendix ............................................................................................................................ 147
13.1 Single Surface versus Multi Surface Machining in 5 Axis .............................................. 147
13.2 At the beginning of all: Single Surface 5 Axis Flowline .................................................. 147
Document number: SC5AUG06001
4
5-axis Machining
SolidCAM2005 Milling Manual
1. Introduction
Simultaneous 5-Axis machining is becoming more and more popular due to the need for reduced
machining time, better surface finish and improved life span of tools. SolidCAM utilizes all the
advantages of Simultaneous 5-Axis machining and together with collision control and machine
simulation, provides a solid base for your 5-Axis solution. A number of intelligent and powerful 5axis machining strategies enable the use of SolidCAM for machining of such complex geometry parts
as turbine blades and impellers. SolidCAM provides a realistic simulation of the whole machine tool,
showing the motion of all rotational and linear axes.
5
2. User Interface
2.1 Adding a 5-axis Operation
5-axis MachiningSolidCAM2005 Milling Manual
5-axis (3)
This operation performs 3-axis operations using special tools such as Lollipop and T-cutter, mostly
for undercut areas. It is also possible to use the standard tools in this operation in order to create a
3D finish tool path; in this case the operation generates 3 axis G-Code and it is not possible to tilt the
tool.
This operation is available for 3 axis, 4 axis and 5 axis CNC-machines.
6
5-axis Machining
SolidCAM2005 Milling Manual
5-axis (4)
This operation is used for 4-axis finish operations such as turbine blade profiles on the outside diameter
and spiral parts. The tool will be normal to the center line but will not necessarily cross the center line.
The only tilt strategies that are available are those that support this type of tilting (4-axis).
This operation generates 4-axis G-code and is available for 4-axis and 5-axis CNC-machines.
This Operation type is unavailable for 3-axis CNC-machine types.
The output from this operation depends on the CNC machine type.
For the 4-axis machine, the output will be performed with the @line_4x and @move_4x commands.
For the 5-axis machine, the output will be performed with the @line_5x and @move_5x commands.
With such output, SolidCAM positions the tool to the proper working angle using 5-axis capabilities
and then performs the 4-axis machining.
5-axis (5)
This operation is used for 5-axis finish and supports all kinds of 5-axis operations. The user has
complete control over all the cutting parameters. The tool can be tilted to any possible direction that
the machine supports. All the tilt strategies are available.
The operation generates 5 axis G-code. The @line_5x and @move_5x commands will be used in the
output.
This type of operation is available only for postprocessors that support 5-axis machining.
7
2.2 5-axis Operation user interface
The following 5-axis Operation dialog is displayed on the screen:
5-axis MachiningSolidCAM2005 Milling Manual
The parameters of the 5-axis Milling Operation are divided into a number of
sub-groups. The sub-groups are displayed in a tree format on the left side of
the 5-axis Operation dialog box. When you click on an item in the tree, the
parameters of the selected sub-group appear on the right side of the Operation
dialog box.
• CoordSys Page
Define the CoordSys Position for the 5-axis machining.
• Tool Data Page
Choose a tool for the operation and define tool-related parameters such as feed and spin.
• Levels Page
Define Milling levels such as Clearance plane and Safety distance.
• Geometry
SolidCAM enables you to choose a drive surface for the machining. Define the machining
parameters such as the Cut control, Cuting area, Cutting method etc.
8
5-axis Machining
• Finish Parameters
This page enables you to define the machining parameters such as Cut tolerances, Stock
to leave, Run tool etc.
• Gaps Page
Surfaces defining the work piece can have gaps and holes. In such cases you can choose
between several options. For example you can choose to have small gaps ignored and
milled without the tool retracting and big gaps detected with the tool retracting back to
the rapid plane and skipping the gap. Such options are set within this dialog. Entry and Exit
moves are also defined here.
• Tool axis control
Define the tool orientation relative to the surface normal.
• Gouge check
SolidCAM2005 Milling Manual
This page contains all the options to avoid the tool gouging selected drive surfaces and
check surfaces.
• Motion Limit control
This page is related to CNC machine definitions. The defaults are determined by the
MAC-file (machine definition parameters). Generally, these parameters are defined in the
first definition of the postprocessor for this machine and usually it is not necessary to
change these values. The Motion Limit control page enables you to change the parameters
locally for the current operation.
• Stock Page
Stock definition can be provided in this page. All tool moves in the air that do not remove
material will be trimmed using this given stock definition.
• Miscellaneous parameters
This page contains special functions for custom applications.
9
5-axis MachiningSolidCAM2005 Milling Manual
Tool path generation Tool axis control
Gouge check
2.3 Stages of the Simultaneous 5-axis Operations parameters definition
The process of the Operation parameters definition for the tool path creation is divided into 3
stages:
1. Geometry, Finish Parameters and Gaps – the type of finish tool paths generated
along the selected faces is defined. Tool tilting and gouging are not taken into
account at this stage.
2. Tool axis control - controls the angle of the tool from the normal vector in every
point along the tool path.
3. Gouge check –the gouge strategies that SolidCAM has to take into account to
avoid tool and holder crashes are defined.
10
5-axis Machining
3. CoordSys Page
SolidCAM2005 Milling Manual
Choose the appropriate CoordSys position for the operation. The CoordSys Position can be chosen
either direcly on the model or from the list.
After the CoordSys selection, the model will be rotated to the selected CoordSys orientation.
