CAM for the Datron 3-axis Mill

This Instructable is for workshop users at Pier 9 who are interested in machining parts on the 3-axis Datron mill. It is expected that users have intermediate to advanced level CNC experience, and have completed at least one personal project on the Haas VF2 Vertical Mill. Click here to learn more about the steps involved in the CNC Learning Path at Pier 9.

In this Instructable, you will learn these CAM principles in Fusion 360 or Inventor HSM for the Datron 3-axis Mill at Pier 9:

Optimal Load

Maximum Stepdown

Minimum Cutting Radius

Stock to Leave

Where to set the Work Coordinate System

How to maximize surface area on the vacuum table

Bottom heights on the vacuum table

Minimum part stickout on the pneumatic vises

Why is CAM different for the Datron versus the Haas Mill?

1) Higher spindle speed, lower torque

The Datron has a high spindle speed, 40,000 maximum rpm, which makes it ideal for detailed engraving and small, precise parts. It's not as well-suited for larger parts with more material removal because the load on the tool must be minimized.

2) Different tool library

The largest Datron tool diameter, other than the face mill, is 8 mm (about 0.315", or halfway between 1/4" and 3/8"). Compared to the Haas library, in which the largest tool diameter is 1", the Datron library consists of much smaller diameter tools. The tools range from 1mm-8mm in diameter, and consist of flat nose, ball nose, and chamfer tools. The longest flute length is about 1", so material taller than 1" cannot be machined in a single pass.

3) Different workholding requires different considerations

The two workholding systems on the Datron, the pneumatic vises and the vacuum table, each require a different CAD and CAM setup. Users should know what workholding system they will be using in advance.

4) Work envelope

The Haas Mill has a cutting envelope of 30" x 16" (X and Y). The Datron Mill has a cutting envelope of 500mm x 400mm (19.685" x 15.748" in X and Y).

Optimal Load is the force, or load, on the tool during 2D or 3D Adaptive clearing operations. The optimal load is the amount of material the tool engages with as it moves, and it is measured in inches because it's the equivalent of stepover for a legacy toolpath.

The default optimal load in Fusion CAM is 0.4*tool_diameter (40% of tool diameter), which is much too aggressive for the Datron.

Also, the optimal load formula that you use for the Haas Mill does NOT apply to the Datron.

Instead, you must check the tool comment of every tool to determine the correct optimal load.

This can be found by highlighting the tool in the tool library, and scrolling midway down the Tool Info section on the top right corner of the dialog.

Or, if you Edit a tool, you can see the comment in the Post Processor tab.

Don't forget that the units in the comment are millimeters! If your program units are inches, you can insert the unit mm in the Optimal Load field and the program will convert it into inches.

This is the most important setting for Adaptive clearing operations. Check it every time.

If you are using a Facing, Pocket, or Contour toolpath, your maximum stepdown should be no more than 0.025".

The only exception would be a finishing toolpath, clearing an area with no more than 0.005" stock to leave.

The Adaptive Clearing, Pocket Clearing, Horizontal Clearing, and Contour strategies produce toolpaths that go fully into sharp corners that can bury the tool. The Minimum Cutting Radius setting on the Passes tab allows you to avoid the sharp corners by specifying the minimum allowed radius to be machined.

By default, the Minimum Cutting Radius for Adaptive is set to 10% of the tool diameter. This is a good idea in theory, helping the Adaptive roughing avoid sharp corners.

However, this does not prepare the part well for finishing operations! Imagine that the default Minimum Cutting Radius was larger than inner corner of a part. This means that there will be more Stock to Leave in inner corners for finishing operations to tackle.

When the finishing tool goes into those corners, the part could move or the tool could break.

To prevent this problem, make sure your inner corners have a radius that's at least 15-20% larger than the radius of the tool you will use in those corners. (In the example images, I set a radius of 5 mm for the inner corners, knowing I'd be using an 8 mm diameter, 4 mm radius tool.)

Then, set your Minimum Cutting Radius to 0.

In your finishing toolpath, you can also add multiple finishing passes with a very small stepover (0.001-0.002").

Finally, highlight both the roughing and finishing toolpaths so they both appear on the part, and zoom into the inner corners. Make sure the gap between roughing and finishing is not larger in the inner corners.

This gap will put unnecessary load on the tool in the inner corners.

There is no gap here, so the load will stay constant.

By default, Stock to Leave on all roughing operations is set to 0.02" in Fusion CAM.

This is too aggressive for finishing operations on the Datron.

Change Stock to Leave to 0.005" for all roughing operations.

Always place the Work Home in the center of your part. The Datron probing cycle will automatically measure the longest side of your part in two locations, so if the stock isn't square the program will automatically adjust.

Make sure to separate the two locations on the same side as much as possible; this will ensure a more accurate angle measurement.

The Datron comes with a vacuum table to hold down stock, which is a convenient alternative to pneumatic clamps. The key to using the vacuum successfully is maximizing the surface area of the stock.

The stock sits on two aluminum vacuum plates that are divided into twenty 100 mm square grids that can be individually opened or closed. To ensure that you do not mill into the vacuum plates, you will place a thin sheet called a VacuCard between the vacuum plates and the stock.

More surface area will ensure a better vacuum hold. Aim to cover three or four grid squares. Avoid only covering one grid square.

Each grid square in use must be covered fully by the stock.

Don't hold more than 1/4" of stock height for each grid the stock covers. For instance, if the workpiece is 1/2" tall, it should cover at least two full grid squares.

The part must be completely flat on the bottom. Remove burrs, tape, or protrusions. Even better, face the part on one side and then flip it over so the flat side sits against the vacuum.

Additionally, when using the vacuum workholding system, place the Work Home at the bottom of the stock.

This ensures that your tool's depth relative to the vacuum table and vacuum card stock will be as accurate as possible. Because your tools will be getting very close to the card stock, and in some cases machining slightly into the card stock, you'll want to minimize the chance of the tool's bottom height being lower than expected.

To ensure the top of your stock is still accurately represented, make sure to measure the height of your stock with calipers once it's vacuumed down. Then update your setups, regenerate toolpaths, and post process.

When probing the stock, first set the Z to the top of the stock and run the cycle. This will set your X and Y values. Then, go back to the Draw tool and pick a point on top of the card stock close to your stock. Be careful to choose a flat point, because the card stock can warp.

When probing, slow down the rapid to ensure the probe won't collide with the stock.

This second probing cycle will set your Z value, but X and Y will remain unchanged since the last cycle.

When using the vacuum table, do not cut all the way through the stock (to the vacuum card) until the very end of the program. Instead, leave a thin skin (0.005") of material at the bottom to maintain the vacuum seal for as long as possible.

Any cuts through the stock will compromise this seal and make it more likely for parts to shift.

At the end of a program on the vacuum, if you need to cut all the way through the stock into the cardboard, make sure the Bottom Height is no more than 0.005" below the bottom of the stock (Bottom height -0.002 to -0.005" from Stock Bottom).

The toolpath should lightly graze the card stock.

Remember, the vacuum table is not a spoiler board!

Just as you would on the Haas Mill, you must determine minimum part stickout when using the pneumatic vises on the Datron.

This ensures that you don't machine the vise jaws or back edge of the machine.

There are three settings in this dialogue that have been optimized for the Datron.

The toolpath is 2DAdaptive, and the tab is Passes.

If you can't detect them, re-read this Instructable!

The Datron tool library can be found through the Pier 9 CNC Data Instructable (Tool Libraries/Datron).

The Datron post processor can be found at https://cam.autodesk.com/hsmposts .

Search for "Datron Next".

Enjoy working with the Datron at Pier 9!