• I want to thank all the members that have upgraded your accounts. I truly appreciate your support of the site monetarily. Supporting the site keeps this site up and running as a lot of work daily goes on behind the scenes. Click to Support Signs101 ...

Cutting 1" acrylic

S

SignMonger

New Member
Does anyone have any tips on cutting 1" acrylic letters with a 1/2" bit. I have been adjusting my feeds and speeds to try and eliminate all the heat on the bit. Right now I'm at 475 ipm with 14000 rpm. I've been adjusting to get a larger chip hoping that will cool the bit but the more I experiment, the more I wonder if it's just a matter of the pocket being so deep that I will not be able to cool the bit with bigger chips. This is my first time cutting 1" acrylic letters and I can't find any info out there about routing 1". Is anyone even doing this? My boss handed this job to me last minute due to the fact that the waterjet company we normally send this stuff to busy and would charge us a rush fee due to a tight deadline.

I'm using Onsrud 60-249 1/2" bit and 1" clear acrylic.
Any advice is much appreciated! Like I said, I've never done this and I'm not sure if others do this or not.

Thank you in advance!!
 
WB

WB

New Member
is that 475 inches per minute?.. seems awfully fast. My 1st thoughts would be 80-100 at 15000-18000rpm.

thickest I've cut is 1/2" though with a 1/4" bit.

Also I use single flute bits.

try 400ipm at 18000rpm like this video

[video=youtube;ra00bFLlYB0]https://www.youtube.com/watch?v=ra00bFLlYB0[/video]
 
S

SignMonger

New Member
Yes, that's inches per minute. I used a speed/feed calculator that got me to 432 ipm at 16000 rpm. I kept adjusting from there because I was still getting a lot of heat built up and not very large chips.
 
G

GaSouthpaw

Profane and profane accessories.
I second the opinion that you're going far too fast (with too low a spindle speed, too).
Though I never used a 1/2" for cutting letters, I have been able to do 4 pass cuts running use 1/4" or smaller bits on 1" thick acrylic (because the letters are viewed relatively close up) 100 per minute (+/- 10%) @ 24000 RPM and gotten great results.
While a feed rate calculator is great, I find that they often assume "perfect" conditions that don't exist in real world work environments. Kind of like when the guy who sells you, say, a plotter- and says it can track straight for 100' (or whatever) but doesn't bother to tell you they were using an automated feed and take up in laboratory conditions when they performed their benchmark tests.
Oh, and the material also matters. I'm not saying buy the top of the line stuff, but sometimes the cheapest material is cheap for a reason.
 
S

SignMonger

New Member
So, I tried the 400 ipm at 18000. It seems to be cutting nicely... still a lot of heat on the bit though. The spindle is getting pretty warm as well and that's the part that concerns me. I guess I just don't know how much heat is too much for the tool or the spindle. It's hard to say what is 'normal' since I don't have experience with this thick of material. I'm using two passes. When I called the guy who sold me the bit, he recommended 300 ipm @ 12000 or 432 ipm @ 432 (calculations from Onsrud catalogue using chip load). He said that using one of these should cause the bit to be warm but that I should be able to raise it directly out of the material and touch the bit without being burned. This has not been the case for either of the settings he recommended.
 
Westcoast Sign Guy

Westcoast Sign Guy

New Member
That all just seems real, errrr......too fast, for me anyway.

I use single flute Belin, but I would probably be more inclined to use 3/8" over 1/2" for 1" material.

My Colombo spindle's sweet spot is 12,000 RPM but I can go any, but I'd be going 7,500 rpm @ 2.85" IPS for 1/2", or 10,000 RPM's @ 2.5" IPS for 3/8"
 
astro8

astro8

New Member
100 inch/minute, 1/4" ITC single flute upcut, 18000rpm, 3 passes.
60 inch/minute, 3/16" ITC single flute upcut, 18000rpm, 4 passes.
I like to use only about 20 inch/minute plunge rate to save the tool tip.
Edit your start points to minimise tool bit jams.
Use dust/pressure foot and vacuum table to minimise small letters/centres popping out and jamming tool.

