Ive recently noticed my gantry vibrating when cutting. It seems only to rattle/vibrate/chatter when cutting on the diagonal.
Im running a brand new .25" vee bit on alder at 9 FPM. I noticed this when cutting out an inlay piece. It was running its path and changed directions to a diagnal cut to the table and it started vibrating pretty good. I put pressure on top of the spindle with my hand and the vibration subsided.
Has anyone else had this issue? Is the gantry not beefy enough to handle a 9 FPM cut with a brand new, super sharp vee bit in relatively soft alder?!? This is very concerning to me and I hope that NWA has a solution. I tried calling their support line, but again was on hold until I was directed to a voicemail box. A voicemail box no one seems to check or return calls on...
Help me Obi Wan....
Chatter in the gantry
Moderators: al wolford, sbk, Bob, Kayvon
Re: Chatter in the gantry
Sudo:
Yes, chatter actually always happens. There's a tiny bit of chatter in every cut, simply from the force of the cutting edge making that initial contact with the material, which deflects the bit, z-axis carriage and gantry system. It's more pronounced in machines like ours that flex, but even the big monster machines show chatter marks.
For really bad chatter, there are typically two places to solve this.
The first, major one, is really more "judder", where the movement of the whole system seems to move in spasms. Horrible to watch! That one can usually be solved by cutting less deeply per pass. In some designs that are more "machining' than carving, you can sometimes control that effect by choosing which axes the bit is moving in (more on that below). In carving type designs, there's less opportunity for that control, other than maybe setting the angle of the cutting passes.
The second one, the one you're most likely experiencing, is good-old chatter. This is actually a resonant phenomenon of the whole motion and cutting system vibrating with the material. Depending on your spindle RPM, changing that up or down by just a few percent can move it out of resonance. If there are multiple passes being made, that initial chatter can actually force the system into even more chatter when the bit hits those even-harder-to-cut chatter bumps.
If I'm seeing bad chatter, and I know it's coming around for another pass, I'll sometimes kick up the RPM by a couple thousand RPM, to give it more power to cut through, and then I'll put my hand on the spindle motor to steady those vibrations. Typically doing that once will smooth the surface enough that a smaller change (~200 RPM) will do away with that chatter on the next pass, and it will slowly reduce to nothing. But, that might very well be due to the way those cuts were being run, not necessarily any great technique. I did notice that if I just gritted my teeth and let it go, in 3-4 more passes in the pocket, the chatter marks were gone.
And really, that's an important criteria to consider. If the amount of chatter is so much that it looks like it's damaging the machine with that flex, of if the cutting effects the final cut surface, then yes, it should be dealt with and removed. But, if the chatter just sounds horrible, and those chatter marks are going to be cut off in the next pass or two, then in most cases, I've just ignored it. I mean, do I really care if there are chatter marks on material that is going to be completely removed in just a minute or two? Nope, those can stay!
But, if those marks ARE affecting the surface finish, then my advice is to add an allowance of about 0.015-0.025 in wood, and 0.005-0.015 in metals, onto those roughing toolpaths. Then, come back through with a separate, high-RPM, VERY thin stepover finishing pass to remove that final amount. Because the stepover is so much smaller, you often want to use a longer depth of cut too, so there are fewer overall passes, and those will be using the same cutting edge. And, if you run that same finishing path twice, that will often leave very nice surfaces.
All that said, our Sharks have a special issue: their cartilage. Because each axis adds at least a little plastic into the chain of floppiness, HOW you cut can sometime be important. But first, let's establish our axes. I'm going to say X runs along the width of the gantry, across the T-slots. Y runs along the length of the T-slots. And of course, Z is vertical. When working at a single Z-axis height, the X and Y will have different characteristics depending on the movement. In the X axis, as it moves back and forth, the forces on the bit will cause the z-axis carriage, and thus the bit, to "rotate" around an axis in line with the Y axis, and will deflect in the XZ-axis plane. This is usually a reasonable amount of flex, and should be considered your "strong" axis. Because the Z-axis carriage sags downward, when the Y-axis is moving toward the router, the bit will tend to dive down into the material. In the opposite direction, when the Y-axis moves in the direction away from the router, it's pulls the bit, and that tends to make the z-axis carriage flex UP and out of the material. In the Z-axis, plunging and drilling when done "too" fast, will flex that carriage up, and you'll get an elongated hole where the initial cut is not on location in the Y axis, and depending on the material and RPM, it can even throw the bit a little in the X-axis direction.
