Guide to Milling Aluminum Plates for MP3DP v5 with EstlCAM

I have just recently embarked on building myself an MP3DP v5 (Forum thread). I decided I would mill the Aluminum plates myself because why not? This is why I built myself a CNC to begin with…I wanted to be able to make things.

My intent here is to detail, as much as I can, how I went from only ever milling MDF, to successfully milling my MP3DP v5 aluminum plates without any major setbacks. There seemed to be some interest in my build thread for some help tackling this job.

!!! Note: Although this all worked for me, there is no guarantee that everything I did will exactly work for you. You still need to do your own tests. My machine is as basic as it gets, so this should be achievable for everyone. If you intend to take some of the advice in this post, please make sure to read EVERYTHING first

My success was made possible with help from @Jonathjon and @vicious1. My goal is to pay it forward and help reduce the barrier of entry for anyone who wants to be able to mill their aluminum printer parts for themselves.

I am not an aluminum milling expert, or even a CNC expert, so please keep that in mind, and if anyone has anything to add below, please do.

My Machine

I have a basic 4’ wide LowRider 3 running the corded Kobalt trim router. Build Thread

I do not have a coolant or air system installed.

The only bits I used were the 1/8" single flute(this or this) and 1/16" 2 flute(this) end mills from the V1 shop

My Settings

I used EstlCAM V12. Please make sure you are using the latest version, 62 or later, due to some very important bug fixes that will help these settings work correctly.

The settings I used to cut the plates are using trochoidal milling. Trochoidal may not be the best way to do it, and it is absolutely not the fastest. It is, however, very beginner friendly. I think it’s more than 2x slower than normal cutting, but if you are new to milling aluminum (like me), I very much recommend starting here to get a feel for how your machine and bits react to the settings.

Also, if you don’t have coolant or air setup, I think the trochoidal milling can help keep the bit a little cooler. It also might be a bit harder on the machine the way it jerks around.

These settings were taken from @Jonathjon, then I backed off of his settings a bit first and worked up to what I was comfortable with. I suggest anyone else do the same if they take my settings below.

My settings are:

I do not have a speed controller so the RPM settings may not be accurate. By the end, I settled on running at Speed 2 on my Kobalt Router and it seemed to handle it fine. I believe @azab2c has a video somewhere where he tested exactly what speed that should correlate to. Maybe he can link it below.

Also, make sure to include a finishing pass on all of the Hole and Part cuts. This will make sanding afterwards waaaaaay easier.


I purchased the following 12" x 12", 3/16" thick aluminum plate here

I was able to mill all plates from this one sheet. I don’t think I could have used a smaller sheet. Bigger is fine, but 12"x12" is the minimum amount of area I would attempt to fit it into with these settings

My Setup

I did not want to attempt hours straight of milling aluminum, so I decided I would prep ahead of time, and make sure everything I did was repeatable. I then planned to make CAM programs for one piece at a time to start

So here’s what I did.

  1. Load 1/16" bit into router
  2. Home Z, Home X, then Home Y
  3. Turn on router and Move -Z until bit is just barely cutting 0.5mm or so into the spoil board
  4. Move +Y200, Move -Y200, Move +X200
  5. Raise machine and turn off router.

This drew a mounting guide where the bottom left corner was at exactly (100,100) and the edges were exactly square with the motion of my machine. I then mounted the aluminum plate with a screw at each corner. (Read the CAM setup section below before drilling holes)

This meant that no matter what happened, I had a repeatable starting point to be able to continue after mistakes, etc.

Spoiler Alert: This came in handy more than once :grin:

CAM Setup

In EstlCAM, I set up the grid to be 1" (25.4mm) squares so I could easily see and layout all my parts and make sure they fit within the 12"x12" area to be cut.

I chose the following layout:

Note: Be sure to add all items before you make your first cut, as EstlCAM will move the Zero point when you add a file. You can also maybe add something into the file that can be used as a reference point in case you lose your Zero point, to be able to easily recover your exact zero from before the add.

Final sheet after all cuts:


I didn’t have any…

So I ran a bit of a manual air assist :grin:

I lowered the PSI on my compressor to around 25 and used that with an air gun to help evacuate chips and cool the bit. Yes, I actually stood there blowing air on it by hand the whole time…

Cam Tips

V1 logos

All of the V1 logos look better when cut with the 1/16" bit. Use a finishing pass.

Holding tabs or not

I decided against using holding tabs. Instead I would plan to screw the part down to the bed by pausing the job before it did the final Part cut, and insert screws into holes, making sure that the holes I picked were far enough away to not hit the bit.

