It's getting to where fewer and fewer designers are
making flat drawings. The trend is to design, test
and machine in 3D, even for parts that have traditionaly
been flat 2D.  Plates, brackets and other simple parts
are being drawn in solid modeling packages like
SolidWorks & Mechanical Desktop.  Mastercam also
has Solid Modeling capability and is compatible with
the packages listed above.

People are drawing with solids for many reasons

• It's easier to draw with solids vs. surfaces.
• It's gives you a true representation of the part.
• You cant "fake" how intersections fit together.
• It ensures that everyone is working off of the same plan.
• It saves you (the machininst) from having to interpret design.
• It saves you from having to redraw it.
• It Lets You Machine The Part Without Knowing The Dimension.

The parts shown below has drilled holes on several levels.
With most Cam systems these would have to be machined
as separate toolpaths. Because all of the depths are different.
Lets assume all of the holes are supposed to be tapped to
a depth of  .950.   The absolute depths, from the top of
the part would be different for each level of holes.

Here's how Mastercam can make that easy to do.

__

At the bottome of the screen you'll see a prompt
to "Select arc to match".  What we're going to do
is pick the arcs by their size, which in turn selects
their locations in X Y & Z.

  Pick any one of the arcs.

A prompt at the bottom will say..
"Enter the arc radius matching tolerance"
and show a value of  .001.    Press Enter.

It should be asking "Tolerance for selecting similar holes".
This means, any hole like the one you selected,
within .001 of the same size,  will be part of the group
being drilled.

Next it wants to know where to look for similar holes.
Select "Window" .....

....and put a window around the entire part
(or at least all the holes).

Now the Point Manager is displayed.
This is where you deceide if you like the order
the holes will be drilled. if it looks like the
picture below, you can just press  "Done".   If not,
you want to select  "Options" to sort the points
into the order you want.  Be sure it starts from the
highest point (top) of the part.

 

On the Tool parameter page, pick a center drill.

 

On the Simple drill (drilling parameter) page set the
values as shown below and set them to Incremental.
This is the important part: The depth will be Z-.185
From The XYZ Center Of The Hole.
I dont have to assign a different depth for each level.
The system knows where the circle is and it calculates the
depth from that "point".   Press OK when your finished.

 

To do the Drilling & Tapping, we could go back and repeat
the selection process, pick our tools and set the information
for each operation.   Or we can copy the operation we just
created, make copies and modify the copy.  A much simpler
process.  And I like simple.

Back on the Toolpath menu. Select  Operations.

In the operations manager point your cursor on the
operation (the blue bar), hold down your right mouse
button and slide your mouse down a little bit.
Let go of the button.

Select Copy After and you'll have a duplicate operation.
Do this again until you have 3 operations.

After you have 3 operations, select the parameters
of the second operation.  Get a  27/64 drill.

Change the values of the depth to -1.25 as shown below.
Be sure the Cycle is Peck drilling. Press OK when finisned.

Select the Parameters for the 3rd operation.  Get a 1/2-13 Tap.
Change the values of the depth to -.950 as shown below and be
sure the Cycle is for Tapping.

You'll see small red X's  in the modified operations.
Press   Select All  and then   Regen Path.
Your done.   Post the file and all of the depths will
be set to the point position.

 

See the posted code for several different control types

Fanuc                   Bridgport DX32                Heidenhain