|
Post by vf2255 on Feb 21, 2021 13:42:51 GMT -5
Using an Amana 46700-K (1/4" compression bit) for 1/2" Baltic Birch.
1st pass is just enough to get the up-cut portion of the bit below the surface (0.3125").
I have adjusted IPM and RPM rates.
Bit is set in collet at the "K" mark.
Followed recommended chip loads, etc.
The machine screams so loud even with double hearing protection it's unbearable. I have no idea what is causing this. Patience is running thin.
Loose screws could be the problem as I have found a few loose screws on the machine, one of which caused a serious issue with the Z-axis (nightmare to get back in). Axiom, it's called lock-tite, get some!
Any recommendations on which screws I should check to see if this is the issue?
This machine is useless in it's current state. I need help.
|
|
johnb
Full Member
New owner @ March 2019, AR16 Elite, Aspire, 4th Axis & Laser
Posts: 326
|
Post by johnb on Feb 21, 2021 15:38:02 GMT -5
What machine? What Controller? How are you "adjusting" feeds and speeds? If your first pass is .3125" into a 1/2" board with a 1/4" bit, you're taking a pretty big bite there. Try dialing it back to a third of that and see what happens
|
|
johnb
Full Member
New owner @ March 2019, AR16 Elite, Aspire, 4th Axis & Laser
Posts: 326
|
Post by johnb on Feb 21, 2021 15:47:05 GMT -5
Also, generally speaking, you "feed" a screaming bit (faster IPM) and slow down the RPM. Try it at 13,000 rpm (Assuming here that your bit isn't dull).
|
|
|
Post by vf2255 on Feb 21, 2021 16:31:09 GMT -5
Machine: Iconic 8.
I need the compression bit's first pass to be enough to get the up-cut bits end all the way into the material (0.3125"). 1/4" bit can do x1-x2 time its diameter in cut depth per pass.
Pushed to 150 ipm, didn't help.
I seated the bit as far as I can into the collet, seems to have helped some.
|
|
|
Post by aluomala on Feb 23, 2021 21:20:18 GMT -5
Machine: Iconic 8. I need the compression bit's first pass to be enough to get the up-cut bits end all the way into the material (0.3125"). 1/4" bit can do x1-x2 time its diameter in cut depth per pass. Pushed to 150 ipm, didn't help. I seated the bit as far as I can into the collet, seems to have helped some. I'm wondering why you call the machine "useless". You bought an entry level machine, and are expecting it to do something that the higher end machines can't do. Where did you get the idea that you can cut x1-x2 times its diameter for depth of cut? Most people use half of the diameter as a starting point. The only thing I agree with you in your assessments of the Axiom product line is the questionable quality control and their refusal to use Loctite to secure nuts/bolts. When I unboxed my AR4, there was a random bolt in the bottom of the shipping crate. I (eventually) discovered that is was supposed to be securing the cable harness under the machine, and it almost got ripped off by the y-axis mechanisms. Plus the "puck" wiring inside the gantry had a loose bolt, causing intermittent connections, and I destroyed 3 bits in one (frustrating) day. Lots of the fan-boys defend the company, insisting it's absolutely normal to check every. Single. Bolt. And. Connector. before you first use it. Because things come loose in transport. Yeah, I don't think I should have to check to make sure that the factory and QC people in the warehouse did their jobs, but apparently that's to be expected with a Axiom product. Plus the rotary axis is pretty much junk out of the box. Mine had too-short of bolts to mount to the standard Axiom table, too short of fittings for the electrical connector coming out of the rotary (so it's perpetually loose). And the factory settings were useless for the stepper motor (easily lost steps due to slipping, until I emailed customer support, and they told me how to adjust them so its, you know, functional. Plus the chuck is pure garbage, so you have to buy a new one. I don't really understand why you need to go .3125" on your first pass. Create a toolpath that has a separate last pass so there isn't damage done to the top of the material. Overall it seems like you don't have a solid understanding of the capabilities and limitations of your machine, or the toolpaths. You're expecting an entry level machine to perform like a production machine that costs at least 5 times as much (or more).
|
|
|
Post by vf2255 on Feb 23, 2021 21:26:44 GMT -5
Thank you for your input. Any idea on how to eliminate the "screaming" from the bits? (shallower passes don't seem to help).
|
|
|
Screaming
Feb 23, 2021 22:46:08 GMT -5
via mobile
Post by mnwoodbee on Feb 23, 2021 22:46:08 GMT -5
Bits should suit your application in a number of areas. I understand your compression depth, I use them all the time. Manufacturers recommended settings can’t always be applied to all machines. If your using a bit that has a 1 1/2” flute length to cut through 1/2” material you will get bit deflection/ chatter/ noise etc. You kinda see that in your choking up in collet test. Always use the shortest bit for the job.
That’s what it sounds like to me. Sound is a good indicator of correct parameters.
|
|
|
Post by joeblow on Feb 24, 2021 17:25:14 GMT -5
Hi VF. I personally would go the opposite direction and slow everything way down and be more conservative with your depth of cut. I would start with 80ipm, 12000rpm and .125doc. Use that as a starting point and adjust from there. So much is playing into the screaming....hold down method, deflection from using a 1/4" bit and very aggressive depth of cut and speeds. Keep in mind that the bit is actually cutting both sides of the toolpath at the same time also. Conventional and climb cut happening at once. Aluomala is correct in that you should really look into the last pass feature in Vectric's profile toolpath if that is the software you are using. Leave .05" or similar for the last pass to remove and the compression bit will do a great job. Also, I wouldn't look at any chipload charts. Get to know your machine, the material you cut, inspect the chips on every job, feel your bit the moment the toolpath is done running. Basically crawl, walk, run.
Good luck and I hope this helps.
|
|
loren
New Member
Posts: 68
|
Post by loren on Feb 26, 2021 7:53:07 GMT -5
I have a particular 1/4 inch straight bit that's about twice as loud as others. I don't know if it's the grind, or if it's imperceptibly bent or what, but it's awful.
In all other cases, I've been able to quiet things down through speeds and feeds.
|
|
vf
New Member
Posts: 1
|
Post by vf on Feb 26, 2021 14:41:16 GMT -5
joeblow, loren, thank you both. I dialed everything down (70ipm/12024rpm), changed to a down-cut bit (instead of the compression). Seems to have eliminated the "screaming". I was really on my last nerve. Chip load charts and recommendations seem to be way off. 0.0029" would be my "calculated" chip load based on 70ipm/12024rpm for a two(2) flute bit. Amana's specs states the chip load should be 0.005 per tooth for the Amana 46415-K bit I'm using (it is a two(2) flute bit). Thank you both for your insight and comments.
|
|
|
Post by joeblow on Feb 27, 2021 6:06:58 GMT -5
Glad to hear you got it dialed in better.
|
|
|
Screaming
Sept 11, 2021 11:27:40 GMT -5
via mobile
Post by kokopelli2020 on Sept 11, 2021 11:27:40 GMT -5
Thank you for your input. Any idea on how to eliminate the "screaming" from the bits? (shallower passes don't seem to help). Because we have 1/4” dia bits, resonance is our enemy and the harder and oily the wood, as well as duller the bits, we end up with a gang of street cats at night brawling it out. Partly from the thinner metals used on the gantry, lots of aluminum which seems to amplify resonance, we need to approach the problem with more steps. Start your cut path with downcut bits past your up cut depth required. Switch out to upcut or compression to complete the cut. Spend more time experimenting with feed and speed rates using the vfr, the up-down Y button on controller and also the decibel app on your phone. Record your findings as they can help set you up faster down the road.
|
|
|
Post by dadealeus on Oct 9, 2021 1:01:22 GMT -5
Thank you for your input. Any idea on how to eliminate the "screaming" from the bits? (shallower passes don't seem to help).
