Mastercam setup for 3-axis router
PAGE UNDER CONSTRUCTION
Mastercam setup on personal computer
MIT IS&T hosted Mastercam installer: follow instructions on archshops
software page and the linked IST page to
install Mastercam on a personal computer.
Understanding the tools (end mills & other router bits, tool holders)
The below image shows a few different types of tools that cut while spinning. The upper row tools are all solid carbide
end mills. The bottom row has 2 carbide-tipped router bits, and last, a simple drill bit. These 3 types of cutting tools
are very common, but they need to be handled differently.
Look closely at the difference in the shapes of the end mills vs. the drill bit. There are differences between the solid
carbide and carbide-tipped tools, as well - there are many very different types of router bits that wouldn't fit into this
page.
More info will be included on a drill handheld router tutorial page; this tutorial will be focusing just on the basics of 3 axis machine setup for milling materials like foam,
plywood, and MDF, and will only refer to on work done with solid carbide end mills. Just keep in mind that these tools are
handled very differently- much more than they may sound at first.
It's very important to recognize the flute, shoulder, and overall length of the end mills we'll be using.
The flute, or sharp cutting edge, does
not extend all the way up to the edge of the recessed spiral on the tool. In the
photo below, the cutting edge of the end mill ends almost 1/3" of the length down, away from the collet holder. The
cutting edge/flute ends at the shoulder, which is just the transition between cutting edge and the fully solid cylindrical
upper part of the tool, called the 'shank'. The shoulder cannot cut. The shank is the solid part that a collet must clamp onto,
to hold the tool securely in the spindle. The tools must be inserted fully into the holders for maximum surface contact between
the shank and the collet, so that it will not move at all during use.
The above image shows a long half-inch diameter tool, installed in one of the Onsrud tool holders, up against a block of
material that was used for a project. The tool clearly is not long enough to reach all the way through with the overall
tool length, never mind just the tool's flute length -
It's extremely important to know your exact tool measurements - flute length, shoulder length, and overall length. These
are measured from the tip of the tool, not from the holder. There is an illustrated tab in Mastercam where these lengths are shown (in
the case of a preset tool library like the Onsrud) or can be entered (in the case of manual tool installation like the Shopbot)
Get Started
Please be ready with a clean Rhino (or other NURBS) file in the correct scale and orientation at 0,0. Please avoid
STL/meshes whenever possible.
Open Mastercam first.
Go File>Router>CRONSRUD. (If you are setting up a file for Shopbot, Intelitek or Prototrak, look under File > Mill).
Find the 3 'files', 'tool settings' and 'stock setup'tabs by expanding "properties" under "machine group 1".
In the "stock setup" tab, make sure "Display" is checked, so you can see the wireframe stock box after you give it
accurate dimensions.
- Click on Files to choose/confirm that Onsrud tool library is being used (if using Onsrud)- this tutorial is focusing
on Onsrud setup specifically.
- Click on stock setup, and enter stock size in XYZ. This must be accurate!. Click once on the red box to move
the arrow, to choose the origin (bottom left corner, as in photo, for 3 axis).
- Check what should now be a wireframe representing material and geometry orientation, relative to the machine's X/Y orientation
(on the Onsrud and Shopbot, the X axis is the narrower dimension on the spoilboard). Double-check the tool library in the "files"
tab, and make sure 'sequential ordering' is turned OFF.
- Click OK (green check button) to save.
- Click on File -> MERGE (in the blue bar) to import your geometry (not 'file ->open').
Confirm its location at the origin when prompted.
Make sure you've imported only relevant geometry into Mastercam (it helps to start by exporting what you need to a clean and
correctly oriented Rhino file, first).
Now you can start setting up toolpaths. There are a few basic concepts that are important when envisioning how to start:
- Toolpaths are driven/defined by either surfaces, or curves.
- There will usually be roughing tool paths to run before finish toolpaths can be run. The process will need to be broken
down into several steps for most jobs- you'll need to plan out the best way to approach the cutting operations for the
best/fastest results.
- The flute, or cutting edge of the tool is the only part of the tool/tool holder that can ever be allowed to come into
contact with the material, and the tool can not be allowed to cut down into the spoil board (below Z zero). Strict boundaries
need to be kept within which the tool is allowed to move - and any excess material left around the edges of toolpaths need to
be taken into account as potential collisions with the non-flute parts of the tool and its holder. Collisions and too-deep cuts
are major fire risks, so staying hyper-aware of where the tool moves at every step in the job is extremely important. The first
step in controlling this is making sure the tools and material are defined absolutely accurately in Mastercam - so it can show you
accurate previews and accurate warnings about what will happen before you actually run a job.
