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 1/4 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).
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 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)
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.
Always use a finishing pass of 10%-25% of your tools diameter. The more dense the material the smaller the finishing pass.
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.
Click on the images for a larger view.
Basic- 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.
Expanded-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.
Roughing 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.
Finishing 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.
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.
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.
- Estlcam – Built in, Christian was happy to work with us to get this correct. Here are the recommended settings.
- Fusion360 – We have two. V9 and a total rewrite. I have not spent enough time with the rewrite I assume it has bee kept more up to date.
- Vectric, Aspire, Vcarve – What we have so far, Here.