The CoordSys selection operation must be the first step in the Operation
definition process.
In the 5 axis (3) Operation, SolidCAM enables you to choose both the Machine
Coordinate systems and CoordSys Positions for the operation. In 5 axis (4)
and 5 axis (5) operations, SolidCAM enables you to choose only the Machine
Coordinate systems. The Machine CoordSys definition contains data of the
Machine CoordSys location relative to the center of the rotation of the machine.
Therefore, SolidCAM enables you to generate the G-Code according to the
center of the rotation of the machine.
11
4. Tool Page
5-axis MachiningSolidCAM2005 Milling Manual
The Data button enables you to choose a tool from the Part Tool Table.
12
5-axis Machining
Feed Finish
This field gets the default from the Feed Finish parameter in the Tool Data dialog. If the
user changes this value it will not change the related field in the Tool Data dialog.
Feed Z
The feed that SolidCAM will use to move from the safety position to the depth point.
Retract Rate
The feed that SolidCAM will use to move the tool from the material to the retract level.
Spin Finish
The spindle speed for the cutting operation.
SolidCAM2005 Milling Manual
Feed Rates
If this switch is set, then the feed rate optimizer is utilized. The feed rate optimizer uses
the machining feed rate supplied by the user and modifies this feed rate based on the
surface curvature. The surface curvature is calculated at each tool path position where the
surface contact point of the tool is known.
13
This function works only on single surfaces and can’t be used to connect 2
surfaces
5. Levels Page
5-axis MachiningSolidCAM2005 Milling Manual
Clearance Plane
The clearance plane is a Z coordinate value and presents an absolute plane at this height
which is parallel to the XY plane. The tool moves from and to this clearance plane to
make major repositionings. In some cases like turbine blade machining around the X axis,
it might be better to have the clearance plane defined in the X axis. Setting the clearance
plane height in the X axis will make the YZ plane the parallel plane and the given X value
will be the clearance value over this plane.
14
5-axis Machining
Clearance plane
Safety distance
Retract distance
Retract distance
Safety distance
Retract Rate
Rapid feed
Retract distance
Retract Distance and Safety Distance
SolidCAM2005 Milling Manual
The tool changes its orientation at the clearance plane (machine tables or spindles are
turned) and then it moves down to the part to the retract distance. The tool then moves
in a rapid motion with some orientation to the safety distance. The tool then approaches
the surface with the cutting feed rate.
Rapid Retract
This option enables you to perform the retract movement with the rapid feed.
When this option is not active, the tool will be moved to the safety distance with the
defined Retract Feed (see topic 4.).
15
5-axis MachiningSolidCAM2005 Milling Manual
Safety distance
Rapid feed
Retract distance
When the Rapid Retract option is active, the retract movement will be performed with the
Rapid Feed.
Depth
The Depth defines a further offset of the tool in the axial direction (especially for swarf
operations).
This command shifts each point of the tool path in the vector direction of the tool. The
start position of the cutting will also be shifted. The gouge control will take out all the
gouges that result from this shift.
16
5-axis Machining
6. Geometry Page
SolidCAM2005 Milling Manual
This page enables you to select the faces to be machined and the machining strategy. The different
strategies available are:
• Parallel cuts
• Cut along curve
• Morph between 2 curves
• Parallel to curve
• Project curve
• Morph between 2 surfaces
• Parallel to surface
For all the above strategies, select the drive surface and the related geometries. In the Morph
between 2 curves and Parallel to curve strategies, the curves have to be part of the surface external
boundaries. Select the faces first, and than select the edges. Do not use sketches to define these types
of geometries.
17
6.1 Drive surface selection
Click on the Define button. The Choose faces dialog will be displayed.
5-axis MachiningSolidCAM2005 Milling Manual
This dialog enables you to select one or several faces of the SolidWorks model. The selected Face tags
will be displayed in the dialog.
If you chose wrong entities, use the Unselect option to undo your selection.
You can also right click on the entity name (the object will be highlighted)
and choose the Unselect option from the menu.
18
5-axis Machining
SolidCAM enables you to machine surfaces from the
positive direction of the surface normals. Sometimes
surfaces are not oriented correctly and you have to
reverse their normals. The Reverse/Reverse All
command enables you to reverse the direction of the
surface normals.
SolidCAM does not enable you to see the surface direction. You have to select
the faces for the 5 axis operation and calculate the operation. If the tool is
machining one of the faces from the wrong direction, return to the Geometry
definition and use the Reverse command.
SolidCAM2005 Milling Manual
19
6.2 Cut Controls:
Y
X
5-axis MachiningSolidCAM2005 Milling Manual
The Exercises of the
Cut control option are located in the Exercises\Cut_Control folder.
6.2.1 Parallel cuts
Parallel cuts option will create tool paths that are parallel to each other. The direction of the cuts
The
is defined by two angles. The angles in X, Y and Z determine the direction of the parallel cuts of the
tool path. Imagine slicing an apple: You can slice it with a knife parallel from top to bottom or from
the left side to the right side. The pictures in the dialog show how the desired cutting direction is set
using the angles.
With constant X
Changing the Machining angle in the Z parameter to 90 degrees creates tool
paths parallel to the Y axis. The X-distance is constant.
