Sunday, November 17, 2013

Mastercam Toolpath Setup

This topic is an overview of the process of toolpath programming in Mastercam 2017 for a 3-axis router. It is specifically focused on the Onsrud Production Router at Taubman College.

The Mastercam User Interface

There are the usual Windows style tabbed panels on the top of the interface. You may also dock a number of toolbars with icons there as well. The machining operations list is on the left. The 3D viewport is on the right.

Viewport Navigation

You can use any of the following methods of manipulating the viewport:
The quickest method to control the view is using the middle mouse button. 
  • Rotate: Press and drag the middle mouse button
  • Pan: Shift-key + Press and drag the middle mouse button
  • Zoom: Roll the mouse wheel
The View panel has operations for zooming, panning, and rotating the viewport.

Use the viewport right-click menu to access other options, like Zoom Extents (called Fit in Mastercam), and to change to Top, Front, Right, or Isometric views.

Choosing Dynamic Rotation lets you rotate an Isometric view.

Note the keyboard accelerators listed for zooming. And as mentioned above you can also use the mouse wheel to zoom in and out of your model.

Operations Manager

The operation manager shows you a list of your toolpaths. The operations are cut in order from top to bottom. You can use cut/copy/paste to move items around in the list. You may also use the red icons in the toolbar to move the position for creating new operations. The red arrow in the list shows where new operations will be inserted.

You use right-click menus in the operations list to add new toolpaths.

Choosing a Machine

The first thing you need to do when setting up a new file is choose the type of machine you wish to use. You do this from the Machine panel. In the Machine Type section, from the Router option, select a machine, for example the 3-axis Onsrud Production router is "CRONSRUD-BR-FIXED_BRIDGE.RMD-7".

If that choice is not available form the list do the following:
  • From the Machine tab choose Machine Type > Router > Manage List...
  • From the dialog presented choose the following from the list on the left:
  • Then press Add to add it to the list on the right side of the dialog. This makes it available. 
  • Press OK to exit the dialog. 
  • Then choose that file from the panel again: Machine Type > Router > CRONSRUD-BR-FIXED-BRIDGE.RM-7 (it now appears in the list). 

This will add a new Machine Group to your Operations Manager list. Add operations to that group.

Importing the Rhino Model

Then you need to bring in your geometry. To import your Rhino file use the File tab. From the list on the left choose Merge. You can load Rhino .3dm files directly.

Important Note: In this write-up it is assumed you have projected your geometry to the CPlane (Z of 0.0). You'll be specifying the Z values (for example depth of holes, pockets, etc.) when you set up the operations to cut that geometry. 

Level (Layer) Control

The layers you create in Rhino are also controllable in Mastercam. Layers are referred to as Levels in Mastercam. There's a tab at the bottom of the Operations Manager to switch you to viewing Levels in that panel.

From the panel you can toggle the visibility of layers using the Visible column. You can use the right-click menu to make a layer current (called Active in Mastercam). You can also use it to "Purge empty levels" which removes those layers with no entities from the file.

Stock Setup

You need to tell Mastercam the extents of the material you wish to operate on. To bring up the dialog to set the stock size click the Stock Setup button in the Operation Manager.

The easiest way to do this is to draw your stock in Rhino. Then turn only that level on. Then use the All Entities button at the bottom of the Machine Group Properties dialog to set the size to that of all the visible entities.

Stock Geometry Setup: The usual way stock is set up for use with the Fab Lab routers is to place the top of the stock at world Z of 0.0 in Rhino. The stock is then all in negative Z. The long axis of the router (the 8' table dimension) is the Y axis. The short axis (the 4' table dimension) is X. The origin is at the closest corner on your right as you face the router. So +X is away from you as you face the router. And +Y is to your left as you face the router. When using this setup make sure that the Stock Origin has a Z value of 0.0. 

After you press the All Entities button the sizes will be shown as well as the stock origin. 

Tool Types

This section provides information on the various types of tools available. See the post CNC Router Tools and Tool Holders for more detail.

The spiral shaped flutes in a router bit can move the chips up or down. The chips and spiral also exert a force on the workpiece, which is either pushed up or down. The edges of the cutter can be smooth or serrated.

Up-Shear Bits

An up-shear bit moves the chips up and out of the cut. This is good in the the chips are cleared away. But it's not helpful that it tends to lift the workpiece up. They can also tear out the fibers at the top of the cut. The vacuum tables on the routers are usually sufficient to hold work pieces about 20-25 square inches. Anything smaller tends to get lifted and pulled away from the table.

