PDA

View Full Version : Acrylic Cutting Help



Tenson
21-12-2012, 04:50 PM
Hi,

I'm trying to cut some parts from 5mm black acrylic and what I'm finding is that cutting on the short axis I get a decently smooth cut, but along the long axis I get a kind of streak of roughness, but it is not across the whole cut depth. Can anybody suggest what is causing this? I did cut in multipul passes and then did a finish pass a well. I'm using a 3.17mm cutter and went at half the speed GWizard suggested, halving both the mm/min and the spindle RPM.

The rough part is slightly inset from the rest of the cut, not proud, is that means anything. Also the rough part is at the top of the cut so it seems like things improve as the cuts go deeper.

Here are a couple of photos.

http://i608.photobucket.com/albums/tt169/tenson_uk/Acrylic-Cut1.jpg
http://i608.photobucket.com/albums/tt169/tenson_uk/Acrylic-Cut2.jpg

Tenson
21-12-2012, 05:06 PM
Ahh, I just looked at the sheet I cut the part from and it seems to have a better finish on it. I used conventional milling as GWizzard suggested but it looks like climb is better?

I'd still like to know why it is okay on the other axis though and what causes it to look bad just on one of the passes.

martin54
21-12-2012, 05:50 PM
I was going to suggest climb milling, not sure what the reasons are but on the signmaking forum I use when the question comes up people always say you get a better finish with acrylic using climb rather than conventional milling.

wilfy
21-12-2012, 06:12 PM
isnt slowing the spindle speed down a bad thing for acrylic? i'll be honest though that looks like crap on the bit, it's not melting the protective sheet to the router bit or anything daft like that is it?

Tenson
21-12-2012, 07:24 PM
Slowing the spindle down shouldn't be an issue if I keep the feedrate proportional, right? The chipload is the important thing I think. Still, maybe it will cut smoother if it is faster, I should try.

I might also simply need to try another cutting bit, perhaps this one is slightly damaged.

Lee Roberts
21-12-2012, 11:00 PM
Slowing the spindle down shouldn't be an issue if I keep the feedrate proportional, right?

I think that's right but dont see it would help for this, i could be wrong.


The chipload is the important thing I think.

Yea its a good indication that things are working well, i.e you want chips not dust, chips not spirals, though this is probably different for different materials.


I might also simply need to try another cutting bit, perhaps this one is slightly damaged.

Are you only getting this in soft stuff "plastics" or what, it could be the deflection/accuracy thing seen in climb vs conventional.

.Me

AdCNC
21-12-2012, 11:17 PM
If your chip evacuation is not sufficient then this is normally the cause of this. Do you use a decent vacuum to remove the chips as they are being cut? What tends to happen is if you start to recut the same chips they become hot and rub and "smear" around the cutter and are deposited on to the material edge and result in what you see in your picture!.. thats what ive come across in the past.

Failing that use some wet+dry like 1200 grit to clean the edge then give it a lick with a blowtorch preferably using MAP Gas as this burns hotter and has less oxygen content so less contamination of the plastics edge.

Tenson
22-12-2012, 12:28 AM
I do have a vacuum but maybe it's not working well enough in that direction of cut. I'll have a closer look tomorrow and also try another bit.

This needs much more than 1200grit, even with 150grit it takes a bit of work to remove the recess where the rough part is!

How much of a finishing pass do you chaps recommend for acrylic? I was using 0.3mm but maybe if I used more, it would sort it out?

Jonathan
22-12-2012, 12:57 AM
From the images in the first post it looks like the machine slightly lost position after a few passes, then continued as normal. Tricky to explain, but what I think happened is at the depth of the poor finish the machine lost position and moved further away from this cut, but not by much, such that on the subsequent passes the cutter didn't quite touch the first bit that was cut, but did stick hot swarf to it, hence the poorer finish. Meanwhile the cutter would have cut more from the waste piece, over the full height - hence the better finish on that part. I've seen this happen on my machine when a part hasn't been clamped well, so it moves ever so slightly giving the same effect. Could be the same here...



Slowing the spindle down shouldn't be an issue if I keep the feedrate proportional, right? The chipload is the important thing I think.

Spot on...

Precisely what feedrate, spindle speed and depth of cut were you using?

Tenson
22-12-2012, 01:15 AM
Hi Jonathan,

I had it pretty well clamped I think. Please remember the roughness doesn't seems recessed from the rest of the cut, so possibly not just re-cut chips embedded in it?

