KeyCreator NC 3 Axis Tutorial

KEYCREATOR NC provides multiple surface and solid tool path generation
and post processing for 2 and 3 axis applications. For this tutorial we’ll
investigate 3 axis capabilities. This tutorial was designed to help you become
familiar with basic 3 axis NC tool path generation and post-processing using
KEYCREATOR. You’ll learn the basic work flow for generating and post
processing a 3 axis tool path. Additionally, you’ll get a chance to look at many
of the 3 axis NC functions and machining strategies used in KEYCREATOR.
KEYCREATOR uses all types of pure geometry (wireframe, solids, and
surfaces) to help define tool paths. The part you’ll be working with
(console.ckd) is a surface model comprised of individual part surfaces. This
tutorial was designed with the assumption that the user has had general
CAD/CAM software experience. It might be a good idea to complete the
KEYCREATOR BASIC TUTORIAL before attempting this tutorial. For
additional information on any of the commands used in this tutorial, please
refer to the KEYCREATOR NC reference material, available for download at
www.kubotekusa.com. Feel free to download the KEYCREATOR NC 2AXIS
TUTORIAL for more NC capabilities.
Get Started - Open and shade the sample part
Open the part, console.ckd that is in the CKD directory of your KEYCREATOR install (or
downloaded with this tutorial). To do that, choose FILE>OPEN from the pull down menus
and browse for console.ckd. Once the part is loaded, type SHIFT+5 (hotkey combination for
shading) to shade the part. The part should be displayed as shown above.
Define Tools
Ball End Mill
Flat End Mill
Diameter
Select
Geometry to
be Machined
Choose
Machining
Method
Generate
Path
Roughing
Finishing
Special
Repeat for
additional tool
paths
Part Geometry
Check Geometry
Containment Boundary
Avoidance areas
Verify
Post-Process
Process the
Tool Path
The four main steps that are followed when creating a tool path with KEYCREATOR are shown
above . Each step is significant to the process and critical information will be defined at each
step. The tutorial will review and identify the importance of each of the steps.
Let’s take a quick look at the NC setup page. Choose TOOLS>NC>PATH>SET UP from the
pull down menus. The setup page contains a few global default parameters that
KEYCREATOR will use to define tool paths. You won’t need to change any of the parameters,
but, it is a good idea to be aware of the usage for each. The table below gives a brief
description of the set up parameters.
TOOL PATH SET UP
PARAMETER
Machining View Number
Clearance Plane
Wall Stock Semi-Finishing
Wall Stock Roughing
Plunge Clearance
Chord Height Tolerance
Filter Output
DESCRIPTION
Defines the machining orientation and is the
view that is normal to the tool axis.
This is a z value, somewhere above the part,
where rapid motion can freely take place.
Thickness of stock to be left behind by finishing
operations.
Thickness of stock to be left behind by roughing
operations.
The z value above the cutting plane where
motion will change from rapid to feed.
Value defining the maximum deviation of the
tool path from the geometry to be machined
Not used.
Step 1 – Define the tools that you will use
Start by defining a tool that you’ll use to machine the part. Choose
TOOLS>NC>PATH>TOOLS from the pull down menus. In the SELECT THE ACTIVE TOOL
dialog box you’ll see a blank tool list. To add a new tool to the list choose DEFINE NEW.
In this tutorial you’ll be defining and post processing a finishing tool path. For this part, use a
10mm ball end mill. In the ADD A NEW TOOL dialog box, set up the parameters shown above
then click OK. Notice the new tool visible in the SELECT THE ACTIVE TOOL dialog box tool
list. By highlighting the tool and clicking DONE, you’ll designate the 10mm ball end mill as the
active tool. Keep in my that a number of tools can be added to this list. Each time a different
tool is needed, return to this dialog to reset the current active tool. Additionally a tool list,
complete with tool definitions, can be saved to a file and retrieved at any time.
Step 2 – Select the geometry
Next, you’ll need to select various geometry that will help you define the tool path. As we
mentioned earlier, wire frame, solid and surface geometry can be used to achieve the
necessary results. There are four different categories of geometry that are defined for
creating a tool path. The categories are PART GEOMETRY, CHECK GEOMETRY,
CONTAINMENT BOUNDARY, and AVOIDANCE BOUNDARY. The table below shows the
different categories and a brief description of each.
GEOMETRY CATEGORY
DESCRIPTION
Part Geometry
Part geometry consists of solid and/or surface
geometry to be machined.
Check geometry consists of solid and/or
surface geometry that the tool will check
against, but not machine. Check geometry can
be used to limit tool motion during machining.
The containment boundary is defined using
curves (wireframe geometry or edges of solids
and surfaces) to define the boundary of the
machining zone.
The avoidance boundary is defined using
curves (wireframe geometry or edges of solids
and surfaces) to define the areas that must be
avoided by the tool during machining.
Check Geometry
Containment Boundary
Avoidance Boundary
For the part that you’ve loaded you’ll need to define PART SURFACES, a CHECK SURFACE
and a CONTAINMENT BOUNDARY. To Start the geometry selection process, choose
TOOLS>NC>PATH>GEOMETERY from the pull down menus. First select the part geometry.
Choose PART FACE in the dialog box. All of the part faces are colored red. KEYCREATOR
allows you to select geometry based on color. This is called entity masking.
