Why does the spindle bounce?

Anything and everything CNC-Shark-related

Moderators: ddw, sbk, al wolford

Why does the spindle bounce?

Postby ronhatchew@yahoo.com » Sat Dec 02, 2017 3:11 pm

For the most part it runs pretty smooth, but moving aft in the x axis I get a lot of spindle bounce which also causes bit marks. How can I fix this?
ronhatchew@yahoo.com
 
Posts: 1
Joined: Tue Nov 21, 2017 7:23 pm

Re: Why does the spindle bounce?

Postby sk8nmike » Mon Dec 04, 2017 8:05 am

Feed speed too fast, trying to take too deep of a cut, or bits would be my first checks.
sk8nmike
 
Posts: 377
Joined: Thu Dec 01, 2011 7:35 am
Location: Carrollton, Tx

Re: Why does the spindle bounce?

Postby Rando » Mon Dec 04, 2017 2:53 pm

ronhatchew@yahoo.com wrote:For the most part it runs pretty smooth, but moving aft in the x axis I get a lot of spindle bounce which also causes bit marks. How can I fix this?


Can you be a little more specific about the direction? sk8nmike's answer is definitely correct, and the easiest/best way to fix it sometimes depends on which way the system is trying to move. If I understand you, you're saying "toward the left in the direction along the width of the gantry, as viewed from the gantry side where the spindle is mounted." Is that correct?

Sneaky short answer: 8-) if you can feasibly add a finishing pass that is just slightly thicker than the gouge-marks, then you can often ignore the gouging. After all, if it's not damaging the machine, and it's overall removing material faster, and a required subsequent pass obliterates the evidence of it occurring, maybe it doesn't really matter.

Long answer: This is if you see it happening and you cringe in horror, and want it to stop, NOW! :twisted:

In essence, the shudder/judder/jumping is caused by having too much of the cutting edge(s) in contact with the material at once. I mean, at the root. This "engagement" has two parts: axial engagement, meaning how far along the length of the cutting edge, or depth of cut. The second part, radial engagement, is related to the stepover, but it's really more about the total bit circumference (360 degrees) that's in contact with the material at a time. A fine finishing cut might be in the 5-10% range, while cutting a full slot means 180-degrees of axial engagement. At any given RPM, the material hardness, combined with the bit sharpness and total engagement produces (in a well-understood and somewhat linear way) torque on the spindle, which is transmitted into the machine structure. Likewise, linear movement in the movement axes places deflection forces on the engaged portion of the bit. The deflection and torque generated at the cutting site are transmitted through the shank of the bit, through the chuck, into the spindle, and then through the Z axis carriage, the gantry, the bed slide rails, the bed frame, the bed t-slots, and work-holding mechanism, and finally the part.

The shaking you're seeing isn't actually because the speeds and feeds are "wrong". In fact, they're just wrong for this machine. If you think of the force-paths I outlined above like electrical circuits, the HDPE parts on our machines are like the light bulbs: energy transferred comes at a cost. Heat in the case of lightbulbs, and "elastic deformation" (and yes, even plastic creep) in the case of HDPE. In the analogy, the metal parts, so much better at transmitting force, would be the wires. So, it's not the electricity's (cutting force's) fault that the lightbulb (HDPE) heats up (flexes), it's just the nature of the the lightbulb (HDPE).

So, we can lower the heat (deflection) by either replacing the lightbulb (HDPE) parts, or by lowering the voltage (cutting forces) feeding the circuit. We'll never get the lightbulb (hdpe) to put off zero heat (deflection), but we can minimize it so it works for what we need it for.

And in our case, that means lowering the cutting forces, pure and simple. Below are some of the techniques I use, somewhat arranged in a "try this first" approach:

1) Verify the feeds and speeds: make sure the numbers are the right numbers for what you're cutting and with what, and that they're really what is put into the software. The idea here is that our machines--especially in wood--should be reasonably effective at "near-normal" speeds for the strength of machine we're working with. The HDPE really shouldn't cut more than ~20% off the normally-expected performance. That why, beyond believing they're right, I'm of the opinion to convince the system to do what it should, not reduce my expectations. But, that's just me ;-).

2) Lower feed rate before you lower spindle speed, but keep chipload in the proper range. If it's juddering, you want to give it more time to cut the material, but you don't want to change the surface-feet-per-minute (SFM) of how fast the cutting edge is slicing through the material. But, if you slow down the feed too much, the resulting chips will be dust, and you'll be rubbing the bit, not cutting the material. Rubbing leads to overheating, which leads to bit dulling and more overheating, and ruined bits and parts.

