Shallow angle profile cut in acrylic mirror

Hello!
I am trying to cut shallow bevels in acrylic. That is nearly a perpendicular cut, between 2 and 10 degree angles.
Does anyone have a bit that they like for this? We thought we'd start with 3 degrees.
Thinking of trying this one:
http://www.advantagesgs.com/Gerber-R...-1-4-x-1-8-x-1
and there's this:
http://www.amazon.com/Tapered-Ball-N...B2CNP4GP91QR1B
And Amana:
http://www.amanatool.com/bits-fv/462...ated-Bits.html
and Onsrud:
http://www.onsrud.com/xdoc/TaperBits

These vary in price from $45 to $140 and it is very difficult to know what would work best.
Does anyone have any suggestions as to spindle speed or feederates for this kind of cutting?
Also, the Amana listing has 1/32" angled bits on there. We don't even have a collet for our shopbot that will hold less than 1/4". Does anyone run 1/8", 1/16", or 1/32" bits? Don't they snap all the time?
Thanks for any thoughts on this.

We posted a while ago when we were looking for a variable angle bit. This seems like a better way to go.

Explain more what you are trying to do...

Are these profile cuts with a beveled edge, or are you adding some decorative engraving to the surface?

If the former, you can use a tapered end mill, although it will not be as clean cutting as a tool made for plastic (O-flute geometry). If the latter, you'll want some kind of v-bit and less than 10 deg is hard to find. You could do it with a variable angle chamfer bit, but the profile would have to be cut 1st and then beveled.

-B

Magazines, We run 1/8 to 1/16'ths bits all the time, everything below .125" uses the 1/8" collet. Spindle or router?
We don't do plastics like you,so can't help you there.:(

Who is Magazines and what do you do?

I didn't know SB would allow a person to hide behind an alien name.

Joe Crumley

We need to know what kind of machine and what you are trying to accomplish if you want constructive help.
Bob

Hi All,
I'm still getting used to this forum and how to enter information, please bear with me. Also I have little experience with shopbot or cnc in general. Looking to learn as much as I can.
Thanks for the responses.

Brady, yes these are to be profile beveled cuts and there are no plans to engrave the surface of the mirror. There will be hundreds of pieces of acrylic mirror cut at around 1-4" widths and 8" lengths. The bevels will be on the long sides. This is really to get around the fact that we don't have a 5 axis machine - we want to cut angles into the sheet. Generally we are cutting sheet goods, mostly baltic birch plywood and acrylic but some other stuff too.
Thanks for pointing out that we should use O flute bits. We have one and have used it with success on acrylic but it does not have an angle. I have heard conflicting things about O flutes, can someone clarify how they differ from normal flutes? I have found no O flute tapered bits, but some with 2 or 3 flutes.
A variable angle chamfer sounds perfect! Do you have any to recommend for plastics?

Scott, thanks for the info about smaller bits! We don't even have a collet for 1/8" bits but I'll move forward without fear on smaller bits now. A friend is cutting acrylic on his mastercam cnc with 1/8" LMT bits but he said he's using 24k spindle speed at 100 inches per minute. As far as I can tell our PRS standard Shopbot with HSD 4hp spindle will not spin that fast. I did not setup the machine and the person who did has moved on. I've found manuals for the shopbot and the spindle driver box but nothing about the spindle! I have been told that with plastics, it is best to run at the right speed - too fast one gets problems and the same with too slow. Is this right? It would be great to know if I can slow it down to 14k.

Hi Joe, I'm sorry about using an anonymous name. I always do for any online forums and didn't want to change for this one. I'm sensitive about online privacy and didn't want to make up a fake name (that would seem weird to me!). But my first name is Peter, so if that works I'm fine with using that. I want to learn and have found it challenging so wanted to post a question or two.

