Your not pocketing that circle, right? Just removing the pieces can save a ton of time on but pockets. I try to limit pockets too places where I’m not going all the way through, or they are very small.
EstlCAM has a little estimate on the preview window. It’s been low by about 25% or so for me, but it gives me an order of magnitude.
What thickness is your material?
For the plunge, do you have the plunge angle set? That helps a lot, because it will drive into a cut instead of trying to just drill into it. The bits (especially ones not designed for milling) don’t remove material in the center when plunging, so you’re just pushing that wood, and it caused a lot of stress. If the bit is moving when plunging, then the sides are cutting and you get a lot less stress. I also had trouble with the plunge with the default pocket strategy, so I use parallel or peel.
For speeds, and DOC, do some tests in the material. I can’t tell you what to use, you have to try it on your material. If it’s anything thicker than 6mm ply, then you’re pushing it at 15mm/s. Deeper and faster are trade off, but deeper uses more of the bit (which makes them wear better). If you’re not using a but designed for milling, then you won’t get as good results as Ryan is.
You’re not just tuning the machine, you’re training yourself. Make some coasters first.
My estimated settings on this project would be 6mm per Pass (8mm 2 Flute bit) - 10mm/s . 90 degree plunge angle with 5mm/s plunge feedrate. Material is 18mm thick.
The big circle will be a full thickness cut.
Haven´t noticed that time window in preview Learned another thing, hehe!
I just tested bits like the bits that come with the makita router.
Cuts through, but leaves some tearout.
Will try with a “more expensive” specially for cnc milling designed bit.
And one more:
Would it make sense to choose the smalles bit possible in terms of mechanical load? I mean…I don´t need to cut away 8mm width, 6mm or less would totally be okay for the parts.
Yeah, a real endmill will work much better with cam software. Woodworking bits are usually very specific to one material or type of cut. Example, most people are trying to mill with really long drywall bits…
Can you find where I said 15mm/s I need to change that for sure. I have been milling 6mm MDF in one pass at 8.3mm/s 15 is not my style at all. A vary all my cuts between 8-12mm/s
On plywood specifically, upcut bits and cheap plywood will create a lot of tearout. A downcut bit leaves a mess on the underside, but it’s a lot less, since the spoil board is pushing against it. The problem with downcut is that they don’t get the chips out as well, so drilling anything is not good, and deep cuts have more load.
Better quality plywood has more glue on the top veneer, so the tearout won’t do as much damage.
I think changing the plunge angle will help. Diving straight down 6mm has some danger to it. The bits don’t have a cutter in the middle, so it’s just pushing that center. IIRC, I used 45 or 30 degrees.
I started trying to write up a milling basics page but dang, there is nothing basic about it…I will try and get something up and maybe I can just keep improving it as we go. These questions come up a lot and I am not doing my part in getting any help up.
What kind of plywood are you cutting? Ive been cutting alot of 1/4 birch, which really measure around 5mm. I cut all the way through into a foam spoilboard at 15mm/s. Ive had the most sucess with
and
Ive also cut some 12 mm birch plywood, that I cut in 3 cuts, 4.5mm DOC per pass.
The other day I tried some 1/4 underlayment because who doesnt like 1/2 the price of birch plywood and I was just cutting out some simple shapes…that stuff sucks, ruined a couple bits and I had to bout about 7mm/s.
Compression bits are supposed to help with tearout, but they are no panacea. They are upcut near the tip and downcut for the rest of the bit, … this is why tearout is limited. But these bits are a bit more expensive.
I purchased a few from the maslowcnc project (.25" diameter, 1" cut length, about 2" overall length, but this is from memory). The bits look good to me. You can get some to try from www.maslowcnc.com/store … I don’t know where they purchase the bits. I have not used one yet.
I delete all the default tools and use this as a conservative test speed setting for an 1/8″ flat endmill in wood. Do not exceed 8.5mm/s in the z plunge field.
Does the MPCNC run at 15mm/s well? This may be a symptom of one guide for multiple machines. Growing pains
Yes, yes, yes. This is great. Precise information, conservative settings, some good rules of thumb.
Pictures are great too. I was told by a very effective salesperson that people either read or look at pictures, but not both, so you have to explain your most important things in text and images.
Ok need some feed/speed advice.
I want to cut and pocket some 25.4mm (1”) Mdf.
I’m using a 1/8” 1F upcut 32mm long due to the size of my Mdf. I have depth passes at 3mm.
Tell me if I’m on the right track with my settings.
14mm/s (840mm/m) feedrate,
3mm/s (180mm/m) plunge,
10000rpm spindle.
This gives me a chipload of 0.042mm /tooth (1.0668“) based on fswizard under wood(no Mdf option).
However recommended chipload for Mdf is 0.102mm-0.1778mm (.004” – .007”).
My pockets are estimated to take 6+ hours using the standard safe milling parameters as stated in the guide, so I do wanna try and lower this time but at the same time be on the safe zone as well.
I know the only way is to trial as every machine is different, but can anyone advise me on a good safe and speedy (and successful) setting just to get this done as I need this to finish off my lowrider controller board. (I’m making a panel for the vfd, control panel etc as I’m removing the exisiting Makita.
Once this is done and all rewired, then I can start experimenting with settings in my new setup.
Also, when using endmill parameters, such as fswizard, what parameters do we need to basically not exceed, such as cutting force, what would you consider is the limit for the lowrider3.
And with fswizard, if I can’t achieve the required chipload even when using my min or max limits, what are the tricks. Eg. 2flute upcut shows half the rpm of a 1F upcut, my spindles min speed is 8000rpm, but the fswizard is calling for 4000rpm. But if I set the 4000rpm to 8000rpm it adjust feedrate to like 30+mm/s(1800mm/m) which would exceed the lowrider I believe.
That speed does not exceed the LowRider, and if your firmware has a max limit holding you back, you can edit to change that. Also, there may be speed limit settings in your CAM software that can be edited. I have run my LowRider much faster than 30+mm/s. On some cuts I’ve run it faster than 80mm/sec.
Ohh that’s good to hear. My cam is vectric.
Where in the firmware would the limit be for me to edit? And what would you suggest the high limit be? 50mm/s? 100mm/s?
:
