Alright, so I finally got Bob Warfield
installed and I learned a few things from it. I'm following the guide here
if you want to follow along. I'm going to be mixing a bit of software review into this post.
The basic question I am trying to answer is: Theoretically speaking, how fast and how deep can I go and still have a good finish?
I'm asking this question because it helps me set all other targets - how fast I can reasonably expect to cut a sheet of parts, how long I can expect a tool to wear, etc. A lot of this is dependent on my CNC router - which is fairly overbuilt. Big motors, strong drives, 12Krpm spindle, etc. So for now I'm just concerned about the feeds and speeds and how they interact.
First things first: Here's the feeds and speeds calc in GWizard. It's not the prettiest thing, and it's not always easy to tell what's a button. For example, the little "gauges" are also buttons - cut optimizer buttons. This took me a lot of blind clicking to figure out.
Note my selections: Machine
-"VMC" - for machining center. I chose this since I couldn't choose "wood router" and because all the other options looked specific to a certain machine. I am assuming this is the generic choice. Material
- Wood:Plywood - obvious choice.
- right now I have HSS (High Speed Steel) downcutting 2-flute bits from Onsrud - but more on that later. Tool Diameter
:1 (guessing this is in INCH units though it is not explicit).
Now, with those settings, I get some disappointing - almost unbelievable - results. GWizard is telling me I can only take .03" off the plywood at a time! At that rate, I would have to take TWENTY FIVE passes to get through the material. That is unacceptable no matter what.
The basic idea of the cut optimizer revolves around having less than 1/1000th of an inch of tool deflection. I agree with that figure and don't want to push more than a thousandth or two - so I have to change something. The first, and most obvious thing, is stickout
. If I change the stickout to .8 inches, you can see that the Depth of Cut doubles:
However, that still means TWELVE PASSES. Unacceptable, but I can't make the stickout any lower - the material is .75" thick, and I want to be able to have some margin for error above the material. So I'm going to switch the type of tool to Carbide Endmill. Interesting! Now GWizard is reporting that we can cut .2577 - over our target depth! This may also help explain why Fab52's CNC operator had troubles with bits breaking
Now here's a complaint. The optimizer does not seem to accept any spindle speed faster than 7500 RPM. This is unfortunate because many routers like mine run at 12,000RPM. Because my spindle is air-cooled, it needs to be run fast to stay alive. So I prefer the higher spindle speeds. Anyway if I go back to the main interface and update the spindle speed to 12,000 RPM, GWizard updates the Feedrate to 287.749 IPM. 300IPM is a pretty good rate for a wood router like this. Due to the intricate nature of these parts, I don't expect we'll ever exceed that by much.
So that's what we can do with a 1/4", Carbide endmill. ~300IPM between 7500 and 12,000RPM at .2577" passes. That means three total passes for each scanner, which seems very reasonable to me.
Another possibility would be to use a 5/16" endmill... could play with that next.