20
5-axis Machining
Y
X
Z
X
With constant Y
SolidCAM2005 Milling Manual
With constant Z
Changing the Machining angle in Z and the Machining angle in X, Y to 90 degrees
creates tool paths parallel to the X axis. The Y-distance is constant.
Changing the Machining angle in Z and the Machining angle in X, Y to 0 degrees
creates circular tool paths. The Z-distance is constant.
21
Fast orientation buttons
5-axis MachiningSolidCAM2005 Milling Manual
Th following buttons enable you to expedite the definition of the orientation of the parallel cuts.
The Constant Z button.
The Parallel button.
In this setup you can enter any angle to get the required tool path.
22
5-axis Machining
Exercise 1:
SolidCAM2005 Milling Manual
1. Load the CAM-Part: Exercises\Cut_control\parallel_cuts.prt
2. Simulate the operations and check the parameters used to control the Machining
angles for the Parallel Cuts strategy.
3. Add operations for the machining of other cylinders. Use the
Parallel Cuts
strategy and define the necessary parameters in order to cut the cylinder normal
to the direction of the center line.
4. In order to cut the cylinder and the top face you have to use a different angle
(inclination). Create some operations to practice this task.
23
5-axis MachiningSolidCAM2005 Milling Manual
The option is chosenThe option is not chosen
Change Parallel cuts to spiral
This option enables you to substitute the parallel cuts with the spiral cuts with the pitch equal to the
defined Step over.
24
5-axis Machining
Exercise 2:
SolidCAM2005 Milling Manual
1. Load the CAM-Part: Exercises\Cut_control\parallel_cuts.prt
2. Simulate the operations and check the parameters used to control the Machining
angles for the Parallel Cuts strategy.
3. Edit the operation rotate around z 45 deg.
4. In the Geometry page, choose the Change parallel cuts to spiral option.
5. Calculate and simulate the operation. Note that the parallel cuts of the operation
were changed to spiral movements.
25
6.2.2 Cuts along curve
90°
90°
90°
Curve
Tool path
5-axis MachiningSolidCAM2005 Milling Manual
The Cuts along curve option enables the user to
select a leading curve. The generated tool path is
orthogonal to this leading curve, so the cuts do not
have to be parallel to each other. If a wrong leading
curve is selected, the cuts can cross over each other
and the result will be unacceptable.
The curve geometry does not have to be located
on the surface or on the edges of the surface. The
selected chain could be a planar or a 3D sketch. In
each point of the leading curve, SolidCAM creates
a plane nornal to the curve. The tool path will be
created at the intersection of this plane with the
drive surface.
This kind of tool path is popular for milling engines
ports or internal curved surfaces.
26
5-axis Machining
Exercise 3:
SolidCAM2005 Milling Manual
1. Load the SolidWorks document: Exercises\Cut_control\cone.sldprt
2. Define a new CAM-Part. Use the Fanuc_4x_x postprocessor.
3. Define the Machine CoordSys with the X-axis directed along the cone centerline
and the Z-axis directed upwards. For the CoordSys definition, use the home_
definition sketch.
4. Start a new 5-axis Operation and choose the Cuts Along Curve strategy.
5. Define the conical face as the
drive surface. Choose the circle
segment contained in the Lead_
curve sketch as a lead curve.
27
6. Calculate and Simulate the
Operation.
Exercise 4:
5-axis MachiningSolidCAM2005 Milling Manual
1. Load the SolidWorks document: Exercises\Cut_control\cone.sldprt
2. Create a new CAM-Part. Use the Fanuc_5x CNC controller.
3. Define the CoordSys on the top face of the model.
4. Start a new 5-axis Operation and choose the Cuts Along Curve strategy.
5. Define the internal face of the manifold as the Drive Surface and the sketch
segment containd in the Center_line sketch as a Lead curve.
28
5-axis Machining
SolidCAM2005 Milling Manual
6. Calculate and Simulate the Operation.
The simulation can be performed using either 3D or HostCAD simulation
modes.
29
5-axis MachiningSolidCAM2005 Milling Manual
First curve
Tool path
Second curve
6.2.3 Morph between two curves
The Morph between two curves option will create swarf cuts morphing between two leading curves.
This option is very suitable for machining steep areas for mould making. The more accurate the
guiding curves are to the real surface edges, the better this function works.
To select the first (upper) and second (lower) curve, click on the Upper and Lower button.
30
5-axis Machining
Upper Edge curve
Lower Edge curve
It is very important to define the geometry for the
Upper and Lower Edge curves correctly. SolidCAM
generates the tool path from the Upper Edge curve
till the Lower Edge curve.
It is recommended to select
the edges of the surface as the
geometry of the Upper and
Lower Edge curves. SolidCAM
will check the distance from
the curve to the surface and if
the distance is bigger than 0.03
and the option that moves the
tool exactly on the edges of
the surface is used, tool jumps can result. The reason for these jumps is that
SolidCAM did not find a point on the surface after creating a circle with the
tolerance size on a plane normal to the point on the curve.
SolidCAM2005 Milling Manual
31
Exercise 5:
5-axis MachiningSolidCAM2005 Milling Manual
1. Load the CAM-Part: Exercises\Cut_control\air_console.prt
2. Create a new 5-Axis Operation using the Morph between two curves strategy.
3. Define the Drive Surface as shown.
4. Select the model edge for the
Upper Edge curve geometry as
shown.
32
5-axis Machining
SolidCAM2005 Milling Manual
5. Select the model edge for the Lower Edge curve geometry as shown.
Make a note to select the short edge as shown.