On the conversation bar you’ll be prompted to SELECT THE PART FACES. Click ALL DSP
then BY TYPE. In the masking dialog box click the color red and choose OK. All of the
intended (red) part geometry will be highlighted. Click ACCEPT to complete the selection of the
geometry. In the GEOMETRY dialog box you should now see that 149 part faces have been
selected. Next you’ll need to select the CHECK SURFACE. Click on CHECK FACE in the
GEOMETRY dialog box. There is only one CHECK SURFACE that needs to be selected.
Part faces
Check face
On the conversation bar you’ll be prompted to SELECT THE CHECK FACES. Use the cursor
to highlight the CHECK FACE (light blue colored surface) shown above. Click on the
highlighted surface then click on ACCEPT to complete the selection. In the GEOMETRY dialog
box you should now see that one CHECK FACE has been selected.
!
Select four edges of CHECK
SURFACE as CONTAINMENT
BOUNDARY
To complete the selection of necessary geometry, you’ll need to select a CONTAINMENT
BOUNDARY. You can use the edges of the CHECK SURFACE to define the containment
boundary. To select the edges, click on CONTAINMENT in the GEOMETRY dialog. In the
CONTAINMENT BOUNDARY dialog box, choose CENTER OF TOOL as the containment
parameter then click OK. On the conversation bar you will be prompted to SELECT FIRST
BOUNDARY CURVES. Click on SINGLE then highlight and click on each of the four edges
shown above. One the edges have been selected click on ACCEPT to complete the selection
process. You have now selected all of the required geometry to generate a tool path. Click
DONE in the GEOMETRY dialog box to complete the geometry selection process.
Step 3 – Choose the Machining Method
KEYCREATOR offers optional machining strategies for both roughing and finishing of 3D
geometry. For a complete explanation of all roughing and finishing options see the
KEYCREATOR NC user’s guide. For the geometry that you’ve chosen, generate a PLANAR
FINISHING tool path. Start by choosing TOOLS>NC>FINISH>PLANAR from the pull down
menus. In the PLANAR FINISHING dialog box set up the parameters as shown above then
click OK. On the conversation bar you’ll be asked DO YOU WANT TO CREATE TOOL
PATH? Click on YES. The PLANAR FINISHING parameters are on the next page.
"
PLANAR FINISHING
PARAMETER
Part Wall stock
Check Wall Stock
Plunge Clearance
Chord Height Tolerance
Step Over
Cutting Angle
Cut Method
Cut Direction
Step Direction
DESCRIPTION
Thickness of stock to be left behind by finishing
operations (defaults to value set in set up menu
earlier).
Thickness of stock to be left behind by roughing
operations (defaults to value set in set up menu
earlier).
The z value above the cutting plane where motion will
change from rapid to feed (defaults to value set in set
up menu earlier).
Value defining the maximum deviation of the tool path
from the geometry to be machined (defaults to value
set in set up menu earlier).
Spacing between subsequent tool path motions.
An angle that defines cutting direction.
Cut can be uni-directional.. (Feed along a vector then
retract and rapid return) or bi-directional (feed along a
vector, step over then feed along the reverse vector)
The cut direction is a vector that can be defined using
an angle (cutting angle) or two points (user selected).
Can be right or left and is determined by looking in the
cut direction at the start of the tool path.
Rapid motions
(dashed line)
Feed motion
(solid line)
The tool path will be generated based on the information that you have input in the previous
steps. Rapid and feed motions are differentiated by color and line type. Manipulation of the
tool path (delete, copy, rotate) can be done with the tools found in TOOLS>NC>PATH from the
windows pull down menu. Keep this in mind as you continue to become familiar with
KEYCREATOR NC. Remember that you can also find a complete description of each
machining method in the KEYCREATOR NC user’s materiall.
#
Step 4– Post process the tool path
To start post processing the tool path choose TOOLS>NC>PATH>POST from the pull down
menus. On the conversation bar you’ll be prompted to SELECT THE TOOLPATHS. Use the
cursor to highlight the tool path then click to select it. Click ACCEPT. Next you’ll need to select
a post processor that was written for your specific NC controller. There are several post
processors in the KEYCREATOR post processor library, however, if you don’t see the machine
that you are looking for a post processor can be written by KUBOTEK USA tech support for
any NC controller. Choose SELECT POST in the POST PROCESS TOOLPATHS dialog box to
access the post processor library. Choose a post processor from the list and click OPEN.
Once you’ve selected a post processor, you’ll need to name the file and directory that the NC
file will be written to. Click on NC OUTPUT FILE in the POST PROCESS TOOLPATHS dialog
box. Browse for the desired directory, name the file and click SAVE. Next, click OK in the
POST PROCESS TOOLPATHS dialog box.
$
On the conversation bar, you’ll be prompted to INDICATE PART ZERO. This is the position
that you will indicate on your actual part or stock as part zero. In practice it may be a good idea
to include geometry in your file that will define the actual reference position for the piece of
stock or part that you’ll be machining. This geometry could be a point, wireframe block or any
other geometry that will help to define the actual cutting environment. By including this
geometry, the selection of part zero will be simplified. For this tutorial you can select the corner
of the CHECK SURFACE as shown above. To do that, choose CURSOR on the conversation
bar, move the cursor over the corner, then click when the CURSOR SNAP snaps to the END
position.
In the NC FILE PROGRAM LIST dialog box you can view and print a record of the NC program
that you’ve just created. Click VIEW NC FILE to view the file in a text editor
(note pad). Click DONE to complete the process.
This completes the basic tutorial for generating a 3 axis tool path with KEYCREATOR. For
more information refer to the KEYCREATOR NC reference manual, the KEYCREATOR NC 2
AXIS TUTORIAL, or contact your local KEYCREATOR Support Center.