Down-Shear Bits

A down-shear forces the chips to the bottom of the cut, which is far from ideal. However it also forces the workpiece down, which is good. Down shear bits leave a clean cut a the top of the workpiece.

Compression Bits

A compression bit has the bottom flutes of the tool lifting up and the top flutes of the tool pushing down. So the top twists one way and the bottom twists the other. This is used to reduce chipping on both the top and bottom surface of the material. This makes a difficult situation for clearing chips because they are being pushed into the middle of the workpiece. These are often used when cutting plywood to get clean cuts on both faces.

Chipbreaker Bits

These bits are used for roughing cuts. The edges are serrated to break up the chips into smaller pieces. This allows for fast material removal - as is desired in roughing.

Tool Setup

For reference, below is a table of common speeds for cutting plywood. The spindle speed is revolutions per minute and the others are inches per minute.

Diameter Flutes Type  Spindle   Feed   Plunge   Retract 
 1/4" 2 Down-Shear Finisher         18,000              250              125              500
 1/4" Ball End Finisher         18,000              250              125              500
 3/8" Brad Point Drill           3,000                60                60              500
 3/8" 2 Chipbreaker Down Shear         18,000              400              200              500
 1/2" 3 Down-Shear Rougher         15,000              600              300              500
 1/2" 3 Up-Shear Rougher         15,000              600              300              500
 1/2" Ball End Finisher         18,000              400              200              500
 3/4" 3 Up-Shear Finisher         18,000              600              300              500
 3/4" 3 Up-Shear Rougher         15,000              600              300              500
1"    2 Chamfer         18,000              300              150              500

If you like to calculate the values on your own please see this site: Onsrud Chiploads | Feeds and Speeds. Even better is using a Feed and Speed calculator, an example of which is GWizard.

Tool Library

A variety of standard tools have been set up already for the FabLab 3-axis routers. These are available in the tools library. To choose tools from a tool library you press the Select library tool... button in the Tool panel. More information is further below on how to get to the tool panel.

Choose the UMich library for wood for example: 

From the Tool Selection dialog you can choose a tool from the list. The tool has all the properties already set - for example spindle speed, feed rate, plunge rate, etc. 

3-Axis Toolpath Setup

In simplest terms toolpaths are instructions to the machine to move a specified tool over the chosen geometry. There are many different toolpath types available. In this section we cover some of the most common ones available for the 3-axis router and how to set them up.

Add Toolpaths

You can add toolpaths to your list of operation by using the Toolpaths tab or the right-click menus in the operations manager. These get added at the position of the red arrow in the operations manager.

You can also use the right-click menu in the Operations Manager panel:

From the right-click menu hover over Router toolpaths. From the flyout menu choose your toolpath type.


Contour toolpaths remove material along a path defined by a chain of curves. Contour toolpaths only follow a chain; they do not clean out an enclosed area.

After you add this toolpath you'll be asked to select a chain for the contour.

You can click on the geometry to chain and it'll appear with arrows to show the direction of the toolpath:

Once you set the chain you can select the tool. You do this by clicking the Tool branch on the left side of the 2D Toolpaths dialog presented. You may choose from an existing tool or from the tool library.

You can also customize the properties of the tool in this dialog. For example setting the various feed rates.

After you choose the tool you can set the Cut Parameters. You do this by selecting Cut Parameters in the 2D Toolpaths dialog.

Controls determine which side of the chain cutting takes place on (left or right), and how much material to leave on the wall or floor of the cut.

You also need to set the Linking Parameters. These controls determine how deep the cut goes and how much it retracts between cuts.

In this dialog you set several very important properties. Either of these can be set to Absolute or Incremental. Absolute refers to a Z value of 0.0 as set in your stock definition. Incremental refers to where the geometry is located. So, for the Depth parameter, an incremental value of 0.0 would follow along the selected chain exactly. A value of -0.25 would cut 1/4" below the chain. An absolute value of 0.0 would cut at the top of the stock above the curve.

Fortunately, Mastercam draws the toolpath in the viewport so you can visualize your settings. And if it isn't what you need - make changes.

Make sure you have the Lead-In/Out settings correct. These are critical for having the tool stay cool during cutting. Plunging directly into the work rather than gently leading in and out generates a great deal of heat. Plunging repeatedly can start a fire in the material. 

Choosing Lead In/Out brings up the dialog to set the properties. The settings below work well for sheet goods (for example 18mm Baltic Birch Plywood):

You can reduce the sizes shown above if the contours are tightly spaced together.