Of course you can run faster than these speeds, but this my 'set and forget' setup.
 
R

rossmosh

New Member
You're using the wrong bit. That bit is what you use on your last pass. To do most of the cutting you want to use a "O" Flute bit. Also you haven't mentioned your DOC. That's just as important as anything else we're talking about here. Also, 1/2" bit sounds awfully big for letters. Maybe I'm ultra anal, but I like to stick to 1/4" or smaller so the interior angles are as sharp as possible.

My plan of attack for something like this would be 3 passes with an "O" Flute 1/4" Bit, 15000RPM and 125IPM climb. I'd oversize the letters about .02" and leave a 1/8" onion skin. Then I'd run a finishing pass which goes full depth and takes off the .02" left over.

This article should be reasonably helpful: http://www.onsrud.com/plusdocs/Doc/index.html?model.code=TECH007
 
S

SignMonger

New Member
rossmosh said:
You're using the wrong bit. That bit is what you use on your last pass. To do most of the cutting you want to use a "O" Flute bit. Also you haven't mentioned your DOC. That's just as important as anything else we're talking about here. Also, 1/2" bit sounds awfully big for letters. Maybe I'm ultra anal, but I like to stick to 1/4" or smaller so the interior angles are as sharp as possible.

My plan of attack for something like this would be 3 passes with an "O" Flute 1/4" Bit, 15000RPM and 125IPM climb. I'd oversize the letters about .02" and leave a 1/8" onion skin. Then I'd run a finishing pass which goes full depth and takes off the .02" left over.

This article should be reasonably helpful: http://www.onsrud.com/plusdocs/Doc/index.html?model.code=TECH007
Click to expand...

Thanks for your input. I did realize today that I am doing this a little backward. These letters were supposed to go to waterjet but my manager gave them to me at the last minute. I had to program and cut immediately and, since I'm new to this kind of depth, I wasn't able to come up with the best plan on the spot. That being said, I should have gone with the 1/4" bit first and finished with the 1/2". Right now, I'm running the 1/2" first and cleaning up with the 1/4" bit. Some of the letters are so large that I'm leaving the inside corners finished with the 1/2" bit. These are letters that go on sign cabinets for a stadium so the largest letters are around 5' tall. Speed of cutting was the most important factor for this job. I'm getting good edge quality with 400 ipm @ 18000 rpm and the bit seems to be staying cool now. I had six 4'x8'x1" to cut, started yesterday morning and I will be done here in about an hour. I'm looking forward to learning more and to adjusting my 3/4" push-thru programs with the knowledge I've gained from this experience. Thanks for the article as well!... it's really interesting to see all the differing opinions and strategies on here.
 
B

bjt140

New Member
If you're ever in a tight spot I'm in Boulder and can laser cut that for you. I had a shopbot for awhile but found the laser to be so much easier!

Good luck!
 
johnnysigns

johnnysigns

New Member
Onsrud provides their feedrate formulas and chip loads in applicable materials. Feed rate (Inch per min) = RPM X # of cutting edges x chip load.

1/2" Diameter 60-200 series calls out a 0.006-0.010 chip load per tooth in hard plastics.

If I average that to 0.008 for the chip load @ 1/2" deep cut I'm at 336 IPM for 14,000 RPMs.
 
Ian Stewart-Koster

Ian Stewart-Koster

Older Greyer Brushie
For 1" thick acrylic, I also use a 1/4" endmill.
Why remove more substrate than you have to? A 1/2" endmill will have to cut out heaps more, for no great improvement in edge finish - and less tight internal corners.

We have a couple of 1/2" endmills, but have kept them for some routing of 3" acrylic - especially where we needed to get the depth! That was interesting going!

I'm guilty of going far too slowly for the official charts, but I've broken enough cutters to be wary.
As long as the shavings don't glue themselves back together I'm happy!

The o-flute onsrud cutters are terrific.
The chinese ebay ones are not so terrific!
 
S

signdog

New Member
There is a big difference in quality and ease of cut with Cell Cast acrylic, as opposed to the less expensive
Extruded:smile:
 
You must log in or register to reply here.
Top