On difficult cuts, like a full slot that goes deep into the material, pushing the bit along the Y, using a square-tipped end mill should be avoided, but pulling the bit is often fully successful, since the tendency isn't to dive deeper and deeper into the material. This can also be greatly helped by using "radiused" endmills, with those sharp tips precision-ground to some radius. (If you're haven't tried radiused endmills, y'all be cray cray!)
But, I digress. You're using a v-bit, so you won't likely see much diving, since the slope of the cut will tend to push the bit upwards. (Yay!).
I try to not push their site too much, but CNC Cookbook has a great series on machining; it's mostly for metals, but the same rules apply. Here's there article on chatter and how to avoid it: http://www.cnccookbook.com/CCCNCMillFee ... hatter.htm
Hope that helps, 'cause chatter SUX!
Regards,
Thom
Yes, chatter actually always happens. There's a tiny bit of chatter in every cut, simply from the force of the cutting edge making that initial contact with the material, which deflects the bit, z-axis carriage and gantry system. It's more pronounced in machines like ours that flex, but even the big monster machines show chatter marks.
For really bad chatter, there are typically two places to solve this.
The first, major one, is really more "judder", where the movement of the whole system seems to move in spasms. Horrible to watch! That one can usually be solved by cutting less deeply per pass. In some designs that are more "machining' than carving, you can sometimes control that effect by choosing which axes the bit is moving in (more on that below). In carving type designs, there's less opportunity for that control, other than maybe setting the angle of the cutting passes.
The second one, the one you're most likely experiencing, is good-old chatter. This is actually a resonant phenomenon of the whole motion and cutting system vibrating with the material. Depending on your spindle RPM, changing that up or down by just a few percent can move it out of resonance. If there are multiple passes being made, that initial chatter can actually force the system into even more chatter when the bit hits those even-harder-to-cut chatter bumps.
If I'm seeing bad chatter, and I know it's coming around for another pass, I'll sometimes kick up the RPM by a couple thousand RPM, to give it more power to cut through, and then I'll put my hand on the spindle motor to steady those vibrations. Typically doing that once will smooth the surface enough that a smaller change (~200 RPM) will do away with that chatter on the next pass, and it will slowly reduce to nothing. But, that might very well be due to the way those cuts were being run, not necessarily any great technique. I did notice that if I just gritted my teeth and let it go, in 3-4 more passes in the pocket, the chatter marks were gone.
And really, that's an important criteria to consider. If the amount of chatter is so much that it looks like it's damaging the machine with that flex, of if the cutting effects the final cut surface, then yes, it should be dealt with and removed. But, if the chatter just sounds horrible, and those chatter marks are going to be cut off in the next pass or two, then in most cases, I've just ignored it. I mean, do I really care if there are chatter marks on material that is going to be completely removed in just a minute or two? Nope, those can stay!
But, if those marks ARE affecting the surface finish, then my advice is to add an allowance of about 0.015-0.025 in wood, and 0.005-0.015 in metals, onto those roughing toolpaths. Then, come back through with a separate, high-RPM, VERY thin stepover finishing pass to remove that final amount. Because the stepover is so much smaller, you often want to use a longer depth of cut too, so there are fewer overall passes, and those will be using the same cutting edge. And, if you run that same finishing path twice, that will often leave very nice surfaces.
