Bit Digs into work on hard wood rough cuts

New Home Forum Mostly Printed CNC – MPCNC Troubleshooting – MPCNC Bit Digs into work on hard wood rough cuts

This topic contains 3 replies, has 2 voices, and was last updated by Profile photo of UnLtdSoul UnLtdSoul 3 weeks ago.

Viewing 4 posts - 1 through 4 (of 4 total)
  • Author
    Posts
  • #37129
    Profile photo of UnLtdSoul
    UnLtdSoul
    Participant

    Hey, I’ve been happily using my MPCNC for over a year now. Mostly I’ve been doing V carving and have done some 3D relief work with various woods now and then. For most of them I skip the rough cut and have been just doing the finish cut. But, in my current design the cuts are too deep and I’m using Hard Maple and so I have to do a rough cut first.

    Maybe I am just pushing things too fast? But, I am having a problem and was looking for some advice on what settings others are using. I use the DW660 with a manual speed controller – I usually set the speed to about 40-50% spindle speed. I am rough cutting with 1/4″ bit, I have tried a straight 2 flute bit and a 2 flute up spiral, and get same results on both.

    I first was cutting at 3000 mm/min (118 inch/min) at 1.2 mm depth per pass. It will seem to be cutting fine for the first 1-2 passes, then all of a sudden you can hear the spindle slowing down and the bit starts digging down into the material. Usually the x or y axis will also get off and i have to hit my emergency switch and stop it.

    I tried cutting at half the speed 1500 mm/min – or 59 ipm and it did the same thing. Am i pushing it too fast for hard maple? Actually, it has been months since i cut with 1/4 i need to keep a written list of good settings. But, since I’me only cutting 1.2 mm per pass, i would think i should be able to at least cut at 100 mm/min. A lot of people (using pro CNC machines) talk about a cutting depth equal to the bit diameter… that would be 6.36mm I am not cutting anywhere near that deep.

    The other part of my question or concern is, why does the bit dig down into the wood? When I say it digs down, it will dig down at least 1/4 – 1/2″ (into 3/4″ stock) and yet it will still often be cutting forward but the x or y will skip and get off because they can’t take the amount of force to stay on course at that depth. And, as it goes deeper down you hear the spindle slowing down because of the added power needed to cut at that depth.

    My point is, I am not sure if it is the spindle that is slowing down first (like it hits a harder spot in the wood and slows down) which is causing the problem, or if it is the Z axis that is too weak and somehow it starts dropping, and as it digs down and cuts deeper that is why the spindle slows down? What I am getting at, is, do i need a stronger Spindle motor or a stronger Z axis motor? I currently have an 84 oz/in Nema 17 motor on the Z-axis. I see there is a low current (1.8 amp) Nema 23 that has ~340 oz/in torque. That would give me 4 times the Z axis strength and would help to keep the bit from digging downward. (Sometimes, however, the bit will pull out of the collet – so i am not really sure a weak Z axis is the problem.)

    My MPCNC is modified. That is, I have 2 pipes on both the X and Y axis, and have 2) 3/4″ plywood platforms on the Z-axis, which gives it a lot more strength – and my table is 3′ x 4′ (have middle feet on all 4 sides, so 8 feet all together – the unit is fairly solid.

    #37141
    Profile photo of Ryan
    Ryan
    Keymaster
    Hey, I’ve been happily using my MPCNC for over a year now. Mostly I’ve been doing V carving and have done some 3D relief work with various woods now and then. For most of them I skip the rough cut and have been just doing the finish cut. But, in my current design the cuts are too deep and I’m using Hard Maple and so I have to do a rough cut first.
    Maybe I am just pushing things too fast? But, I am having a problem and was looking for some advice on what settings others are using. I use the DW660 with a manual speed controller – I usually set the speed to about 40-50% spindle speed. I am rough cutting with 1/4″ bit, I have tried a straight 2 flute bit and a 2 flute up spiral, and get same results on both.

    1/4″ is large for this machine, 2 flute adds to this. what stepover and what clearing strategy are you using?

    I first was cutting at 3000 mm/min (118 inch/min) at 1.2 mm depth per pass. It will seem to be cutting fine for the first 1-2 passes, then all of a sudden you can hear the spindle slowing down and the bit starts digging down into the material. Usually the x or y axis will also get off and i have to hit my emergency switch and stop it.

    3000=50mm/s that is faster than I set my rapid travel moves at… To give you an idea in IPE (much more dense wood) I used 1/8″ 2 flute end mill, at 2.5mm DOC 15mm/s with a 45% stepover and a peel/adaptive pass to get a proper bit load. Have you checked for perpendicularity of your cutting tool, I have a little test part on thingiverse.

