Introduction: How to Mill Tall Stuff Using Not-So-Tall Endmills

So... I recently wanted to mill something that was 11 inches in height, but only had 3-inch-long endmills available.

This is how I did it. There’s no magic, but a couple of tips and tricks that might be useful.

Spoiler Alert: I ended up milling 4 separate pieces and gluing them back together.

Read this as a how-to, or as an intro to CAM... I'm mostly interested in documenting it now so I don't forget how I did this stuff.

Step 1: Breaking Up (a Model) Is Easy to Do ...

I had a design I wanted to mill out of MDF, but it was taller than the endmills I had available.

First thing I did was calculate how many sections I needed to split my model into, and roughly how tall those sections should be. Given that my model was about 11 inches tall (280mm), and my longest ball nose endmill was 3 inches long, I divided my model into 4 sections of roughly 2.77 inches each.

Before splitting the model, I added some registering holes through the whole thing, so I could easily put the final piece back together using some support wooden dowels. I used 5 holes, 3 that go all the way through, and 2 that only go through 3/4 of my design.

The diameter of the holes were selected based on the drill bits available. I initially wanted 1/8” holes, but didn’t have any 1/8” bits that were longer than 2 inches. I ended up using a 7/16” bit because those are pretty long, and I had 7/16” wood dowels available.

Actually splitting the model should be easy to do in any CAD tool. I have my design in Fusion 360, and breaking up a solid body can be done using offset planes.

Planes can be constructed by using the Construct -> Offset Plane menu option, and entering the offset amount. Once those planes are created, the Modify -> Split Body tool can be used to actually split the body into its 4 shallower parts.

I then aligned all the pieces vertically (using the Modify -> Align tool), and arranged them in a way that seemed area-efficient. The overall area for my model is about 730mm x 500mm, or 29” x 20”.

The model should now be ready for CAM’ing!

Step 2: Stock

Actually, before setting up the CAM, it’s a good idea to prepare the actual stock of material that is going to be milled. This way its exact measures can be put into the CAM software.

I decided to use MDF because it’s soft and porous. It’s definitely not light, but it’s soft and porous.

Since I needed a block that was about 29” x 20”, and MDF comes in panels measuring 48” x 96”, it was easy enough to cut six 32” x 24” pieces. And since the panels I had were 1/2” thick, I got away with cutting just one large panel, to make a final block that was about 32” x 24” x 3”.

I made the block by gluing all the panels with wood glue, and clamping them overnight. The block was then affixed to a 1/2” thick piece of plywood with double-sided tape and a couple of screws.

Step 3: ​Stock Options!

I used the beta version of CAM 360, which I got by signing up here.

Before starting a toolpath in CAM 360, it’s a good idea to turn on the origin visibility in the modeling environment. This helps set up stock orientation.

Then, first thing to do is set up the stock. This was done with the Setup -> New Setup menu option. For Work Coordinate System Orientation, I chose the “Select Z axis/plane && X axis” option. Then, clicked on the model’s axes that I wanted to use for X and Z orientation (this is why it’s good to make the model’s origin visible, it gives me an absolute coordinate system to pick from). Sometimes I had to flip one or both of the axes in order to get the correct orientation for my stock and model.

Then, I chose “Stock box point” for the Work Coordinate System Origin, and picked a point on the stock. For this path, I chose one of the upper corners.

Since my block was about 32” x 24” x 3”, but my model only 29” x 20” x 2.77”, I had to add stock offsets to almost all of the sides. The only side I didn’t add anything to was the bottom. I wanted the model’s bottom to be flush with the stock bottom.

Step 4: ​CAM Rules Everything Around Me!

Once the stock was all set up, I started with tool paths. First, I set up a Face path, using a 2-inch facing bit. This was used to take out the excess 1/4” of material from the very top of the stock.

Then, since I didn’t need a whole lot of precision or tight turns in my design, I decided to use 1-inch endmills for roughing and finishing. The roughing path type I used is called Pocket Clearing, and it was easy to set up. A couple of important options I modified were the step-down amount, the overlapping amount, and the feeds and speeds. I set the step-down to 10mm, which is a little bit larger than 3/8”, and the overlap to 10mm, which is a bit less than half of the endmill radius. Feed was 5080 mm/min and spindle speed 4000 RPM.

I also set the bottom limit to be 2mm above my model’s bottom plane. This was to make sure that the roughing pass didn’t go all the way down to the plywood and released the pieces from the block.

After roughing, I set up the drilling for the registering holes. If this was harder wood, or metal, I would have been more careful and used some kind of pecking routine. Since MDF is soft, I could drill all the way through in one pass with a slow feed rate.

This was done by selecting Drilling from the top menu, and selecting the hole geometries in the model. I used a spindle speed of 10000 RPM, and a plunge feed of 1000 mm/min.

After drilling, a finishing pass using the Scallop option under the 3D menu. Feeds and speeds of 5080 mm/min and 7000 RPM, respectively, and a Stepover value of 2mm. Also, to make sure the sides of the shapes were being milled, and not just the tops, I had to add an Additional offset of 12mm (half of the tool diameter) to the Machining Geometry Boundary. Smooth!

Step 5: Pop It Out

Only thing left to do was a final pass with the roughing bit to release the pieces from the bottom of the block. This was done last, as a separate path, so I could make sure the pieces I was cutting out were still stuck to the table with the double-sided tape after all the other passes. This was an easy path. All I had to do was select the four bottom faces, and make sure to only go through once, with a starting height of 2mm above the model’s bottom plane, and a finishing height a couple of mm below the bottom plane.

And that’s it. I could then run the Post Process script from the Actions menu to start exporting some G-Code. In the Post Process export options, I had to select Inches for the units because, even though g-code can be generated in both inches and millimeters, some of the pre-programmed routines in the machine I was using were hardcoded to inches, so it made sense to just use inches throughout. Also, I had to make sure the program number and file name were made up of exactly 6 numerical digits. Or else it didn’t show up in the machine. And, increasing the G51Lookahead value to something like 0.002 or 0.005 sped up the milling process. The G51 code is actually a lookahead tolerance value. This is how close the machine’s head has to get to a target before it starts executing the next movement.

Step 6: Mill !!

Making chips! And dust!

I think I took a good 6 hours to mill this, mostly due to inexperience and caution.

For example, instead of running one long program, I broke up my job into separate files/programs, so I could clean up the work area between paths. This helped keep dust down, and also gave me a better view of what was happening.

Overall, there were no big problems.

Step 7: Assemble, Sand and Finish

Once the pieces were out of the machine, I put dowels in the registration holes, and started gluing the layers together. I was able to apply pretty good pressure while gluing the first 3 layers together, but since the last one didn’t have a nice flat surface for clamping, I waited and glued it separately after the others had already dried in place.

The dowels were then chopped with a small handsaw, and the gaps between the dowels and the MDF piece was filled with a paste made of sawdust and wood glue.

After waiting for the glue to dry, a bit of sanding was necessary in order to get rid of any grooves, marks, lips and bumps on the surface of the piece.

And, voilà, an 11-inch model made from 3-inch bits!!