Note that the lead in/out appears on the Start Point of the contour. You can change that position and move it to where you like. Do that following these steps:

Click the Geometry branch in the Operations Manager beneath the Contour operation. This brings up the Chain Manager dialog. Click on the Arrow icon to find a particular chain.

Select it in the viewport and you'll then see it selected in the list (it is faint, but it is visible). Then right-click on the contour to change and choose Start Point. This will let you visually drag the start point in the viewport.

From the dialog click the arrows icon shown below to allow you to click in the viewport and move it: 

You can also change the side a contour is cutting on (to have it be outside of the part) using the right-click menu choice Change Side. To get there do the following:

Click the Geometry branch in the Operations Manager beneath. This brings up the Chain Manager dialog. Click on the Arrow icon to find a particular chain.

Select it in the viewport and you'll then see it selected in the list (it is faint, but it is visible). Then right-click on the contour to change and choose Reverse Chain. This will switch that particular contour to cutting on the other side of the line:

Depth Cuts also need to be set. Normally, you'll only want to cut to a depth that's no more than twice the width of the tool. For example, if you are using a 3/8" diameter tool, you'll only want to cut to a maximum depth of 3/4". To put less stress on the tool you can cut less deep.

You do this by selecting Depth Cuts in the 2D Toolpaths dialog.

Enable Depth Cuts by checking that box. You can set the Max rough step to the amount you want to cut in each pass. Here is an example - the max depth is set to 0.25". You can see in the viewport the number of passes around the contour increases.

You'll want to add tabs to your parts. Tabs are small bits of material that hold the part in place while cutting. You can set the width and height of the tabs. Set them up following these steps:

Click the Tabs branch in the tree in the 2D Toolpath dialog. Click the checkbox next to Tabs to enable them. Set the desired width and thickness. I usually use about 0.75" wide and between 0.05 and 0.1" thick. You can see the settings below:

Once you have the sizes set click the Position... button shown above. This lets you select contours in the viewport and you can visually place where the tab should be located. Move between any of the contours in that operation to set the tabs.

If you want to edit the tabs later (add more, move them, delete them) locate a particular chain in the Chain Manager dialog, right-click it and choose Edit Tabs:

You can then choose what type of edit to make.


Drill toolpaths cut holes in your parts.
The Linking Parameters let you set the limits on the top of stock, depth, and retracts.

Use the 1st peck and Subsequent peck amounts to control how deep each peck travels.


Pocket toolpaths are used to clean out material from an enclosed boundary.

When you add the pocket you'll be asked to pick the chain for the pocket boundary. This dialog is the same as was used for contouring.

By making selections on the left in the tree you bring up panels on the right side for roughing, finishing, depth cuts, and linking.

On the Cut Parameters page you can choose a machining direction. This will be either Climb Cutting or Conventional cutting.

Climb Milling cuts the chained geometry with the tool rotating opposite the direction of travel along the cutting side of the tool.

Conventional Milling cuts the chained geometry with the tool rotating in the same direction as the direction of travel along the cutting side of the tool.

Climb Milling Versus Conventional Milling Video

Typically conventional cutting provides you with the best edge provided you have picked the right tool geometry to cut the specific material. This applies to sheet goods (plywood, MDF, etc). If you are cutting solid wood (hardwood) where multi-directional grain patterns have to be considered, it is often necessary to climb cut thereby limiting the chip the tool can remove at one time and reducing splintering. This is the main application for climb cutting.

Use conventional cutting wherever possible. This allows the tool to clear the chip from the work instead of pushing into the work. Conventional cutting allows the chips to be thrown behind the tool yet climb cutting requires the chips be thrown in front and then run over, thus creating more pushing of the work piece due to pre-loading of the flute. If rough and finish passes are utilized, use a climb cut on the finish pass.

You can also select the amount of stock to leave on the walls and floor of the pocket. 

Next, in the Roughing page, you can choose the cutting method and a step over amount.

On the Entry Motion page you establish how the tool enters the workpiece. You can choose to ramp into the cut or enter by cutting a helix.

On the Depth Cuts page you determine how deep the tool moves as it cuts to the bottom of the pocket. If you leave this unchecked it will be cut in a single pass. If you pocket is deeper than 1/2 the width of the tool then use depth cuts to minimize stress on the tool.

Finally you can set the linking parameters which control the depth of the pocket and the heights for top of stock, feeding, and retracting. You can use Absolute or Incremental numbers.
  • Absolute values are always measured from the origin 0,0,0. If you were to translate geometry associated with a toolpath, and the toolpath depth were set to an absolute value, the tool will try to cut to that same absolute depth value no matter where the geometry is located.
  • Incremental values are relative to other parameters or chained geometry. Depth and Top of Stock parameters are relative to the location of the chained geometry. Clearance, Retract, and Feed plane are relative to the Top of stock. 