6. Save, Calculate and Simulate the operation.
33
Exercise 6:
5-axis MachiningSolidCAM2005 Milling Manual
1. Load the CAM-Part: Exercises\Cut_control\impeller.prt
2. Create a new 5-Axis Operation using the Morph between two curves strategy.
This option is used due to the inequality of the distance between the upper and
lower curves of the blade.
3. Define the Drive Surface as shown.
4. Select the model edge
for the Upper Edge
curve geometry as
shown.
Make a note to select the geometry accurately without gaps. The accurate
selection results in a more accurate tool path without tool jumps.
34
5-axis Machining
SolidCAM2005 Milling Manual
5. Select the model edge for the Lower Edge curve geometry as shown.
Select the short edge as shown - the absence of this edge in the geometry
causes an inaccurate tool path.
35
6. Save, Calculate and Simulate the
operation.
6.2.4 Parallel to curve
Curve
Tool path
The Parallel to curve option will align the cut direction along a leading curve.
5-axis MachiningSolidCAM2005 Milling Manual
Click Single Edge and select the curve.
36
5-axis Machining
Exercise 7:
SolidCAM2005 Milling Manual
1. Load the CAM-Part: Exercises\Cut_control\air_console.prt.
2. Create a new 5-Axis Operation using
the Parallel to curve strategy.
3. Define the Drive Surface as shown.
4. Select the model edge as shown
as the Curve geometry.
5. Save, calculate and simulate the
operation.
37
Exercise 8:
5-axis MachiningSolidCAM2005 Milling Manual
1. Load the CAM-Part: Exercises\Cut_control\impeller.prt
2. Create a new 5-Axis Operation using the Parallel to curve strategy.
3. Define the Drive Surface as shown.
4. Select the model edge for the Lower Edge curve geometry as shown.
38
5-axis Machining
SolidCAM2005 Milling Manual
Select the short edge as shown - the absence of this edge in the geometry causes
an inaccurate tool path.
5. Save, calculate and simulate the operation.
39
6.2.5 Project curves
Curve & Tool path
Project curves generates a single tool path along a curve.
Click on the Projection curve button to define a curve.
5-axis MachiningSolidCAM2005 Milling Manual
The projected curve is a result of the projection
of the specified curve onto the selected surface.
SolidCAM will not check the curve against the
surface to check if it is a good curve. The calculation
algorithm tries to retrieve the vector to each point
of the curve according to the surface normal in this
point. If the point is not on the surface the point
will be eliminated from the tool path and handled
like a gap.
The tool will move with the center on the selected
geometry. It is not possible to get the tool path in the
left or the right side.
40
5-axis Machining
Exercise 9:
SolidCAM2005 Milling Manual
1. Load the CAM-Part: Exercises\Cut_control\Solidcam.prt.
2. Create a new 5-Axis Operation using the Project curves strategy.
3. Define the Drive Surface as shown.
41
5-axis MachiningSolidCAM2005 Milling Manual
4. Select the model edges of the text for the Projection curves geometry as
shown.
5. Save, calculate and simulate the operation.
42
5-axis Machining
Exercise 10:
SolidCAM2005 Milling Manual
1. Load the CAM-Part: Exercises\Cut_control\3D_engraving.prt.
2. Create a new 5-Axis Operation using the
3. Define the Drive Surface as shown.
Project curves strategy.
43
5-axis MachiningSolidCAM2005 Milling Manual
4. Select the curve in the middle of the surface as the Projected curve geometry.
This curve has to be created in the middle of the selected face and projected on
the surface or created exactly on the surface.
5. Save, calculate and simulate the operation.
44
5-axis Machining
Drive surface
Upper edge surf
ace
Lower edge surface
6.2.6 Morph between two surfaces
SolidCAM2005 Milling Manual
This option is similar to the Morph between
two curves
option. SolidCAM will create
tool path morphing between two leading
curves. In contrast to the Morph between
two curves
option where the leading curves
are directly selected on the model, the
Morph between two surface option enables
you to choose two surfaces adjacent to the
drive surface. The common boundaries of
these surfaces and the drive surface will be
used as the leading curves.
For proper machining, the Calc based on tool center option must be enabled.
If the calculation is not based on the tool center, a wrong tool path will be
generated. The option is located on the Misc. Parameters page.
45
Exercise 11:
5-axis MachiningSolidCAM2005 Milling Manual
1. Load the CAM-Part: Exercises\Cut_control\insert.prt.
2. Create a new 5-Axis Operation using the Morph between two surfaces strategy.
3. Define the Drive Surface as shown.
46
5-axis Machining
SolidCAM2005 Milling Manual
4. Select the upper fillet as shown to define the Upper Edge surface geometry.
5. Select the lower fillet as shown to define the Lower Edge surface geometry.
47
6. Save, calculate and simulate the
operation.
Exercise 12:
5-axis MachiningSolidCAM2005 Milling Manual
1. Load the CAM-Part: Exercises\Cut_control\air_console.prt.
2. Create a new 5-Axis Operation using the
3. Define the Drive Surface as
shown. Select all the tangential
side faces of the pocket.
4. Select all the adjacent top faces
as shown to define the Upper
Edge surface geometry.
Morph between two surfaces strategy.
48
5-axis Machining
SolidCAM2005 Milling Manual
5. Select all the faces of the lower fillet as shown to define the Lower Edge surface
geometry.