EDIT: I just checked the model of the compression endmill you were using and it was, indeed, a 2-flute - which is odd that's it's screaming like that. I'm assuming you tried the feeds and speeds they specifically recommend (https://www.amanatool.com/pub/media/productattachments/Solid-Carbide-Spektra-Compression-Spirals-for-Baltic-Plywood.pdf). It's possible that the deflection was causing the noise considering the cutting height alone is 1.25" on that endmill.
---
A bit late to this one, but I figured I'd reply. A "screaming" endmill, in my experience, is due to the endmill rubbing the material instead of taking bites out of it. As others have stated, you generally need to try to push the endmill through the material faster (increasing feed speed), while decreasing RPMs (so each blade is able to take a larger bite).
However, more than likely, the first endmill you were using (the compression bit) was a 4-flute endmill. I started with these, too, and had the same issue. In wood, 4 flutes are simply too many blades for a "squishy" (non-metallic) stock. As the blades spin, there's not enough room between them to get a good bite of the material, so regardless of how fast you push it, it's going to end up rubbing and generating a loud whine (and a lot of heat).
Basically, for any clearing operation in wood, you should be using a 2-flute endmill - which is why the 2-flute downcut you're using eliminated the whining. The reduction in the number of blades allows larger bites of the material, letting the blades work as knives instead of sandpaper.
Anyway, it took me a while to figure this out, but I have a large stock of 2-flutes that I now use for all my clearing operations. If you're interested in reducing tearout without generating a lot of heat (a downcut is going to force all those chips back under the endmill - cutting them multiple times, which generates heat and dulls your endmills more quickly. I used to use a downcut endmill to go no deeper than the diameter of the tool, then I switch to an upcut. That eliminates tearout and gives you a clean surface finish, but you have to change out endmills.
As a good medium, try a simple, 2-flute, straight-cut endmill. You'll have nice, clean edges with no tearout on both the top and bottom of your cuts. Straight endmills will dull more quickly than an upcut or downcut, but you can still get plenty of life out of them before they no longer cut cleanly.
I keep a few of these on-hand and they perform the vast majority of my clearing and cutting operations:
www.amazon.com/gp/product/B000K2EAIG/ref=ppx_yo_dt_b_search_asin_title?ie=UTF8&psc=1Finally, if you're interested in a great tool that helps you with feeds and speeds, I recommend checking out GWizard. It's been a godsend for me. There's a free trial to give it a test run (they give you a free week or month or something - I can't remember. I just know I bought the full version after my first few cuts using its numbers).
Hope that helps!
|
|
Rob
New Member
Posts: 15
|
Post by Rob on Oct 31, 2021 19:50:44 GMT -5
I am new to this as well but from what I can see, this consumer industry is too new with lots of bad information. Amana Tools publishes speed and feed but they are different for every machine. This will take a decade to figure out. I spent 6k on a CNC machine and I feel no one can truly answer my questions. It's pretty sad after watching all of the amazing videos of people making money. Sponsorship seems to work!
|
|
|
Post by dadealeus on Oct 31, 2021 20:09:33 GMT -5
I am new to this as well but from what I can see, this consumer industry is too new with lots of bad information. Amana Tools publishes speed and feed but they are different for every machine. This will take a decade to figure out. I spent 6k on a CNC machine and I feel no one can truly answer my questions. It's pretty sad after watching all of the amazing videos of people making money. Sponsorship seems to work!
It's easy to be down on your own abilities when you see the carefully crafted videos that people release that show nothing but their successes. Social media is a cancer because it makes people believe they have to be perfect in order to not be a loser.
In short, it makes people afraid of failure.
However, what anyone with real success will tell you is that failure is a part of success. No one just hops on a bicycle for the first time and successfully rides it; they fall repeatedly until they finally succeed.
Picking up a new skill like CNC machining is no different. You're going to fail a lot more than you're going to succeed at first, but important to keep your head up and keep trying.
The feeds and speeds, for example, are not really that different per machine as they are per the material they are cutting. Wood, for example, can get a single recommendation, but there are hundreds of different varieties of woods, knots, grain considerations, etc. to consider, so you have to adjust it for each cut - a skill that you develop over time.
