PROFILE TRAINING LESSON:
IMPORTANT:
V21 has a global environmental option that is called, “Auto
Pre-select.” This allows you to draw
geometry whether freehand or by using coordinate values and have the geometry appear
on the CAD screen “selected” and ready to be used for functions that are
considered Object/Action. This simply
allows you to draw shapes and not have to select them first to use a
function. For advanced operators, this
can help save time. In this lesson, we
would like you to turn this option OFF to prevent any discrepancies executing
the steps of this lesson. To do this, go
to the main FILE menu and select ENVIRONMENT.
Choose the DEFAULTS TAB and UN-CHECK the Auto Pre-select button if it is
checked. Now click OK to exit the
dialog.
STEP 1
Start this
lesson with a NEW CAD drawing screen.
Go to the
OTHER menu and select RECTANGLE. Select
Bottom Left under the section called, “Mode.”
Select Fillet as the Corner Type and enter .25 as the radius. We will be using the bottom left corner of the rectangle as our point of reference. Now enter 1 for X, 1 for Y and leave the Z
value set at 0.
Now, go
ahead and enter a width of 5 and a height of 5.
This is going to be a basic square shape with radius corners.
Now click
OK to draw the shape.
STEP 2
Now we are
going to draw a point on the screen to indicate our start position for the
tools approach into the profile cut.
This is not mandatory for profiling.
However it is a new option that we need you to be aware of.
Go to the
POINT menu and select COORDINATES. In
the box that appears, enter 2 for X and leave Y and Z at 0. Click OK to draw the point.
STEP 3
Now go to
the Special/NC CAM main menu and select INSERT NC. This opens the Insert NC Data box and is
where you will select the post processor.
For this lesson select the FANUC 6M configuration and click OK to open
the
NOTE: If your CAD window splits into 2 or more CAD
windows it is because you opened a new file without fully closing out the last
window. Simply use the Maximize option
in the upper right corner of the CAD window we are working in. This is the middle, square looking button.
This will
open the drawing window that we are working in to full view. Now select the VIEW ALL icon from the main
CAD toolbar. This is the small
magnifying glass with the letter, “A” inside of it.
STEP 4
Go to the
Now click
OK to insert this data into the NC Editor.
The NC Editor is similar to a standard word processor allowing you to
type in it and make editing changes manually as needed. This is where the entire program is
generated.
STEP 5
Select the
MACHINE menu from the
The profile
box will automatically appear asking you if you would like to pick your own
lead-in/lead-out point for this profile or not.
Because we drew a start point for this we will select YES.
The
“Default point” referred to in this box will be the starting point of the line
you clicked on if you were to choose NO.
In any case, select the YES button.
Go directly
to the point that you created and click on it to open the Tool Depth Settings
box.
STEP 6
Have a look
at this new box.
Under Tool
Position Z you have your Rapid Plane.
Enter .1 for this as it represents the tools clearance above the part
during rapid moves. Your material top
for this part if 0 and the CUTTING DEPTH is -.25. We are not going to be roughing this profile
so do NOT check the Enable option under Automatic Roughing. In the FEED section enter F5 for
Now select
NEXT.
STEP 7
Now you
will have the Profile Milling command box.
Let’s take a brief break from this lesson and have a look at this box.
The Profile
Milling command box gives you control over the following:
- The tool diameter that you will be using. Everything in this box is associative,
meaning that if you make a change, the preview will reflect the changes
made. If you change the size of the
tools diameter and hit your enter key the preview will reflect this
modification.
- The tool compensation. By
choosing Automatic, you can use
the right or left options in this box and the software will automatically
create an offset on the left side or right side of the original
geometry. The lead-in and lead-out
will be added to this offset unless you select the “Straight Plunge”
option. Basically, the software
does the offset for you based on half the distance of the size tool you
use. By choosing Machine G41/42 you are telling the
software that you would prefer to cut the original profile geometry using
right or left compensation (G41 or G42) and that this G41 or G42 code will
be added to the g-code program created in BobCAD. By choosing NONE you are indicating that you are not going to use
compensation at all and will be using the drawn geometry for cutting with
the center of the tool being used.
This is the same as using the Auto Cut function in BobCAD and
whatever you have selected in the Contour menu will be added to the
code.
This is important to understand when
using these options. Some post
processors are setup differently when
it comes to the Contour menu in the
If you have something selected in
the contour menu and use the profile wizard for compensation, the profile wizard will over ride this menu
command unless you select NONE in the comp section of the profile wizard. Therefore, you should check the contour menu
in the
Here it is again. If you use a comp option in the contour menu
and choose NONE in the profile wizard, the
option selected in the contour menu will be used when the software creates the
g-code program. If you use compensation in the profile wizard it
will over ride the option selected in the contour menu. It’s that
simple.
You see, you do not always have to
use the profile wizard for profiling in BobCAD.
You can simply create manual
offsets for your tool (half the distance of the tool size), use the Tool Depth
Settings and then the Auto Cut function
in the machine menu along with the comp option you need selected in the contour menu if your post processor
configuration supports it.
Just remember one important thing,
when you are using G41 or G42 comp from the CONTOUR menu and will be using the Auto Cut option, you
will want to create a lead-in and lead-out manually by using the approach/depart function from the
OTHER menu of the software.
- Compensation Direction. You have two options, Right and
Left.
- Lead-In/Out. This section offers you a circular/radial approach and
depart or an angled line approach and departure for your tool. The radius value allows you to adjust
the overall radial approach as well as the departure and the “Distance”
option offers you the ability to shorten or extend the length of the
approach and departure of the tool.
Here’s an example of the Circular approach and departure below.
You also have the ability to create an angled line
type approach and departure for the tool. The “Angle” value is
simply the angle of the lead-in and lead-out line itself and the “Line Length”
option determines how long or short
you want these lines to be. Let’s take a
look at this in the example below.
The NONE option refers to straight plunge
ONLY.
OK,
let’s get back to the lesson now that you understand how to use this box. Go ahead and enter .25 for Diameter under TOOL SETTING.
STEP 8
Select Automatic under the Tool Compensation. Under Compensation Direction choose the LEFT
Option. Under Lead-In/Out select the
CIRCULAR approach option. Now enter .25
for the Radius and .5 for the Distance.
Now select OK to produce the toolpath and your G-Code
program.
STEP 9
Now go to the EDIT menu on the
Congratulations!
You have completed this lesson.