Note that if you have projected all your geometry to Z of 0 you'll need to use Absolute values to specify the depths. 

Surfacing - Roughing

Surface roughing toolpaths typically use larger tools, multiple stepovers, and multiple step downs to quickly remove larger volumes of stock and leave an even amount of stock for finishing. The roughing toolpaths you choose for your part depend on the shape of the part, shape of the stock, and machining situation.

Surfacing - Finishing

Surface finishing toolpaths typically finish a part down to the drive geometry (or to the stock to leave amount if one is specified). These are usually using a small stepover and don't cut very deep. The surface a 3D form a typical stepover is 0.05". The typical amount of material being removed might be 0.25" or 0.125".

See the post Surface Rough and Surface Finish Toolpath Setup for details.


There are several ways to simulate your cuts in Mastercam.

The "Backplot" features lets you see a wireframe drawing of the selected operations. You may scrub the slider back and forth to see the sequence.

The "Verify Selected Operations" feature lets you see a solid model of the selected operations. This model can also be exported to an STL file for checking in another program (like Rhino).

Important Note: Always check that the cutters are not cutting far into the spoil board on the table. The easiest way to do this looking in a side view. On a 3-axis router you should only see the tool move a few thousandths of an inch below your material. If it's going deeper you need to adjust your toolpath.

Code Generation

When everything is set up correctly you are ready to generate code for the machine to use to cut your workpiece. To generate code press the Post Selected Operations button.

You can generate an NC file for all the operations or just the selected ones. When you click the G1 icon you'll be presented with the following dialog to set up the output:

You can choose to have a text editor appear after the code is generated by checking the Edit box. Once you OK the dialog you'll be asked if you want to post all operations or just the selected ones:

Note that on the Taubman Refurb router you want to save the operations one at a time for a particular tool. On the Production Router which has a tool changer you can save all the operations to a single NC file.

You'll be prompted for the filename to save. Press OK to create your .NC file.

Monday, November 11, 2013

CNC Router Tools and Tool Holders

This post provides information on common CNC tools used in the lab. It also shows examples of the two types of tool holders we employ. Lastly it shows how the tools are measured for length so the CNC machines knows exactly where the tooltip is for accurate cutting.


This section discusses a few different CNC router bits and their common cutting application.

The most common types are:
  • Straight Bits: These tools cut on both the end of the tool and on the sides. There are many variations of the geometry of these bits. Most of the material below is devoted to explaining the differences and their use.
  • Ball-End Bits: These bits have a circular profile at the tip. This allows them to cut 3D surfaces.
  • Chamfer and Engraver Bits: These cutters come to a point at the tip. They are commonly used to label parts by cutting the numbers as a shallow V shaped groove.
The following illustrations show the difference in cut pattern and the effect of wide versus narrow step-over in toolpath setup.

Tool Material

There are a number of common materials used to make bits. 
  • HSS (High Speed Steel): Typical applications in non-abrasive plastic, solid wood and aluminum where keen edges perform best. High Speed Steel tools a tougher core which helps to prevent tool breakage. These are the least expensive.
  • Carbide Tipped: Used for a variety of applications in composite woods, hardwoods, abrasive plastics and composites plastics to hard aluminum. Limited by geometry in some applications due to the brazed nature of the tool. These last longer than HSS but are more expensive.
  • Solid Carbide: Typically used for widest variety of applications including man-made board, solid wood, abrasive plastics, and some aluminums. Solid Carbide does not deflect allowing the tool to be fed at higher feedrates. Solid tools also have major edge keenness advantage thought only possible in HSS until a few years ago. The Taubman Fab Lab uses most solid carbide tools.

Flute Geometry

The geometry of the flutes in the cutters has a great influence on their application. 

  • Up-shear (up cut) Flute - This is a spiral geometry. It provides the best surface finish and allows for good chip extraction. May cause part lifting if vacuum or fixturing is not sufficient to hold the parts in place.

  • Down-shear (down cut) Flute - This is also a spiral geometry and provides a downward force which helps eliminate part lifting. Chip overheating may occur if there is no space below the part for chip expansion.

  • Compression - Visualize combining an up-shear and a down-shear and you've got a Compression Cutter.  The flutes go one way on the bottom of the flute length and the other way at the top. They are particularly suitable for double-sided melamine or laminated material. They’re used because they pull towards the middle of the cutter, which reduces chipping on both the top and bottom.