6. Save, calculate and simulate the operation.
49
6.2.7 Parallel to surface
Edge surface
Drive surface
5-axis MachiningSolidCAM2005 Milling Manual
This option is similar to the Parallel to curve option. SolidCAM will align the cut direction along a
leading curve. In contrast to the Parallel to curve option where the leading curve was directly selected
on the model, the Parallel to surface option enables you to choose the surface adjacent to the drive
surface. The common boundary of this surface and the drive surface will be used as the leading
curve.
50
5-axis Machining
Margin
Tool center
Margin
You can work with margins. The tool has to be a sphere mill and the Calc based on tool center option
has to be activated in the Misc. Parameters page.
SolidCAM2005 Milling Manual
51
Exercise 13:
5-axis MachiningSolidCAM2005 Milling Manual
1. Load the CAM-Part: Exercises\Cut_control\insert.prt.
2. Create a new 5-Axis Operation using the Parallel to surface strategy.
3. Define the Drive Surface as shown.
52
5-axis Machining
SolidCAM2005 Milling Manual
4. Select the lower fillet as shown to define the Single Edge surface geometry.
5. Switch to the Finish parameters page and set the Step Over to 5.
6. Save, calculate and simulate the operation.
53
SolidCAM finds the common edges between the drive and edge surfaces and
defines the leading curve for the tool path. The tool path is a result of the offset
of the leading curve along the drive surface. The jumps in the top side of the
face are created because SolidCAM did not find a vector from the surface in the
geometry point. All these points are eliminated and the gap control handles this
gap in a later step of the calculation.
5-axis MachiningSolidCAM2005 Milling Manual
6.3 Flip Stepover
Flip step over changes the start cutting direction. This can change the machining direction from the
outside to the inside or from the left to the right.
The machining begins at the top of the
workpiece.
With the Flip Step over option the machining
begins at the edge.
54
5-axis Machining
Exercise 14:
SolidCAM2005 Milling Manual
1. Load the CAM-Part: Exercises\Cut_control\insert.prt prepared in Exercise 11.
2. In the Geometry page make sure that the Flip step over checkbox
is not activated.
3. Simulate the Operation. During the simulation, note that the cutting is performed
from the upper boundary of the drive surface downwards.
4. Activate the Flip step over checkbox.
55
5. Save, calculate and simulate the Operation. Note that the cutting direction was
changed: the cutting was performed from the lower boundary of the drive surface
upwards.
6. Do not close the CAM-Part.
6.4 Cutting Method
5-axis MachiningSolidCAM2005 Milling Manual
SolidCAM enables you to choose the following Cutting methods:
• One way
• Zig Zag
If you have a closed geometry and you select one way machining, the tool will always move around
the part in the same direction.
One Way Zig Zag
56
5-axis Machining
SolidCAM2005 Milling Manual
If the geometry is not completely closed, then it is recommended to set the option
Enforce closed contours.
57
6.5 Cut Order
5-axis MachiningSolidCAM2005 Milling Manual
In the cut order menu you can choose between three options:
• Standard - Sets a default cut order.
• From Center Away - The machining begins in the center of the surface.
58
5-axis Machining
• From outside to center - The machining begins from outside the surface.
SolidCAM2005 Milling Manual
59
Exercise 15:
5-axis MachiningSolidCAM2005 Milling Manual
1. Use the CAM-Part prepared in Exercise 14.
2. Edit the 5-axis operation.
3. Make sure that the Flip step over checkbox is not active in the Geometry page.
4. Set the Cut order to the From center away option.
5. Calculate and simulate the operation. You will see that the tool path starts from
the center and moves sequentially one step up and one step down.
60
5-axis Machining
SolidCAM2005 Milling Manual
6. Set the Cut order to the From outside to center option.
7. Calculate and simulate the operation. As you can see the tool path starts from the
top, moves to the bottom and then moves to the second top and so on.
8. Do not close the CAM-Part.
61
6.6 Direction for One Way machining
5-axis MachiningSolidCAM2005 Milling Manual
This option is available only for the One way Cutting method.
The Clockwise and Counter clockwise options are not for the spindle rotation. They are used
to determine whether the tool should move around a closed surface model in clockwise or
counter clockwise direction.
• Ccwise
This option enables you to perform the machining in counter clockwise direction.
62
5-axis Machining
Tool movement direction
Tool rotation
Tool movement direction
Tool rotation
• Cwise
This option enables you to perform the machining in
clockwise direction.
SolidCAM2005 Milling Manual
• Climb
The tool movement and the tool rotation have the
same direction.
Climb milling is preferred when milling heat treated
alloys. Otherwise chipping can result when milling
hot rolled materials due to the hardened layer on the
surface.
• Conventional
The tool movement is opposite to the tool rotation.
Conventional milling is preferred for milling of
castings or forgings with very rough surfaces.
63
Exercise 16:
5-axis MachiningSolidCAM2005 Milling Manual
1. Use the CAM-Part prepared in Exercise 15.
2. Edit the 5-axis operation.
3. Switch to the Geometry page and choose the Cwise for the Direction for one way
machining option.
4. Calculate and simulate the operation. As you can see the tool path works in the
opposite direction. When the tool path is normal to the surface, it is not so clear
what is the conventional or climb milling direction. So you can use the CW or
CCW to get the requested tool path direction.