I was using:

700mm/min
11,000RPM
2 flute 3.17mm cutter
1mm multiple passes
0.3mm finishing pass

I'm not sure how it would have lost position at such a low feedrate. I guess I might need to check the rotating ballnuts to make sure the cogs aren't working loose.

By the way I got my vacuum extraction working just the other day.


http://youtu.be/rT-Hfd-k3Zw

m.marino
22-12-2012, 05:32 PM
Increase feed rate a bit. With that type of pass in acrylic you want to be getting chips that are quasi snowflakes to proper chip form. Dust is a sign that you are cutting to slow and you will deal with melt and it will cause problems. Next is this cast or extruded acrylic (easiest way to tell that I know of is almost all extruded has a translucent protective covering and cast is white) When I am surfacing 1212 I am going between .75 to 1.5 mm deep with a 3 flue TCT MG end mill and running it at about 14K and 2.3 m/min and getting rather nice finish. Acrylic is a problem child in that it will melt easily IF F & S is to slow (even cast will start too but requires really slow).

Cutting plastics requires testing and learning what works, due to large number of variables that are out there. Type of plastic, type of end mill, S & F's; these all play a part then add how rigid is the machine and things get interesting.

Michael

PS From everything I have seen I agree with ADCNC that is redeposit of plastic on passes after the original cut due to too slow of feed rate.

Tenson
22-12-2012, 05:56 PM
I don't think it is just the feed and speed, since the X axis direction is fine at the same speeds. I suppose increasing feedrate might reduce the need for better extraction though? If I push feedrate too high without increasing RPM of course the bit will deflect or break, it is only 3mm dia.

I can probably improve dust extraction (for one, I emptied my vacuum!). I'll have a play and let you guys know how I get on.

Tenson
23-12-2012, 07:56 PM
Okay well I actually found that my entire Z axis was loose from the X axis. Strangely though I'd have expected that to make the X axis cut poor but that one was great, lol. Still it couldn't have helped matters. I've also made a modification to improve dust extraction. I haven't tried another cut yet, I'll do that tomorrow.

I'm also considering getting a more suitable tool for cutting plastics. Looking at the Cutwell Tools site.. what do you think is better for acrylic they have 45deg Helix flutes (do these extract the chips better?) plus some YG single flute HSSE and some Karnasch cutters. Are the Karnasch worth the extra money?

JAZZCNC
23-12-2012, 08:18 PM
Are the Karnasch worth the extra money?

Never used any to cut plastics but have in Ali and they are excellent cutters. Best finish I've had from any brand cutter so far.

AdCNC
23-12-2012, 08:20 PM
If your looking at cut-wells range have a look at the YG1's Alu-power, summat like a 6mm 2flute should give you good results but with these you need to keep the RPM down or the feed up when cutting plastics. The bests cutters I've used so far are OSG and M.A. Fords for Aluminium and plastic but that all depends on your budget and how sturdy your machine is.

Tenson
23-12-2012, 11:19 PM
Unfortunately I need to use a 3mm bit for this work.

Do you think the Alu-Power are better for plastics than the HSSE ones? Cutell seem to suggest the HSSE are better for plastics.

AdCNC
23-12-2012, 11:24 PM
Ive never used the hsse cutters but i dont see why not! Give one ago.

JAZZCNC
24-12-2012, 11:13 AM
Unfortunately I need to use a 3mm bit for this work.

Do you think the Alu-Power are better for plastics than the HSSE ones? Cutell seem to suggest the HSSE are better for plastics.

Most of the Alu-power are HSSE cutters and the single flute certainly are. That said other than the Karnasch I think HSSE give a better finish in Ali than carbide does.! They just wear quick.

m.marino
28-12-2012, 12:55 PM
That can also be a byproduct of feeding to slow as you get melt and fusing at the top of the piece being cut. Just something that came to mind as I was cutting and cleaning up a new jig for the machine. When doing finishing surface profile with a 6 mm 2 flue I am normally running at 2.25 m/min or slightly faster (up to 3m/min on really thin finish passes) and that leaves a very nice smooth finish that polishes easily if needed.

Michael

Tenson
28-12-2012, 04:08 PM
Any comment on the 45deg helix cutters? Is assume this is done to get better chip evacuation? Worth a go?