  • Straight Flute - Offers a neutral cutting action. There is no spiraling, augering action to move the chips up or down. These bits are the least expensive because they are easy to manufacture. The downside is that they apply the cutting force all at once rather than progressively like the spiral flute geometry.
Here's how you can look at a bit and determine if a bit is up-shear or down-shear: The router bits we use in the lab are designed to spin clockwise. Hold the tool shank up and the tip facing downward. Look down the length of the tool. Spin the tool in a clockwise direction. Note if the spirals are pulling upward, or pushing downward. If they are pulling upward you have an up-shear. 

    Chip-Breaker Grind: Another variant on flute geometry are Chip-Breaker grind bits. These usually take the form of a serrated edge on the flutes. The break in the edge fractures the chips into smaller pieces which can improve chip removal. Some chip-breaker bits can leave a striated finish unless the serrations are staggered between the flutes. 

    Here's a picture of a test cut showing the difference between up-shear and down-shear bits. This example shows the direction the tool is moving with the arrows. This sample is White Oak.
    The bit is turning clockwise. Note the upper edge of the up-shear cut. It's pretty clean. That direction is like petting a dog along its back in the direction the fur flows (head to tail). The other side of the bit is like petting the dog from tail to head - backwards. In the down-shear case it doesn't make much difference.

    Number of Flutes

    The Fab Lab has single, double, and 3 and 4 flute cutters. Note: As the number of cutting edges increases, your feed rate should increase to prevent burning and premature tool dulling. 
    • Single Flute - Allows for larger chip loads in softer materials. Certain materials produce large chips - for example Aluminum. 
    • Double Flute - Allows for better part finish in harder materials. Because of the two flutes the feed rate must be increased over a single flute.
    • Multiple Flutes - Allows for an even better part finish in harder materials. Again, because of the multiple flutes the feed rate must be further increased. 

    Drill Bits

    Drill bits are for making holes in your work. There are three types commonly used in the lab: 
    • Twist - these leave a cone shape at the bottom of the hole. Thus you need to drill deeper to get fully through the material.
    • Brad Point - the edges of the bit are sharpened and extend to nearly the same length as the tip. This allows the end of the hole to be less cone shaped. Thus, you don't need to cut as deep to ensure that the material is fully cut through.
    • Forstner - These are used for cutting flat bottomed larger holes. There is a small detent in the middle of the hole from the point in the center of the bit. Note that if you want truly flat bottom holes you can use a boring toolpath and an endmill rather than a drilling operation.

    Tool Length

    A note about tool length. In choosing a bit for any application, always select one with the shortest cutting edges and the shortest overall length that will reach the required cut depth. Excessive length intensifies deflection and vibration, which degrade cut quality and lead to tool breakage.

    Formulas Relating Chip Load, Feed Rate, and Spindle Speed

    There are standard formulas for feed rate and spindle speed. These are listed below. However, I prefer to use a software tool to generate these values. The calculations are much more sophisticated than the standard formula. One example I like is the G-Wizard Machinist Calculator.

    Chip Load = Feed Rate / (RPM x Number of cutting edges)
    Feed Rate (IPM) = RPM x Number of cutting edges x Chip Load
    Spindle Speed (RPM) = Feed Rate / (Number of cutting edges x Chip Load)

    • Feed Rate = The speed of the tool moving through the work.
    • IPM = Inches Per Minute
    • IPR = Inches Per Revolution
    • RPM = Revolutions Per Minute

    Tool Holders

    There are two types of tool holders used in the lab. One uses a conventional collet, the other a shrink fit collet.

    Conventional Collet

    The conventional collet is a holding device that forms a collar around the tool to be held and exerts a strong clamping force on the tool shank as it is tightened by means of a tapered outer collar.A torque wrench is used to apply the correct amount of clamping force.

    Shrink Fit

    A shrink fit collet holds the tool in place by the collet shrinking and tightening around the tool shank.

    Tools are inserted and removed using this machine.

    The collet is heated until the tool barely slips in. Once hot it shrinks enough that the tool can be slid in or out. Compressed air is then blown onto the collet to cool it down. This locks the tool in place.

    You cannot use HSS (high speed steel) tools in the shrink fit machine due to the very high temperature. 

    Tool Measurement

    The tools are measured for length using a digital height gauge. First the gauge is zero'd on the base ring. 

    Next the tool is placed on the right and the height is measured. The height is entered into the tool table of the machine.

    For the 3-axis routers in the Fab Lab we always manually measure the tools. The Roland 4-axis and the Onsrud 5-axis routers have the ability to measure the tools automatically, right on the machine.