3) Add one or more finishing passes, sized appropriately. If you can't avoid gouging, then measure it and leave that much as a margin, then remove the gouges in one finishing pass, and then do the actual finished surface in a third pass. Timeconsuming, but it can be overall faster than having a large number of roughing-pass layers.

4) Use the shortest bit available. Not only are stubby bits stronger, but the reduced length lowers the mechanical-advantage of deflection forces in the spindle mount. Always use the shortest bit you can, but never chuck into the flutes.

5) Use radiused end mills. In situations where you're using a flat-ended end-mill (as opposed to a v-bit), those sharp tips very often are the culprit with catching and essentially drilling into the material. By adding a radius, those tips are not only much stronger (less breakage!), and the radius produces a slight upward force, sometimes completely eliminating diving on full-slot cuts. The fillet also makes the parts overall stronger and more resistant to stress fractures at sharp internal corners.

6) Lower "cutter stress spikes". That is, momentary increases in the bit engagement. Fast spikes in engagement lead to broken bits and unwanted deflection. You can hear and see those spikes when the bit is forced into a corner at speed. That momentary groan is the radial engagement going from 20-degrees to 100-plus degrees in an instant. More modern, High-Speed Machining (HSM) and Constrained Engagement toolpaths take this into account by never allowing that engagement to spike. I use them all the time in area-clearing pocket situations, as they really do produce a faster "Material Removal Rate", even on our machines.

Most of the things I produce aren't "artistic" and are more "parts". I do a lot of aluminum machining on the Shark, and there definitely are limitations to get around. A frequent difference between art and part is that a part often MUST be machined in a particular way. If the part requires a 1" deep slot 0.30" across and 4" long, well, there's only so many ways you can make that! Which means that sometimes I have to make specific limited choices to improve how a part gets made. And so, I tend to do these kinds of things when faced with juddering and similar, and I'm constrained to make the cut that way whether I like it or not:

* Side to side along the width of the gantry: I use a shorter depth-of-cut and reduce the speed if doing full-slotting. If it's doing it in a pocket (as opposed to a profile), if it's not severe, and a finishing pass will get rid of it, I often consider ignoring the juddering.

* Parallel to the t-track bed slots, in the direction where the gantry "pushes" the z-axis carriage in front of it: if possible, I avoid this, and instead "pull". If it really is required to go in that direction, slowing way down and using radiused endmills is the way to go.

* Parallel to the t-track bed slots, in the direction where the gantry "pulls" the z-axis carriage along behind it: this is the best direction for doing full-slots, since the bit tends to ride up out of the material, not plunge down into it. Adding the radiused endmills means that it almost never judders unless it's going way too fast. But, it also means you need to be careful with the slot depth, since riding out of the cut means it's not really as deep as programmed...leading you back to a finishing pass.

* Down into the material, in a drill operation: this has surprisingly more deflection than you 'd think, and can lead to out-of-round drilled holed in the part. If the hole is critical for either placement or roundness, you need to definitely do pecking, at no more than a couple mm per peck, and also dwell at the bottom for about 0.25s on each peck. Trust me, you'll see it flex and then settle back into the right place with each peck.

Alrighty then...I need to go make some parts ;-).

Hope that adds a whole heapin' helpin' of information to the discussion; deflection and its scary results are what I deal with always :D.

Regards,

Thom
Last edited by Rando on Mon Dec 04, 2017 8:00 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)
Rando
 
Posts: 462
Joined: Tue Jan 06, 2015 3:24 pm
Location: Hoquiam, WA

Re: Why does the spindle bounce?

Postby Kayvon » Mon Dec 04, 2017 6:33 pm

Rando wrote:Can you be a little more specific about the direction? Kayvon's answer is definitely correct
Wasn't me this time :)
User avatar
Kayvon
 
Posts: 271
Joined: Tue Oct 21, 2014 11:46 pm

Re: Why does the spindle bounce?

Postby Rando » Mon Dec 04, 2017 7:59 pm

Kayvon wrote:
Rando wrote:Can you be a little more specific about the direction? Kayvon's answer is definitely correct
Wasn't me this time :)


Oh weird...I thought all correct answers at some point came through you :D.
Cheers, Sir!
=====================================================
ThomR.com Creative tools and photographic art
A proud member of the Pacific Northwest CNC Club (now on Facebook)
Rando
 
Posts: 462
Joined: Tue Jan 06, 2015 3:24 pm
Location: Hoquiam, WA


Return to CNC Shark

Who is online

Users browsing this forum: No registered users and 4 guests

cron