Along the way, I also decided to print some screw “cushions” to stop the screw from marring the surface, like this:

I took a cue from @Jonathjon and instead of trying to manually pause the job, I manually edited the GCode before transferring it to machine, and inserted the following gcode:

(Move away and pause for screws)
G91 (set relative mode)
G0 Z10
G0 Y250
M0 (Insert Screws)
G0 Y-250
G0 Z-10
G90 (set back to absolute mode)

Please test this code before using it on your machine to make sure it works as you expect


EstlCAM will not automatically order things in the way I wanted, so I manually overrode the order. My preferred ordering was…

  1. All 1/16" cuts
  2. 1/8" drill tool paths
  3. 1/8" holes, smallest to largest
  4. Part tool paths (these will be last by default)

If you don’t order these yourself, you may end up with extra bit changes


I used the Gcode above sometimes multiple times in a program. As I got more comfortable and was making programs that cut for longer, I started using the pause more just to let my machine and bit cool.

So, for instance, after all of the drills, I would insert the pause. Then when the program ran, I would let it pause, turn off the machine, and hit it with some compressed air until the bit was cool to the touch.

For now, this is all I can remember. I will update this post if I think of anything else useful pops into my head.

I hope this is useful to someone and I didn’t leave out anything major. Please ask as many questions as possible and @Jonathjon will answer them all :laughing:


Very awesome write up @Michael_Melancon and great job on all your parts! Idk if I’m the best one to answer any questions but I’ll sure try to help where I can. You got all your parts the first try, I messed up a few and then ultimately messed them all up and now I’m re-cutting them all LOL. None of those were LR problems, they were all yours truly LOL


Well, while I did get them all completed on the first try, I don’t want to make it sound like there weren’t issues.

Luckily, the mistakes I made didn’t ruin my parts.

I do have some extra holes and stuff in places outside of where my parts were though…

Some of the prep I did because I was scared of ruining my sheet helped a lot in being able to save myself a few times.


Yes your well thought out placement and all is a huge time saver and screwup saver lol. Good job!

For this section here. The easiest way for me to find where to put this…

Open the .gcode file in windows notepad
Click Edit - Find
Type: Part
Click find next. It will take you straight to the first part operation, which is usually the last operation in Estlcam. There is a single line gap just above it and that’s where I put mine. I do my code a little different but that doesn’t matter in the end.


Thanks for pointing that out. I did the same.

After exporting the file, I would leave EstlCAM on the Preview so I could easily see the order and know exactly what text to search when I had multiple places I wanted to add them





Nice results and write up. Appreciate learning what’s working for you. Cheers!

Sure thing…


I do mine in this order except I put the 1/16th at the end, that way most of the material is gone, and this is just cleaning up corners.

I did use your DXF organization method. It does help a lot and when I did for get a toolchange I was able to go back and just do the small logo cut and it was flawless. Excellent tip!


Yeah he waited till I had already started to share that tidbit LOL.

I think I would have done it opposite though. I only use the 16th for the real small logo cut outs. So I would have just done the entire plate worth of those from the get go as one job. That’s what I am thinking about doing with my redo anyways LOL

As I got towards the end and was doing bigger batches, that was how I was doing it.

All of the 1/16" stuff first, then all the drill holes. Pause. batches of 1/8" holes, then each part with a pause in between.

With your faster settings and it being possible to do it in a reasonable amount of time, breaking it up by small holes and drills, then all of the bigger stuff, you should have 2 manageable halves of time where if you need to step out at the pause you’d be fine to

That’d be a lot of screws and pads though lol

I have plenty of screws lol. But only printed 12 washers. But that’s just a quick print to get more! Laying mine out now then will see how many more I need to do it that way

Plumbers washers at box store would work well also!

1 Like

There are a couple of benefits, in my opinion, to using the printed ones if you have a 3D printer and can make them

  1. There’s not a lot of clearance between the holes and part tool paths. Being able to size them exactly to the screw head helped. in some cases I was just 1-2mm away from where the bit traveled.
  2. I wanted them to be very rigid to keep the same downward pressure on the part as the screw did to make sure it didn’t move. I don’t know how dense that rubber is or whether it would be a problem, but the plastic held very well
  3. Printing 24 of them is only like $0.10 in plastic
  4. You get to use your printer to make something useful lol

Did you ramp into the material, or just do a straight plunge?

With Trochoidal it does a spiral plunge down. No need to do an angle plunge. Its nice and gentle. Like a helical drill function.


An end mill will cut through a rubber washer like butter. I wouldn’t worry about the size of the washer at all.

I would worry about because I don’t really want the rubber all over my bits, and because multiple $0.15 washers per cut would get expensive.

That’s roughly an extra $7 or so per sheet of MP3DP v5 parts if you cut it all at once, versus $0.30 max of printed ones that are re-usable

1 Like

I used mine again to hold down polycarbonate sheet for the panels :partying_face:

Here is the file for the washers I was using. AFAIK they were the same dimension’s as Mikes

Aluminum Screw (31.5 KB)