With any material thicker than a sheet of plywood/MDF, there is likely to be a lot of material that needs to be 'roughed' away
before you are able to approach the finish surfaces of the object with the tools. This is going to be the first step for most
work done on the routers (one exception would be the most simple jobs - 2D curves cut into a single sheet of material with a
compression endmill, which needs no roughing out first).
If the roughing part of the process is neglected, risks of fire and broken tools are high. Taking the time to set up good roughing
toolpaths is very important, even though they don't directly create the finished part's surface qualities. Good roughing toolpaths
will be efficient, and also minimize stress on the tool.
There will often be more than one option for particular details, but some will be faster than others, and some will produce nicer
results. One thing to keep in mind regardless, though, is that you should never expect to be able to cut any 3 axis job in one or two
blanketing toolpaths - expect to approach it in multiple steps. Your results will usually be pretty awful, and attempting to remove
all the excess material and simultaneously cut the finish surfaces can be dangerous in a lot of cases, as well. So don't shy away
from the idea of multiple steps.
This image shows a preview of a roughing tool path in progress (defined by a topography-like surface) - see how the yellow flute
(cutting length) of the tool is only able to extend partway into the material to the curve (where the finish surface is)?
The roughing tool paths need to do 2 things - cut away as much material as possible, without wasting time or stressing the tool,
and also without plunging too deep- only the flute can ever come into contact with the material. If it goes deeper, melting/burning
happens immediately- and the end mill can just snap like a twig if it's overstressed.
You'll prevent all this in carefully setting the details of your roughing toolpath.
We almost always use "surface rough parallel" to rough out excess material.
Right-click on 'toolpath group 1', and go to - router toolpaths - surface rough - parallel
These images also show a bit of distance between the tip of the tool and the finish surface - this is an intentional step
to leave a little bit of material for the finish toolpaths to remove later. The toolpaths leave 'mill marks' in material,
just like any other cutting machine - if you want to remove the mill marks from roughing, you need to leave a skin of material
on the 'drive surface(s)' - this is a setting in the roughing toolpaths.
With really thick material, it's necessary to rough in steps down ('stepdown' setting in the roughing toolpath) to approach the
finish surfaces, because the tools' flute lengths just aren't long enough to cut that deep in one pass - even in relatively soft
foam this is not possible.
As you can see in the images, if you were to try to plunge immediately down close to the finish surface, the shoulder/shank/collet
of the tool would crash into the material. Foam will crush/tear when this happens- but because the spindle will be spinning at
several thousand rpm as it happens, the friction will also cause melting - this cannot be allowed to happen. Melted foam will get
in the way of the tool cutting properly, and also releases dangerous (usually styrene) fumes.
But if the material is thinner, can you safely skip this? The answer depends on some details.
The roughing is going to be done with tools with wide diameters - normally .75 if on the Onsrud, or .5 if on the shopbot (.5" is
the largest diameter tool the Shopbot can hold). There's no reason to rough with thinner tools - it's efficient to rough away
material as quickly as possible (with proper feeds/speeds set using the chip load calculator).
If you have thinner material, like a single sheet of 2" foam, and you want to skip straight to finishing, and all the tools you
want to use have flute lengths that can safely reach the finish surfaces without any collisions, then in such soft material, it
would be safe to do.
If you're using hard material - plywood, MDF, solid wood, wax, plastic, etc., then you probably will not be able to go straight to
finish toolpaths with thin tools.
The problem is that attempting to plunge into solid material and push the tool sideways as it attempts to cut its full diameter in
hard material is bad for the tool - in a situation where you're trying to skip roughing, if thinner end mills are plunging deep,
they're almost guaranteed to break immediately.
If you're skipping roughing, you're more likely to be attempting to use tools needed for finish details, which are more likely to be
narrower in diameter.
When plunging deep into material (like in a deep pocket) is unavoidable, the toolpath, if set up well, should start by carefully
opening up a space deep into the pocket first, just wide enough for the tool to have some breathing room around it (while not
cutting deeper than the flute length can cut), and then spends the rest of its time cutting mostly or entirely just along the side
of the tool, rather than dragging around at the tip.
ABOUT
RESERVATIONS
HOURS
TUTORIALS