Thanks for any further advice on this project!
Peter

2nd part post:
Also, I wanted to add that when I called Amana to ask about their bits, I was recommended to call up Woodline.com. When I got them on the phone, they were very helpful and explained that tapered bits are pretty unusual but that a rounded ball bit such as the links I posted would probably work. He recommended that I be prepared to cut 1/8" into the sacrificial board to get past the ball part. As it turns out, they had cut some custom ones before for a job a few years back and are going to make a 3degree version for me for $80. That sounds good, so it is on it's way. Apparently 3 flutes, but not O-flutes. He said he'd include recommended feed and spindle rates, which is a huge help.
Does this sound like a good way to go?
Peter

Hi Peter, As I said, No experience with ANY kind of plastics, but feed and speed are co-dependent, if you are in the "sweet spot" for the material and it's cutting the way you want---If you want to increase feed for production you have to increase speed roughly in proportion.
With smaller bits just use some scrap and shallow passes and conservative cuts until you get what you want and then tweak it up incrementally until cut quality is unsatisfactory and then back it off 5-10%.
Plastic is different than wood though.

Edge cutting O flutes don't come in angles so you can stop worrying about that, but I would investigate them for straight cuts in acrylic. Which one works best is very dependant on the type of acrylic, what size parts you are cutting, thickness, hold-down etc. It varies a lot!
For any mill if you can't run as fast a spin as reccomended then you speed up the feed speed accordingly.
I don't know what kind of edge quality you need, but typically when a Shopbot cuts acrylic the edge needs at least some sanding to really look good. For your parts I would make up my toolpaths by drawing vectors to cut on, take into account the diameter of the bit, and draw a continuous squared end zig zag first in the x direction and then in the y so it is cutting continuously making long strips first and then for the squares crosscutting the parts. You need good hold-down vacuum to do this. It is difficult to stop part movement when the parts get small even with a good vacuum and I would bet that Brady would reccomend his transfer tape hold down system for this. I think he has a link to it bookmarked and will likey post it here soon! I know even though I have a pretty good vacuum I would likely use his system for these parts instead.
Since your crosscuts don't need to be bevelled I would use an o flute here. I like straight single flute cutters often as they neither push cuttings down nor try to lift the part, and when cutting at the right feed and speed the cuttings don't get hot enough to reweld. Transfer tape hold down may enable you to use an upcut o-flute, which is better for some acrylic.

Cast acrylic cuts best. Extruded is a bigger pain and I only use a straight o-flute for that.

Virtually all of my acrylic cutting is with cast that is thicker and I actually use a fairly slow speed and feed for best edge. (Like 1.5-2ips and 8-12k) I ramp in instead of straight plunge

Peter,
You can use a regular old tapered (square) end mill if the angles are that shallow.

However...CNC as wonderful as it is, isn't always the most efficient way to cut something. I would entertain the idea of using an edge sander like the ones Grizzly sells to put those shallow bevels on the edge.

Either CNC routing or sanding will require edge polishing or flame polishing depending on your project's needs & the level of polish required.

Just a thought...

-B

Thanks to everyone for their suggestions.
Well, I got a chance on Friday to try out a tapered bit. This is an onsrud 1/4 shank upcut with a ball nose. The results were not the best and I wonder if anyone has any suggestions about what to do differently.
But I fear I may have other problems. I read about problems with chatter, but the cuts that I made are wobbly has all get out. I did 2 ips at 12k Rpm and then went down to 1.5 ips and 1 ips at 14k rpm and then did .5 ips at 14k. Thanks for the suggestions for feed and rotation, Dave, can you check out these images? I'm guessing you get better quality from yours if you have it dialed in.

These are 1/8 acrylic mirror on the bottom, 1/8 sintra mounted to protect the back. Most of what you see is sintra, but it gives a good idea of variation of line. All but the 1/2 ips is pretty unusable, and that is not what I would consider great.

Unfortunately another user broke our o-flute bit, so I have to wait to try that.
I don't know whether the images will appear in line or not, but here are some pictures.
These are named with speeds.
There is also one showing how the plastic dust sticks in the cut. I had our vacuum table on with all the dust removal working.
I would still really appreciate any further guidance you all have. I can't work on this but every couple of days, but really want to get to the bottom of it!
Thanks
Peter

So in my last post, the 1st image of the O is 2 ips at 12k rpm. The second one with the 2 S's is 1 ips at 12k, the 3rd with the N is .5ips at 12k. The 4th shows the cutting debris and the 5th shows the E cut at 2 ips at 14k. These are supposed to be straight lines.

