Before You Do Anything¶
The basics for milling are not…well…basic. This subject can get very deep and intimidating so I will try and present this in a tiered manner. Improving as we learn collectively and as the software (CAM) improves. I am no expert. I learn by reading and trial and error.
Test cuts speak volumes and should be considered a requirement. You should have test cuts that are small but representative of your part. If you are doing a 3D sculpt isolate a small part and mill it out, if you are cutting out a part with a pocket and some holes make a small part with a pocket and a hole. These test cuts can save hours on the actual job, every time you do one I promise you will learn something.
You should have already done some plotting, as shown here. You should have a very clean drawing if you don’t you should not be milling yet. Make sure the pen picks up all the way (clearance plane), and the parts are the right size. This ensure your machine works correctly and you are familiar with the basics of CAM and how your machine moves.
After plotting the next step in milling would be HD foam, (I find it at the big box store “foamular” $5 for a ¼ sheet), this material holds amazing tolerances, mills very well, and will not destroy your machine when you make a mistake. If you are new this should always be the material you make a first test cut in, then on to test cuts in the material you want to use. You can make test cuts on both sides and the $5 it costs will pay for is self many times over in saved bits and refined CAM settings (time & accuracy).
Some of the first cuts ever made on an MPCNC.
For The Impatient¶
If you just want to get the machine dirty here is the generic recipe. This should work in every material, you can optimize later.
- Single flute ⅛″ upcut bit.
- 8mm/s Feed Rate (The speed at which you move through the material).
- 3mm/s Plunge Rate (The speed at which you move vertically into the material).
- 1mm Depth of Cut (The thickness of material your bit will be removing per pass).
- 45% Step Over (The percentage of bit diameter that should be in contact with the material)
- Use the Peel pocketing strategy.
- Always use a finishing pass of ≈10% of your tools diameter. The more dense the material the smaller the finishing pass.
At this point you should be in HD foam, if that works out you can try some soft wood like pine.
If that works at this point the only variable you should be changing is the depth of cut. You can vary this and it will increase the load on your machine in trade for more material removed per pass or decrease the load by taking shallower bites.
Peel, Is usually the best pocketing strategy.
When you get that out of your system come back and learn things a little more in depth.
A More Proper Introduction¶
These are some of the first things you should understand when just getting started. I am going to collect and link all the great resources I think illustrate the point the best. Most of these pictures should link to an outside site for more information. If you disagree with any of the following information please let me know…politely.
An island is that pesky little thing in the center of a cut, like the middle on an “O”, or the center of the logo. Super easy only takes 3 steps.
- Using the Part tool select the inner feature.
- Next is the Hole tool, select the outer feature.
- Then in the Properties box select Island.
A work offset is simply moving your origin. This is typically used when there are more than one operation in your job, multiple fixtures can be used, locating pins, or other locating methods. More typically for us to avoid Negative X and Y moves when using endstops.
- Not Offset
- Offset (Good for Dual Endstops)
A finishing pass allows you to complete your job faster with more accuracy. What?!
By leaving a bit of material on your roughing cut you can then cut off a very small amount of material leaving you with a very accurate final cut with a better surface finish. This means you can rough out your part faster (high machine loads increase deflection) and the finishing skim cut (extremely low machine loads) will bring it to final dimension. All cuts should have this, most importantly slotting operations.
- Just select your finishing tool, usually the current tool you are using. Shown in the yellow box.
- Use a 5-25% tool diameter allowance. Shown in the yellow box.
- The finishing pass is show in the picture as the lighter red path.
Climb vs. Conventional Milling¶
For the most part you always want to Climb mill. The edge of the cutter starts with a large bite and ends small, reducing work hardening and heat retention.
Feeds and Speeds Calculator¶
I can not stress this enough, these numbers are different for every build. Only use them as a guide to find the right settings for your build. You can make a few test cuts a quickly work out how to get reliable numbers for your machine with the right settings though.