All that said, our Sharks have a special issue: their cartilage. Because each axis adds at least a little plastic into the chain of floppiness, HOW you cut can sometime be important. But first, let's establish our axes. I'm going to say X runs along the width of the gantry, across the T-slots. Y runs along the length of the T-slots. And of course, Z is vertical. When working at a single Z-axis height, the X and Y will have different characteristics depending on the movement. In the X axis, as it moves back and forth, the forces on the bit will cause the z-axis carriage, and thus the bit, to "rotate" around an axis in line with the Y axis, and will deflect in the XZ-axis plane. This is usually a reasonable amount of flex, and should be considered your "strong" axis. Because the Z-axis carriage sags downward, when the Y-axis is moving toward the router, the bit will tend to dive down into the material. In the opposite direction, when the Y-axis moves in the direction away from the router, it's pulls the bit, and that tends to make the z-axis carriage flex UP and out of the material. In the Z-axis, plunging and drilling when done "too" fast, will flex that carriage up, and you'll get an elongated hole where the initial cut is not on location in the Y axis, and depending on the material and RPM, it can even throw the bit a little in the X-axis direction.
On difficult cuts, like a full slot that goes deep into the material, pushing the bit along the Y, using a square-tipped end mill should be avoided, but pulling the bit is often fully successful, since the tendency isn't to dive deeper and deeper into the material. This can also be greatly helped by using "radiused" endmills, with those sharp tips precision-ground to some radius. (If you're haven't tried radiused endmills, y'all be cray cray!)
But, I digress. You're using a v-bit, so you won't likely see much diving, since the slope of the cut will tend to push the bit upwards. (Yay!).
I try to not push their site too much, but CNC Cookbook has a great series on machining; it's mostly for metals, but the same rules apply. Here's there article on chatter and how to avoid it: http://www.cnccookbook.com/CCCNCMillFee ... hatter.htm
Hope that helps, 'cause chatter SUX!
Regards,
Thom
Last edited by Rando on Tue Apr 25, 2017 3:05 pm, edited 1 time in total.
=====================================================
ThomR.com Creative tools and photographic art
A proud member of the Pacific Northwest CNC Club (now on Facebook)
ThomR.com Creative tools and photographic art
A proud member of the Pacific Northwest CNC Club (now on Facebook)
Re: Chatter in the gantry
Thom,
I really appreciate you taking the time to write all of this out. The resonance thing blew my mind. Ill definitely try everything you suggested.
I really appreciate you taking the time to write all of this out. The resonance thing blew my mind. Ill definitely try everything you suggested.
Re: Chatter in the gantry
Thanks for your kind words.
My philosophy has always been that any knowledge I possess is worthless unless shared freely to anyone who asks. That I make use of it for myself is incidental to why I learn. Of course, my bosses persuaded me (with $$$!) that I shouldn't just give away THEIR stuff
Darn them!
Regards,
Thom
My philosophy has always been that any knowledge I possess is worthless unless shared freely to anyone who asks. That I make use of it for myself is incidental to why I learn. Of course, my bosses persuaded me (with $$$!) that I shouldn't just give away THEIR stuff
Darn them!Regards,
Thom
=====================================================
ThomR.com Creative tools and photographic art
A proud member of the Pacific Northwest CNC Club (now on Facebook)
ThomR.com Creative tools and photographic art
A proud member of the Pacific Northwest CNC Club (now on Facebook)
Re: Chatter in the gantry
Sudo:
Sorry, sorry, just remembered one other very usefull technique for dealing with "real" chatter:
The chatter-inducing vibrational mode is a combination of the stock material, the bit, the RPMs and the feedrate (and depth of cut, stepover, etc.). You typically don't want to change the material, buying new (redundant!) bits is expensive, and validating new cutting parameters isn't always easy. So, to change the chatter characteristics, you can get the same effect by changing either the RPMs **OR** the feedrate. Or both, in truth.
But more importantly, what that means is that if you run the finishing pass at a significantly different FEEDRATE, you can actually run both the roughing and finish passes using the same bit, at the same spindle/router RPMs. Because the movement through the material will be significantly different, the likelihood of chatter in both is almost none, and the finishing pass might even help get rid of subtle chatter/deflection marks....with the added bonus that you can now run both roughing and finish toolpaths from a single GCODE/tap file
.