A software like Gwizard is great to get some initial feeds and speeds, but I always start on the conservative side of those suggestions and then move up from there.
Just know that you're going to break a few end mills and ruin a few pieces along the way, but you need to just practice like any other skill. Pick up trash pieces of wood off the side of the road and run different feeds and speeds through them (after checking for nails, etc.) or try working on some cheap foam insulation boards.
Just know that for a specialized skill like this, no one is just going to be amazing out of the gate. Everyone works to get where they are and this is no exception.
|
|
|
Post by gerry on Oct 31, 2021 20:09:42 GMT -5
I am new to this as well but from what I can see, this consumer industry is too new with lots of bad information. Amana Tools publishes speed and feed but they are different for every machine. This will take a decade to figure out. I spent 6k on a CNC machine and I feel no one can truly answer my questions. It's pretty sad after watching all of the amazing videos of people making money. Sponsorship seems to work! This consumer industry is not that new. The junk information comes from listening to folks with toy CNC machines. They make a lot of videos with a lot of incorrect information. The feeds and speeds are not a fixed quantity, but they do mostly reflect commercial machines. There's a vast difference between driving a 1/2" mill with a 1" DOC @ 300IPS and a 1/4" mill with a 0.1 DOC @ 60IPS. Testing is a requirement, but folks want a canned answer NOW.
|
|
|
Post by aluomala on Nov 4, 2021 20:07:52 GMT -5
I am new to this as well but from what I can see, this consumer industry is too new with lots of bad information. Amana Tools publishes speed and feed but they are different for every machine. This will take a decade to figure out. I spent 6k on a CNC machine and I feel no one can truly answer my questions. It's pretty sad after watching all of the amazing videos of people making money. Sponsorship seems to work! My recommendation to you: sell your machine and buy a Cricut machine. Buy only Cricut branded materials, and do exactly what they tell you to do with that material. It works for legions of "crafters" and might be right up your alley. Amana sells products primarily intended for commercial application, not hobbyists. Expecting them to hold your hand while you learn the ropes is illogical (and somewhat moronic). Their tools are designed to cut pretty much EVERYTHING, from acrylics to ferrous materials, and everything in between. Plus, there are literally millions of permutations of the various CNC machines, with the low end ones using a Dremel tool (my first CNC (ShapeOko2) came with a knockoff Dremel), to handheld routers, to water cooled spindles that can cut through 2" oak in a single pass (that might be an exaggeration, but I doubt it, based on some of the industrial machines I've watched videos of). If you expected to hit the ground running, cutting whatever your heart desires by looking at some chart (feeds and speeds) without having to do some amount of research, experimentation, frustration, etc, you definitely got into the wrong hobby/business. When I break a bit, it's almost always my fault, or very rarely, an issue with the machine (very common with low-end CNCs with crappy wiring, and connected directly to a PC). I don't blame Amana for my ineptitude, since only a poor carpenter blames his tools, right?!
|
|
|
Post by Gary Campbell on Nov 5, 2021 9:49:56 GMT -5
I am new to this as well but from what I can see, this consumer industry is too new with lots of bad information. Amana Tools publishes speed and feed but they are different for every machine. This will take a decade to figure out. I spent 6k on a CNC machine and I feel no one can truly answer my questions. It's pretty sad after watching all of the amazing videos of people making money. Sponsorship seems to work! I don think there is so much "bad" information as there is "different" information. The tool MFGR's publish OPTIMAL feeds and speeds for their bits. Assume this means that if you have a machine with thousands of pounds of steel in its frame and 20 horsepower, this would be the highest chipload you could run. And even if you do, your hold down and material may dictate a lesser chipload. It shouldn't take a decade, but yes, you must take time to figure out what feeds and speeds work on your machine. Those before you have done it, because learning is the most important (and frustrating) part of the CNC journey. Lets say you dropped $6k on a guitar, boat or set of golf clubs. Would you also expect instantaneous spectacular results from those hobbies? Even woodworkers that use only hand tools take years to refine their craft, hopefully you will have a portion of that to refine your new one.
|
|