    I tried cutting at half the speed 1500 mm/min – or 59 ipm and it did the same thing. Am i pushing it too fast for hard maple? Actually, it has been months since i cut with 1/4 i need to keep a written list of good settings. But, since I’me only cutting 1.2 mm per pass, i would think i should be able to at least cut at 100 mm/min. A lot of people (using pro CNC machines) talk about a cutting depth equal to the bit diameter… that would be 6.36mm I am not cutting anywhere near that deep.

    Careful comparing this to a $200k+ machine not really the same.
    1500=25mm/s. I choose a feed rate that works well for my machine 8-15mm/s, and a bit appropriate for my spindle 1/8″ single flute (because the 660 is high rpm) with adaptive or peel as a clearing strategy, I feel a 1/4 in dense wood is asking for trouble. So using those basic settings I do a few test cuts to see how deep I can cut per pass. You might find you can do a full depth. For roughing the less passes the faster it cuts, 2 5mm passes is much slower than one 10mm pass.

    The other part of my question or concern is, why does the bit dig down into the wood? When I say it digs down, it will dig down at least 1/4 – 1/2″ (into 3/4″ stock) and yet it will still often be cutting forward but the x or y will skip and get off because they can’t take the amount of force to stay on course at that depth. And, as it goes deeper down you hear the spindle slowing down because of the added power needed to cut at that depth.

    The bit is pulling/drilling into the wood, the spindle is strong enough not to stall, if you have to high of a chip load it will pull itself into the material. unless you are using an upcut then it will jump out of the cut.

    My point is, I am not sure if it is the spindle that is slowing down first (like it hits a harder spot in the wood and slows down) which is causing the problem, or if it is the Z axis that is too weak and somehow it starts dropping, and as it digs down and cuts deeper that is why the spindle slows down? What I am getting at, is, do i need a stronger Spindle motor or a stronger Z axis motor? I currently have an 84 oz/in Nema 17 motor on the Z-axis. I see there is a low current (1.8 amp) Nema 23 that has ~340 oz/in torque. That would give me 4 times the Z axis strength and would help to keep the bit from digging downward. (Sometimes, however, the bit will pull out of the collet – so i am not really sure a weak Z axis is the problem.)

    No as explained above, just a much more appropriate chip load, you are pushing 4 times faster with a bit twice the diameter than anything I have ever done, so in my opinion you are asking at least 8x’s too much of it.

    My MPCNC is modified. That is, I have 2 pipes on both the X and Y axis, and have 2) 3/4″ plywood platforms on the Z-axis, which gives it a lot more strength – and my table is 3′ x 4′ (have middle feet on all 4 sides, so 8 feet all together – the unit is fairly solid.

    This also gives it a lot more moving mass which is bad, have you turned down the accelerations and Max speed in the firmware? Making this out of solid steel would not necessarily make it any better, is is a very balanced system.

    #37142
    Profile photo of Ryan
    Ryan
    Keymaster

    This is pushing it hard in softwood.

    #37213
    Profile photo of UnLtdSoul
    UnLtdSoul
    Participant

    Ryan
    Thanks so much for taking your time to respond.

    My problem is I am too impatient. But, I’ve taken your advice and took out my last 1/8 end mill i had.

    I tried it and it seems to be working well. I ran the profile and rough cuts at 1000 mm/m (16.7 mm/s) with a cutting depth of 3mm (.12″). (70% step over on the rough cuts). It cut smoothly with the hard maple. I didn’t try pushing it any faster or deeper – yet – I will later – but, i needed to complete this project for now. And, even though it is only clearing out such a small amount per pass, because i was able to go 3 mm DOC per pass, it did the rough out faster then the 1/4″ at 1.25mm DOC.

    So, taking your advice it looks like i may need to switch to 1/8″ end mills for this machine.

    Like I said, I use a manual speed controller on the DW660 – $15 from Harbor Freight. For this run I set it to 50% position. Pn this controller when you turn the dial all the way down, the motor still runs at probably 12-15,000 rpm. So, at the half way position I am sure the motor still runs around 20,000 rpm (I will have to measure it to see what it does run at). While cutting it probably drops to around 16,000, but, like i said, i will have to measure it to know for sure.

    Now I need to order some 1/8″ end mills. I will try a single flute and see how that works.

    When I first set this up I tried 1/8″ at first, but, i guess i saw so many others (with other machines) say they used 1/4″ for their rough cuts, I’ve been using them since.

    My next project is to try and add a 4th – lathe – axis to this. But, when i get around to it… Thanks for the advice.

    1 user thanked author for this post.
Viewing 4 posts - 1 through 4 (of 4 total)

You must be logged in to reply to this topic.