Trouble with acrylic


(Dylan) #1

Hey guys, I’ve been having really unpredictable results with acrylic. Sometimes it will go for hours with no problem. Sometimes it gets caught in the material and can pull the spindle out of alignment, cutting chunks out of the part and making some really uniquely horrible noises as it does.

I’ve been using the parameters listed in the Nomad Feeds/Speeds chart:

DOC: 0.019"
RPM: 9000
FEED: 44
PLUNGE: 14

Is anyone working with acrylic and getting good/consistent results? I’m not sure what parameters to play with here. I’ve been working with 1/2" cast acrylic and it often doesn’t get caught till several hours into the job which is frustrating. I appreciate any recommendations you all might have.


(Dylan) #2

Oh, and I’m using the 1/8" ball mill that came with the nomad for the clearing. The flat end mills i’ve tried really struggle with acrylic.


(James Carter) #3

Acrylic is very temperature sensitive… and has a low melting point. I recommend starting by reducing your RPM and feed rate until you generate “chips” instead of dust or smeared half-melted blobs. I would go half on the RPM right away though.


(Dylan) #4

Thanks for the tip! Temperature doesn’t seem to be much of a problem. I’m getting good, consistent chips and not any melting or powder. It seems like the bit just gets stuck occasionally and the spindle doesn’t have enough power to pull through. I can hear the spindle slow down a little each time it plunges and that seems to be where it’s most susceptible to catching the material.


(William Adams) #5

In that case, please check the belt tension of your spindle motor —

When pushing in the center of the pillows, about 2–4mm deflection is normal for the belt.

Don’t overtighten, since that will lead to a loss of torque from friction. If that doesn’t help, contact support@carbide3d.com and we’ll do further diagnoses.


(Temujin Kuechle) #6

Also, consider creating toolpaths that are offset from your part and make that first cut very shallow. Then start the next cut a little closer, leaving the final cuts equally shallow but closer to your part. This gradual approach seems to work well for a friend of mine. The edge finish seems to come out more precise/crisper, if that is what you are wanting as an end result and it doesn’t melt. Definitely reduce RPMs.


(Dylan) #7

Thanks for the tips guys!

I adjusted the belt just slightly to see if it would make a difference. I haven’t noticed much of a change other than the noise from the spindle is a bit higher pitch.

I have also been playing around with ‘Climb’ vs ‘Conventional’ toolpaths and have found that conventional seems to be easier for the machine but leaves a rougher surface finish. Climb is a much cleaner finish but it gets caught in the plastic more often.

That sounds like an interesting approach. I’m using MeshCam for my toolpaths so I don’t have a ton of control without altering the Gcode which I’m not familiar with. But I suppose I could build out geometry offset from the part with a tapered edge so that it forces this sort of clearing.


(William Adams) #8

For climb vs. conventional, my suggestion would be to use conventional for roughing, then climb for a finishing pass — pair that w/ @Tem’s brilliant technique and hopefully you’ll get a reliable process (please document how you go about it).


(James Carter) #9

I found a “multiple tool path” solution works best with meshcam. I create a new tool path for each tool I use… The repeatability is 100% if you don’t take the part out of the machine :slight_smile:

I also took the precaution of installing hard stops on my vises, so once I set my X and Y zeroes, I rarely have to mess with them again.

EDIT: You can choose the direction of the cut… just use “climb” for the finish pass!


#10

Just looked at my last job in acrylic (essentially a repeat of the clamps I posted in Calling All Makers: Carbide Community Build Competition #6 starts now! ), and your numbers seem about right for a 1/8" tool for slotting. (90m/min surface speed, 1100mm/min travel, 375mm/min plunge)

That said, I ran a ramped entry for the plunge on contours (slot cutting parts from sheet), and left 0.1mm (radial) for finish cut so the finish would be done in a single pass with space for the chips to clear.

The last job with a lot of clearing (a LOT of clearing for the part size, pockets and edge. About 50cm^3/part removed on stock that started at about 120cm^3 at 10mm thick) ran about a dozen times without an issue. This was done at same speeds, but 40% tool engagement (1.25mm radial depth), climb, and axial depth of cut/stepdowns 1.5mm. I used a helical entry for the pockets. The strategy was trochoidal (Fusion/Inventor’s “adaptive clearing”). Vacuum chip removal.

I would really, really suggest using a square end tool for everything but a finish contour. A SHARP one. Heat and chip buildup are your enemy, and dull tools rub. Ball end tools can rub near the center and have issues with chip removal and the low surface speed near the center.

For heavy clearing or finish, I would suggest ALWAYS climb with acrylic. The cutting edge gets in to the material without rubbing. Conventional, especially on a light cut, tends to rub, heating the material and dulling the tool. There are sources that will say the result is cleaner with conventional, and it can be since, if the chips stick, they get swept by the next cutting edge. On the other hand, climbing gives a better finish surface, in general, and if set up properly with a sharp tool, the chips won’t stick. A light, but substantial, finish cut (5% to 10% radial engagement is where I tend to go) leaves a fine finish.