I’ve had my Onefinity for about a week now; it’s my first CNC machine. I’m still in the process of cutting out the wasteboard, L Brackets, and cam clamps. While cutting out the wasteboard & L Brackets, I’ve noticed that the pocket cuts for the mounting holes are fairly quiet, but the outside profile cut is very loud and high pitched. I’m using the Amana Tool 46577-K 2-flute upcut bit and I chose a feedrate & RPM that matches the low-end chip load of .006 to cut the MDF. The pictures below are my settings in VCarve Pro. I’m using a 1" ramp and about 2.5 on the dial of the Makita router.
Since I don’t really know what the cutting is supposed to sound like, is that normal? I’m not seeing any burning on the MDF.
Matt - generally I would say sounds like that are ‘normal’. I usually get it with Maple and other hard woods. However, my gut says 180ipm is really fast at 0.2" DOC. Though I just plugged your end and material into our new CNC Explorer app and it says 144 is optimal, with 120-168 being the range. So, a little fast than recommended but close; I can’t say slowing to 144 would make a huge difference in the sound. YMMV. Hope this helps.
Looking at the spec sheet it appears to be tapered which might mean the deeper you cut you end a slot you will have full contact with both walls of the slot you are cutting. The Amana recommendation would be to slow your feed rate by 50% at 3x diameter depth of cut. I don’t know what RPM a setting of 2 would correlate to, the recommended feed rates from Amana are generally at 18000 RPM.
Thanks for the info…I’ll try the slower feed rate tomorrow. I’ve tried to use the CNC Explorer app and created a login, but it says Demo Limited Trial at the top and says I need a license to create recipes.
Unless I am mistaken the definition of the bit is incorrect. The diameter of the bit is set at 0.25 when it should be defined as 1.0. When I did my spoilboard I set my Makita on 2 and ran very shallow depths like .05. I put pencil marks across the spoilboard and just shaved off the top until the pencil marks were all shaved off.
The profile cuts are made with a 1/4 diameter upcut. I believe you are referring to surfacing the board, which is unrelated. 1/4 inch is the correct diameter. Thank you for your input though.
High pitched sounds or sounds that go up when cutting are bit shearing where the bit is not taking a big enough chip and is rubbing the wood. This is a sign that speed is to SLOW. You need to increase feed rates.
When the sound starts to bear downwards or get loud in the bogging down sound or the router is struggling that is when you have too much speed or ipm.
This bit on mdf should be running 300-350ipm at 15000 rpm. at .25doc
When the sound goes up to a scream you are too slow and when the sound goes down to a roar you are too fast.
You can see the amana recommend speeds are 215-290 and those are conservative. Mdf ususally has a chipload around .011-.013 which is why i said 300-350ipm
Everyone needs to understand that if you run your machine too slow you are doing more harm to the bits than running them at proper speeds. Heat is transferred from the bit to the wood during the cut and if the chip is not big enough then the bit holds the heat and gets hot. Running the machine too slow ipm or not deep enough causes the bit to not take a big enough bite and cannot transfer the heat to the chip.
I cut out 2 cam clamps from MDF last night. One with a feed rate of 140, the other with 250. Both at setting 2.5 on the router. They both sounded to train horns, but the faster one appeared to eject chips better. Once I finally get my wasteboard, fence, and clamps done, I’ll experiment more with the feed rates.
Okay, so I set the router dial to 3 and cut out some more cam clamps. Below are the settings I used and a short video of the sound. BEWARE, it’s loud so adjust your volume. Does this sound right?
Reduce the stepover to around 32% and increase your plunge to 125. Also you should Input the spindle speed as 18000 so the software reports the correct chipload. Right now it says you are past the max chipload for that bit.
The cut is calculated as it moves around the pattern and this is a factor to how much of the bit to use during the turns. The plunge is how much material is removed as it goes down and the rpm calculation for chipload so those are factors as well.
On Amana bits there is a line where the the bit should sit in the collet make sure the bit is at this line and not too far out of the collet.