64
5-axis Machining
Edge
Edge
6.7 Cutting Area
SolidCAM2005 Milling Manual
SolidCAM enables you to choose the following options for the Cutting area:
• Full, start and end at exact surface edge
If this option is chosen, the tool path
will be generated on the whole surface
and exactly to the surface edge or to the
nearest possible position.
Simulate the appropriate operation of
Exercise18. The CAM-Part is located in
the Exercises/Cutting_area folder.
65
• Full, avoid cuts at exact edges
Edge
Edge
Point 1
Point 2
With this option the tool path will be generated on
the whole surface but avoids the surface edges.
Simulate the appropriate operation of Exercise18.
The CAM-Part located in the Exercises/Cutting_
area folder.
5-axis MachiningSolidCAM2005 Milling Manual
• Limit cuts by one or two points
This option enables you to limit the machining
between one or two points. The Data button
displays the Limit cuts between two points dialog.
This dialog enables you to define point coordinates
or pick the points from the workplane.
Simulate the appropriate operation
of Exercise18. The CAM-Part is
located in the Exercises/Cutting_
area folder.
66
5-axis Machining
Exercise 17:
SolidCAM2005 Milling Manual
1. Use the CAM-Part prepared in Exercise 16.
2. Edit the 5-axis operation.
3. Simulate the operation. Note that the tool path does not reach the edges of the
drive surface because of the Cutting area option. This option is set to Full, avoid
cuts at exact edges.
4. Switch to the
and end at exact surface edges.
Geometry page and set the Cutting area option to the Full, start
67
5-axis MachiningSolidCAM2005 Milling Manual
5. Calculate and simulate the operation. Note that the first and last cutsare performed
exactly on the drive surface edges.
68
5-axis Machining
SolidCAM2005 Milling Manual
6.8 Start Point
Examples of the Start Point option are located in the Exercises\Start_Point folder.
The Start point option enables you to choose a new start point where the machining begins. Depending
on the geometry, 5axmsurf tries to find the nearest possible position next to your point.
With the Rotate by option you can relocate the start position for the following cut. The coordinates
will be calculated with the stepover and the angle you set.
Click on the Data button. In this window you can enter X, Y and Z coordinates for your new point or
select a point in your geometry.
69
5-axis MachiningSolidCAM2005 Milling Manual
Original start point
New start point
20°
20
°
20
°
Start points
Default tool path start position Tool path start position with new start point
This is a tool path start position with a new start point and a 20 degrees rotation angle.
Simlate operations of Exercise4 . The CAM-Part is located in the Exercises\Start_Point folder.
70
5-axis Machining
7. Finish Parameters page:
SolidCAM2005 Milling Manual
71
5-axis MachiningSolidCAM2005 Milling Manual
Radius
Move direction
Center
Front
7.1 Tool Contact point
Examples of the Tool Contact point option are located in the Exercises\Tool_Contact_point folder.
This parameter defines the contact point of the tool and drive surfaces. At a surface point with a given
surface normal direction, the tool can always be placed tangentially.
You can see the touching points in the above picture.
Center is exactly in the middle of the tool. Front
is the point where the flat part of the tool ends and the radius starts, but only in the move direction.
Radius is every point on the round radius surface.
72
5-axis Machining
Tool Center
Move direction
Tool Path
Tool Radius
Move direction
If this parameter is set to AT CENTER, then the tip of the tool touches the surface’s
contact point. If the tool axis orientation is changed due to tilting options, then the tool
will be tilted around this tip point. In such a case, the tool and surface are not tangential
anymore and the tool will gouge the surface. This situation must be avoided by setting the
first gouge check strategy to retract the tool from the drive surfaces.
SolidCAM2005 Milling Manual
AT CENTER
AT RADIUS
If this parameter is set to AT RADIUS, then the tangentiality is maintained like in the case
of AUTO, the difference is that for a bull nose tool, the tip of the tool is never used as the
touch point on the drive surfaces.
73
5-axis MachiningSolidCAM2005 Milling Manual
Tool Front
Move direction
Touch points
Move direction
AT FRONT
The option AT FRONT is similar to AT CENTER and forces the tool touching point to be
always a fixed point on the tool. In this case, this fixed point is the beginning of the radius
of a bull nose tool in the direction of the tool motion. All changes to the tool orientation
are done around this pivot point which can cause gouging of the drive surfaces. Setting the
gouge control is critical when working with this option.
If the AUTO option is chosen, the tool can be placed tangentially at a surface point with
a given surface normal direction. If the user changes the orientation of the tool, then the
surface contact point remains and the contact point on the tool moves from the tip of the
tool to the radius of the tool still maintaining the tangentiality between the tool and the
surface.
Simulate the operations of
Exercise13. The CAM-Part is
located in the Exercises\Tool_
Contact_point folder.
AUTO
74
5-axis Machining
Exercise 18:
SolidCAM2005 Milling Manual
1. Load the CAM-Part: Exercises\Tool_Contact_point\blade.prt.
2. Simulate the CAM-Part. This part is machined
using the 4 axis CNC machine. The blade is
twisted and if the tool is positioned tangentially
to the surface, the tool path will not be parallel.
It is possible to define a parallel tool path by
using the Run tool option.
3. Edit the 5-axis operation and switch to the
Finish parameters page.