- All things being equal, this is the amount of material your tool encounters in percentage of the tool diameter. The lower the percentage the lower the force on the machine, the more accurate the cut.
- A good thing to know is most flutes are not 50% of the diameter of the bit, usually less. Just typing in a percentage does not mean that is the actual chip load, Feedrate, RPM, and Depth of Cut all play a major part. All the numbers you enter are a fine balance of an equation giving you total chip load per tooth.
- is 50% or less, typically 45% depending on material density. More than 50% you will be both climb and conventional milling and should be avoided.
- is 20% or less depending on amount if detail and tolerances desired (I typically use 2-8% time vs. quality), ball endmills should use 10% or less to minimize scalloping.
Dual EndStop Tool Changes, Z Probing¶
For this method you will need the Dual EndStop firmware, an LCD, optionally a digital spindle speed controller.
The pause here is to allow you to remove the Z probe wires.
G90 ; Absolute positioning, just in case G92 X0 Y0 Z0 ; Set Current position to 0, all axes G00 Z5.0000 F500 ; Raise Z 5mm at 8.3mm/s to clear clamps and screws G28 X Y Z ; Home in order, w/zprobe G92 Z0.15 ; Account for probe thickness (set your thickness) G00 Z5.0000 F500 ; Raise Z probe off off of surface M00 ; pause for LCD button press M03 S<s> ; PID, set spindle speed
The steppers are disabled so you can move the head to an area where you can more easily change the tool, make sure you do not let your Z axis drop onto your work surface. If you need you can insert another pause before the steppers are disabled to make sure you are there to catch it. This first pause is to let you physically change the tool and install the Z probe. The second pause is to allow you to remove the Z probe.
M05 ; PID, Stop spindle G0 Z35 F500 ; Raise Z axis 35mm M84 ; Disable steppers M00 ; Wait for LCD button press ;Change tool: <n> G28 X Y Z ; Home in order, w/zprobe G92 Z0.15 ; Account for probe thickness (set your thickness) G00 Z5.0000 F500 ; Raise Z probe off off of surface M00 ; pause for LCD button press M03 S<s> ; PID, set spindle speed
Make sure you tune the final Z lift to your machine.
M05 ; PID, Turn off spindle G0 Z30 ; Lift Z axis 30mm ; M84 ; Optionally turn off steppers.
If you do not have a PID controller you do not have to remove or worry about the code. This is the basics, you can easily modify this.
Depth of Cut¶
Equal steps – Depth of cut, DOC, Should be planned for. Making equal steps will produce the best results. Just because you can cut deeper doesn’t mean you should. Know the deepest you can cut your material and from there divide the cut equally. The only way to save time is less passes, if you can not save a pass make the step smaller.
Through all – Through all cuts, cuts that are intended to go all the way through the material, should move past the bottom of your material. The amount past depends on the flatness of your build, all build have some sort of variance. A 0.5mm-4mm would be pretty typical. Factor this into your equal DOC from above.
When making Gcode from your CAM program it spits out raw coordinates, speeds, and a few other commands. A post processor simply formats in a way that your firmware will recognize it.
For example, Marlin treat
G0 (rapid move) and
G1 (Work move) the same. Other machines set the
G0 speed in the firmware, Marlin does not. To over come this we Use a line in the post processor
to set the actual speed in each line so it doesn’t matter. There are all sorts of things like this.
All machines require a post processor.
The ones we have working¶
Please share your links to other PP’s. I know there are more.
- Built in, Christian was happy to work with us to get this correct. Here are the recommended settings
- Guffy has really made what seems to be a feature complete PP here, Guffy’s GitHub. Fusion CAM intro.
Fusion’s free plan no longer supports more than one speed, so the feedrate for XY turn into very fast Z movements. More details in the forum here
(10/23/19) Do not use arcs unless you are using 417 or newer firmware.