Regards,
Thom
Sorry, sorry, just remembered one other very usefull technique for dealing with "real" chatter:
The chatter-inducing vibrational mode is a combination of the stock material, the bit, the RPMs and the feedrate (and depth of cut, stepover, etc.). You typically don't want to change the material, buying new (redundant!) bits is expensive, and validating new cutting parameters isn't always easy. So, to change the chatter characteristics, you can get the same effect by changing either the RPMs **OR** the feedrate. Or both, in truth
. But more importantly, what that means is that if you run the finishing pass at a significantly different FEEDRATE, you can actually run both the roughing and finish passes using the same bit, at the same spindle/router RPMs. Because the movement through the material will be significantly different, the likelihood of chatter in both is almost none, and the finishing pass might even help get rid of subtle chatter/deflection marks....with the added bonus that you can now run both roughing and finish toolpaths from a single GCODE/tap file
.Regards,
Thom
=====================================================
ThomR.com Creative tools and photographic art
A proud member of the Pacific Northwest CNC Club (now on Facebook)
ThomR.com Creative tools and photographic art
A proud member of the Pacific Northwest CNC Club (now on Facebook)
Re: Chatter in the gantry
Can I ask, on average in wood cutting, what feed rate you use?
I use to think that I could push 20 or even 40 FPM and be safe. Now im finding that 7-10 FPM seem to work best (and even 10 is pushing it).
Obviously the slower the cut the better the result, but I just want to make sure Im on par with everyone else running the HD4.
Thanks again!
I use to think that I could push 20 or even 40 FPM and be safe. Now im finding that 7-10 FPM seem to work best (and even 10 is pushing it).
Obviously the slower the cut the better the result, but I just want to make sure Im on par with everyone else running the HD4.
Thanks again!
Re: Chatter in the gantry
I measure in IPM. In aluminum, for a 3/16" diameter bit, I'd use typically something like:sudo wrote:Can I ask, on average in wood cutting, what feed rate you use?
I use to think that I could push 20 or even 40 FPM and be safe. Now im finding that 7-10 FPM seem to work best (and even 10 is pushing it).
Obviously the slower the cut the better the result, but I just want to make sure Im on par with everyone else running the HD4.
Thanks again!
* full-slot with a 3/16 will be in the low 20's IPM.
* "normal" light-roughing cut will be in the 40s,
* High-speed machining toolpaths (stepover ~8%, Vectric does NOT produce these) in the low 60's,
* A finishing pass (stepover < 0.010" ) in 70+ IPM.
In the rare instances I do wood, I'd probably go another 50% higher, but not much more than that, because of that flex in the system, so that would yield:
* full slot in the mid-30's IPM
* light rough in the upper 50s
* HSM for wood is silly
* finishing passes in the 90+ IPM region
However, you have to remember that flex occurs during even unloaded acceleration, so I tend to stay relatively low speeds, not anywhere near the claimed 200 IPM. As far as I've seen, only rapids should be anywhere near that, and with a heavy spindle I lower the rapids to like 160 IPM. I've also lowered somewhat the acceleration maximum (Ctrl-G, 787) in the Z-axis because of that extra spindle weight. Better slow than lost steps!
What's funny is that I cut wood so infrequently, I don't even have a cut catalog for wood. I have one for aluminum, and another for HDPE and acrylic, but not for wood
. If a search in the forum doesn't turn up a cut catalog to take a peek at, let me know and I'll post it to this thread (also?).In all cases, my cut parameters are verified using the CNCCookbook's G-Wizard. 100%, no shortcuts. If the torque or HP are out of line, and the cut parameters don't fit in with what I've actually found to work, then the parameters are considered suspect. For machining projects with, say 30 toolpaths, I reserve a full day for validating and verifying cutting parameters, and examining lead-in/outs, ramps, all that. Homey don't like broken bits
.Of course, divide by 12 to get your FPMs.
Regards,
Thom
=====================================================
ThomR.com Creative tools and photographic art
A proud member of the Pacific Northwest CNC Club (now on Facebook)
ThomR.com Creative tools and photographic art
A proud member of the Pacific Northwest CNC Club (now on Facebook)