4. Set the Tool Contact point option to At center.
75
5-axis MachiningSolidCAM2005 Milling Manual
5. Calculate and simulate the operation. It is recommended to use 3D simulation
mode to perform the simulation of the tool path with the tool displayed.
The tool center is coincident
to the drive surface along the
whole length of the tool path.
This causes gouges, so this
option has to be used together
with the gouge control options.
76
5-axis Machining
SolidCAM2005 Milling Manual
6. If a flat tool is used for rough face milling, the At Front option enables you to mill
the front part of the tool. Change the Tool Contact point option to At Front.
7. Calculate and simulate the operation. It is recommended to use the 3D simulation
mode to perform the simulation of the tool path with the tool displayed.
The front of the tool is placed on the point and the angle results from the vector
of this point. (Later on we will see how we can tilt the tool more in the cutting
direction to get better cutting conditions).
8. To use the At radius option we have to define the tool with corner radius for the
operation. Change the Corner Radius to 2.
77
5-axis MachiningSolidCAM2005 Milling Manual
9. Set the Tool Contact point option to At radius.
10. Calculate and simulate the operation. It is recommended to use the 3D simulation
mode to perform the simulation of the tool path with the tool displayed. Note
that the tool corner radius is tangent to the drive surface along the whole length
of the tool path.
Make a note that the corner radius of the tool is tangent to the surface. Note that
the tool path is not parallel because SolidCAM tries to put the radius tangential
to the surface normal.
78
5-axis Machining
7.2 Lead in / Lead out
SolidCAM2005 Milling Manual
This switch turns on and off the tangential entry and exit moves.
The Lead in / Lead out dialog enables you to define the parameters of Lead in / Lead out.
79
5-axis MachiningSolidCAM2005 Milling Manual
Tool path
Lead in arc
Arc sweep
Lead in point
Tool Path
Tool Path
Lead out
Lead in
Lead in
90°
Lead in/Lead out– These checkboxes enable you to define the lead in/out. The approach/retreat
movements are performed by an arc with the following parameters:
Arc sweep – The sweep angle of the lead in/out arc from the entry point on the tool path.
Arc diameter / Tool diameter % - This parameter specifies the ratio of the lead in/out arc diameter to
the tool diameter.
Don’t plunge with tool
This option enables you to perform
the arc approach in the plane normal
to the tool vector in the entry point.
80
5-axis Machining
Tool Path
Tool Path
90°
90°
Lead in
Lead in
Lead in
Lead out
SolidCAM2005 Milling Manual
When this option is not chosen, the approach arc plane will be normal to the previous plane.
81
Exercise 19:
Drive surface
Upper edge surface
Lower edge surface
5-axis MachiningSolidCAM2005 Milling Manual
1. Load the CAM-Part Exercises\Lead_in_Lead_out\insert.prt
Now we will see how to use the entry and exit arc moves.
2. Set the following parameters in the Finish page.
Choose the Morph between 2 surfaces option in the Cut Control field.
Choose the Drive, Upper edge and Lower edge surface as shown.
82
5-axis Machining
SolidCAM2005 Milling Manual
Choose the Zigzag option in the Cutting method field.
Choose the Standard option in the Cut Order field.
3. Switch to the
Finish parameters page and set the following parameters:
Set the Step Over value to 3.
4. Activate the Lead in/Lead out checkbox and click on the Lead in/Lead out button
in order to define the Lead in/Lead out parameters.
83
5-axis MachiningSolidCAM2005 Milling Manual
5. In the Lead in/Lead out dialog activate both the Lead in and Lead out sections.
Set the Arc Sweep to 90 and Arc diameter/Tool diameter to 200 in both
sections.
6. Switch to the
Gaps page and set the following parameters:
84
5-axis Machining
SolidCAM2005 Milling Manual
7. Calculate and simulate the operation.
As you can see, the entry and exit movements are performed by arcs. The arc size
is double the tool radius.
The arcs are parallel to the tool path direction in the entry point.
8. Display the Lead in/Lead out dialog and activate the Plunge with Z-Axis option.
9. Calculate and simulate the operation.
As you can see the entry and exit arc are
rotated
90 degrees and are now normal
to the tool path direction in the Lead
in/Lead out point.
85
Exercise 20:
5-axis MachiningSolidCAM2005 Milling Manual
1. Load the CAM-Part Exercises\Lead_in_Lead_out\Undercut.prt
We will now see how the gouge checking affects the entry and exit arcs.
2. Start a new 5-axis Operation and choose Tool #1 from the Part Tool table.
3. Set the following parameters in the Geometry page:
Choose the Parallel Cuts option for the Cut Control.
Click on the Constant Z button to define the Machining Angle.
Choose the One Way option in the Cutting Method field.
86
5-axis Machining
SolidCAM2005 Milling Manual
4. Define the Drive surface as shown below.
5. Switch to the Finish parameters page and set the following parameters:
Set Step Over to 6.
Check the Lead in/Lead out checkbox.
87
5-axis MachiningSolidCAM2005 Milling Manual
6. Switch to the Gouge check page and define the following parameters:
Activate the Enable/Disable checkbox.
Inactivate the Check surfaces option.
In the Strategy field, choose the Tilting tool away with max. angle option.
The Gouge check options will be explained later.
7. Switch to the Gouge 2 page and define the following parameters:
Activate the Enable/Disable checkbox.
Inactivate the Drive surfaces option.
