CAM Tips & Techniques
Tips & Techniques are provided here and throughout
the documentation. They
provide useful information and guidance that can help you take full advantage
of VX CAM and its advanced features.
Many of these are hypertext links (blue text) that jump to other help pages that contain the "Tips & Techniques" box. You may have to expand one or more drop down topics to locate the box on that page. Others are links (green text) that drop-down (i.e., expand) the current page when selected and then collapse when selected again.
How to run third party post processors from PostWorks inside of VX CAM
Use the following procedure to run third party post-processors from PostWorks inside of VX CAM.
In the CAM Plan Manager, right-click on the machine to modify in the manager tree and select Edit from the popup menu. This will display the CAM Machine Manager.
Pick Programming to display the Machine Programming Details Form.
Pick Post Processor and select pworks from the list of supported post processors.
Pick OK from the CAM Machine Manager and then close the form (both forms will close).
In the manager tree right-click on Output and select Edit from the popup menu. This will display the Output Form.
Select the operation to output and then pick the Document tab.
Complete the form as desired making sure to enter the output file name and place a check in the box next to Display Output.
Pick G and M Codes and the NC Program Window will display the G and M codes output for the selected operation. The output file will be created automatically via the PostWorks post processor.
The default directory, in which the PostWorks
software is installed, is "C:\nccs\postworks\bin."
If you installed PostWorks in a different directory, you need to modify
the "runpost.bat" file
and change PWORKS_PATH accordingly.
Do not use any <space>
characters in output names or directory names when third party post processors
are used.
How to output spindle speed in decimal format
You can choose to output
spindle speed in decimal format. Perform
the following steps to do so.
First make a backup copy of the post processor configuration file "fanuc10.fp" located in the "output_def" folder of your VX installation folder (e.g., fanuc10_bak.fp).
Next, edit
the "fanuc10.fp" file
to change the SPINDLE_SPEED_DECIMAL
flag to "TRUE." By
default this flag is set to "FALSE."
This flag
is located under the "General Settings"
section of the file. See
below.
# General settings.
SPINDLE_SPEED_DECIMAL:TRUE
DECIMAL_PLACES:3
LEADING_ZEROS:FALSE
TRAILING_ZEROS:FALSE
ARCCENTERMODE:INCRFROMSTARTPT
How to choose among drill, bore and ream operations
Drilling is always the
first to choose from as long as it meets your tolerance requirements.
If higher tolerance is required, consider reaming next for smaller holes
(less than 1 inch in diameter). Reaming is considered over boring because
it is easier and more economic to perform. Boring should be considered
for relative large holes only.
How to select profile curves for CAM containments
Cam containments can
be open or closed but must be selected in a strict order to determine
if machining is on the left or right side. Please use chain picking cautiously
to define containments since chain pick inputs curves are not orderly.
For closed
profiles, pick the curves in a COUNTER CLOCKWISE direction to define material
as being inside the profile (i.e., as you march along the profile curves,
material is always on your left hand side).
Use Caution
with the "Enhance Corners" parameter in QuickMilling operations
Gouging and Collision avoidance'
A collision is when the cutter body (or holder)
collides with other geometry in the CAM plan. A
gouge is a local occurrence as the cutting part of the tool cuts deeper
into the part than is intended. For
Intelligent hole making and 2-1/2 axis hole operations, gouge checking
can be enabled or disabled from the operation definition forms.
Collision avoidance will occur automatically with all geometry contained in the features list for the operation including tool holder/attachments and stock/fixtures. For all other operations, gouge and collision will be checked and avoided automatically with all geometry contained in the features list for the operation.
Quick and dirty QuickMilling test run
VX CAM is so easy to use that you can perform
a quick and dirty QuickMilling test run in just a few simple steps.
Build a simple part.
Open a CAM Plan.
Click on Geometry > pick your part from the browser > YES.
Click on OPERATIONS > Q-Mill (tab) > LACE (Finish pass).
<Right click> on Tool > Manage > OK > Close (this will use a default tool).
Click on FEATURES.
Click on your part above (This adds your part as a feature).
<Right click> on Lace 1 > Calculate.
See Basic CAM Walk Through for a more in-depth look at VX CAM and Applying VX CAM for additional techniques.
Machining compound holes with Intelligent Hole Making
You can use Intelligent Hole Making to machine compound holes such as counter-bore-sink holes or counter-sink-bore holes. Just use the CAM Feature Manager to define the compound holes by selecting multiple holes consisting of arcs or cylinders. VX will auto-detect possible compound holes and find all the necessary tools from the tool library to machine them.
Detect tool body collisions
Recommended "% First Step" parameters for QuickMilling operations
Using "Min Rest Height" for 3D limiting in QuickMilling Operations
Generate swarf cut tool path without limitation on tilt angle and using skew angle
File name characters not supported by the OS
When you ask for file names to be named after
individual operations VX CAM checks for characters not supported in file
names by the OS such as " * / \
: < > ? |. If
any are found you are asked if substituting "_" is OK. If
not, the output process is halted and you're instructed about what do.