Tenson
28-12-2012, 05:23 PM
Okay I have had another play.

I secured my Z axis properly to the X axis(!) and also made a kind of extender tube to get the vacuum suction closer to the work piece. I then tried a cut, but this time I reduced the spindle speed. I used GWizard to receommend a feed and speed and I noticed that actually it was giving me a smaller chipload than recomended. I suppose it was trying to keep tool deflection as low as possible but I found I could reduce the spindle RPM and still keep deflection below the problem area. GWizard sugested (for a 2flute 3.17mm bit) 1mm passes with 2000mm/min and 22,000RPM. I reduced this to 17,000RPM and kept the rest the same.

The cut is clean, but does have a slight texture, is this about as good as you guys are getting or should I still aim for higher?

http://i608.photobucket.com/albums/tt169/tenson_uk/DSCF8649.jpg

http://i608.photobucket.com/albums/tt169/tenson_uk/DSCF8647.jpg

http://i608.photobucket.com/albums/tt169/tenson_uk/DSCF8648.jpg

Tom J
03-11-2016, 05:22 PM
Just broke last carbide single flute 1/8" 3.175mm bit doing 700mm/min at 10.000 rpm, 600mm/min was ok but still poor finish.

Rye
03-11-2016, 07:26 PM
I usually cut acrylic with 1 mm passes using a 3.175mm single-flute @ 1050 mm/min - somewhere between 10000-13000 rpm (i think). Will be cutting some tomorrow. Will post RPM here.

Tom J
04-11-2016, 12:06 AM
I usually cut acrylic with 1 mm passes using a 3.175mm single-flute @ 1050 mm/min - somewhere between 10000-13000 rpm (i think). Will be cutting some tomorrow. Will post RPM here.

I follow 50%+ rule of DOC which was 2mm in for 1/8" will try less. Going to buy decent Trend bit 1/4" 6.35mm

magicniner
04-11-2016, 10:17 AM
Several mentions of "Climb V Conventional" in this thread.
If you are cutting a slot when profile cutting a part there is no climb and conventional, the cut direction only affects the deflection direction toward or away from the part, the cutter is cutting both climb and conventional in alternate halves of it's rotation.
Climb V Conventional only comes in when the cutter is engaging less than 100% of it's width in material,

- Nick

Rye
06-11-2016, 01:32 AM
I follow 50%+ rule of DOC which was 2mm in for 1/8" will try less. Going to buy decent Trend bit 1/4" 6.35mm

Cut some 4mm acrylic today using a 4mm shank/3 mm dia cut single-flute shop-apt bit. Did two passes @ just under 2mm on each with a finish pass. Feed rate 1200 mm/min with spindle speed around 13200 rpm (220 hz). Cut fine leaving a nice finish (just a couple of tool marks on one side.) Not saying that's the correct or optimal speed, but it worked for me. Usually I stick to smaller passes because I have a habit of not properly sticking/securing the acrylic to the spoil; and there's nothing worse than spending ages engraving acrylic just to have it lift from the table when cutting :)

Dean jeffery
08-11-2016, 08:15 PM
I'm also considering getting a more suitable tool for cutting plastics. Looking at the Cutwell Tools site.. what do you think is better for acrylic they have 45deg Helix flutes (do these extract the chips better?) plus some YG single flute HSSE and some Karnasch cutters. Are the Karnasch worth the extra money?

I've just bought a 2mm single flute cutter from cutwel last week for cutting acrylic, 10mm think stuff and ran at 24k 2000 feed 1.5mm DOC the finish is fine but needed some 400 wet&dry treatment not a great deal though.

I didn't bother with a finish pass no real need when I was polishing the edge anyway, it cost 32 or 34 and like a tool it slipped from the collect and lucky as I am hit a metal bolt I use to hold the spoil board down :( still cuts ok but not the same :(

Top tip before undoing the collect nut put a silicon boot on the cutter :)

But I've now change the profile method and use a larger dia cutter 10mm doc taking a finish pass, the edge is spot on, no wet&dry treatment and can be buffed to a shine straight on the buffer.

Can't be seen very clear but the finish is flawless using my new method, I now use the 2mm bit for rapid removal rate and semi finished profile.


http://uploads.tapatalk-cdn.com/20161108/7e67b5d228ccedcf83b0aa7b2b1f1c32.jpg