88
5-axis Machining
Check surfaces
SolidCAM2005 Milling Manual
8. Define the Check surfaces as shown below.
The chosen strategy enables the user to avoid gouging by retracting the tool along
the tool axis.
89
9. Switch to the
Tool Axis Control page.
5-axis MachiningSolidCAM2005 Milling Manual
10. Set the following options:
Choose the Tilted relative to cutting direction option in the Tool axis direction
combo-box.
Set the Tilt angle at side of cutting direction value to 90.
Choose the Follow surface iso direction option in the Side tilt direction combobox.
11. Calculate and simulate the operation.
90
5-axis Machining
SolidCAM2005 Milling Manual
We can see arcs in every tool path depth in the right side approach and only one
in the left side. This is because the gouge check sees that the tool will gouge to
the left wall and moves the tool along the vector of the tool center till this gouge
is finished. In this part all the paths move to a safe point (in the same point in
this part) and then adds the exit arc. The gouge algorithm and the Entry/Exit
algorithms protect the part from gouging.
12. Close the simulation.
13. Choose the Leaving out gouging points option in the Strategy field of the Gouge
check page.
14. Calculate and simulate the operation.
As you can see the arc is mirrored and moved
out from the corner and the part is gouge
protected.
91
7.3 Round surface by tool radius
5-axis MachiningSolidCAM2005 Milling Manual
This switch can be set to find small radius areas and inner sharp edges in the surface model. Such areas
will be left out from the tool path generation. Inside corners can cause “fish tails” in tool paths. Such
fish tails are removed by turning on this switch. This flag can also be considered as a fillet generator.
The surface model is rounded (filletted) in the direction of tool path slices with a radius to avoid small
radii and inner sharp corners. The applied radius is the main tool radius plus the current stock to leave
value. The fillet generation is independent of the tool type and shape. In most cases, this switch is used
in the presence of a ball cutter, lollipop cutter or a conical cutter with a ball tip. If swarf machining is
applied (side cutting), then also cylinder or torus cutters are used together with this switch.
The Round surface by tool radius option is not active.
92
5-axis Machining
The Round surface by tool radius option is active.
SolidCAM2005 Milling Manual
93
5-axis MachiningSolidCAM2005 Milling Manual
Stock to leave
7.4 Stock to leave
The Stock to leave parameter describes the stock to be left on the finishing surfaces. This parameter
can also be negative, e.g. for cutting electrodes.
For example, if this value is set to 0.2 units, then the tool will not come closer than 0.2 units to the
surface. Therefore, after the machining, there will be remaining stock on the surface of about 0.2
units.
Simulate the operations of
Exercise14. The CAM-Part is located in the Exercises\Stock_to_leave
folder.
94
5-axis Machining
7.5 Multi Passes
SolidCAM2005 Milling Manual
This switch can be turned on to calculate multiple tool path passes on the same geometry.
The Multi passes dialog enables you to define the following parameters:
The Roughing passes section enables you to define a number of rough passes (specified by the
Number parameter) with the specified spacing (the Spacing parameter) between them.
The Finishing passes section enables you to define a number of finishing passes.
95
5-axis MachiningSolidCAM2005 Milling Manual
Without the Constant Stepover option
With the Constant Stepover option
1
2 3
4
1
2
3
4
pass
pass
pass
pass
With Constant Stepover Without Constant Stepover
pass pass pass pass
Constant step over at each pass – this option enables you to define the order of execution of the
roughing and finish passes.
When this option is turned off, all the rough and finish passes will be done at the current height level
before moving to the next height level. When the Constant step over at each pass option is not
selected; each pass will be finished for all height levels before moving to the next pass.
Simulate Exercise16. The CAM-Part is located in the Exercises\Multi_Passes folder.
96
5-axis Machining
7.6 Surface Quality
7.6.1 Chaining Tolerance
SolidCAM2005 Milling Manual
The chaining tolerance is an internal value for the tool path generation and should be 1 to 10 times the
cut tolerance. If you have untrimmed simple surfaces, then this value can be set to 100 times of the
cut tolerance and will increase the calculation speed drastically.
Using higher values in the chaining tolerance can cause inaccuracies. The tool path will not be as good,
but the calculation time will be faster.
Simulate
Exercise5. The CAM-Part is located in the Exercises\Chaining_tolerance.
97
5-axis MachiningSolidCAM2005 Milling Manual
7.6.2 Cut tolerance
The Cut tolerance is the tolerance for the accuracy of the tool path. A tight Cut tolerance gives you
more tool path points on the drive surface. Therefore the generated tool path is more accurate. The
result of the machining is a very good surface quality but the calculation time is increased.
A loose Cut tolerance generates less points on the tool path. After the machining, the surface is
rougher but the calculation time is much faster.
Loose Cut tolerance Tight Cut tolerance
98
5-axis Machining
7.6.3 Distance
SolidCAM2005 Milling Manual
Whether you have more or less points depends on the Cut tolerance. You have more points on
round surfaces because the tool path always changes direction. Use the Distance option to get more
points on flat surfaces. Although the Cut tolerance is the same you get more points on straight or flat
surfaces. Setting a small value gives more points whereas a high value gives fewer points.
Result without distance Result with distance
99
7.6.4 Stepover
The Stepover is the distance between two neighboring parallel cuts.
5-axis MachiningSolidCAM2005 Milling Manual
Small stepover
Big Stepover
100
Loading...