Dave, what is your recommendation about ramping?
Brady, I don't have the money right now for an edge sander and our shop doesn't have one. Im trying to get the best cut off the bat so that the hundreds of cuts have the least amount of followup work. I'd say the diamond edge thing is way out of our price range. To make the best initial cut in acrylic, I've heard table saw, router, jointer, etc. Still trying to figure out for myself though.
THanks
Peter

Oh, and is there a standard Shopbot cutting pattern to gauge how well the machine itself is working? A test pattern of some kind that people compare apple to apple to be sure they are getting what they should?
Thanks

would it help some to reverse (climb) the cuts, some of it looks like tearout

It looks to me like the first thing you need to do is power up the machine & shake down every axis with considerable force (don't overpower it) - and see if you can track down if the pinions are loose. Those cuts are horrible.

You should NOT be using a ball end tool unless you are doing 3D or decorative engraving. The tapered bit should be square. Your RPM is too low for plastic - you want to be in the 16-18k range, and slow that move speed down. Shoot for 1.2,0.7 for your XY, Z speeds and adjust as needed. No sense in running 2" per sec on a 2" tall letter, right? Do your cuts in multiple passes using a smooth ramped entry (in profile toolpath options in VCP/Aspire) - 1 pass may be too deep causing the motors to stall.

You may also want to adjust your VR settings to the numbers I lay out in the Ramping Article - but check for mechanical slop first.

Let us know how you make out. What model machine are you running...Assuming it is a Standard?

-B

It does look like machine! The cuts should look Much better.
Peter, I'm totally guessing, but you have basically 2 different materials. Maybe 2 toolpaths for the same bit? One pass at your dialed in speed and feed for the full depth (plus a hair) of the top layer, and then a second pass to your full depth(at THOSE best feeds and speeds for the bottom material).
But first figure out what is loose on machine and make sure material isn't moving at ALL.
Like I said Guessing what I would do, if I were trying it. I might even try an offset of .01" on the top layer so the second toolpath would just have to remove a skin and bit deflection would greatly lessen.
I could be ALL wrong because it's plastic.:(

I have cut acrylic with foam
you have to take in to consideration both materials plus your glue
and also your vacuum. pieces move if not glued properly.
glue builds up on bit
you may need to use 2 different bits for the 2 different materials or at least multiple passes
2 materials could cause vibration
if you would like additional info PM me

Frank

here is a pic of acrylic and foam I did

Your issues are starting before your cut. There is something or a bunch of things not dialed in on the mill. Brady got here first with the reply and he is completely correct. Check pinions for wear and tightness. Check every bolt. Make sure your motors are engaging properly. It could also be time for a new collett. Your vacuum may not be holding well enough. No matter what bit you use in what material you can't get professional results unless your tools are tuned up.

Sandblasting should be left to the pro's. If you have a CNC go for that.

When I look at the witness marks in your spoil board on that last picture I see uneven vectors. You may need to do some serious node editing. Bob

There are a number of things that stand out. The original post implied that there were straight cuts in the 8-10" range in acrylic mirror that had to be made. Your latest post shows a laminated material, with materials of different densities and curvy letters - not the same animal at all. There are several concessions that have to be made or you might as well just use a jig saw.

Quote:

---

Originally Posted by magazines

Unfortunately another user broke our o-flute bit, so I have to wait to try that.

---

You absolutely need to have o-flute tools to cut this layup with any degree of quality. An end mill isn't going to give you the edge quality you want & you'll spend a TON of time on the back end cleaning up. You need to get single and double o-flute tools to make your best effort. A triple flute may be in order if you need to sneak up on final edge quality. Find your Onsrud dealer & let him tell you what tools you need. This is what they do for a living.

If you still require a beveled edge, then you do the majority of your cutting (say 90% through cut) with the o-flute tool, then swap out for a SQUARE end mill with taper to just kiss the edge and go the final depth. This will result in a cleaner edge than using the taper itself, but still not as clean as a square cut o-flute bit will.

This entire job - laminated dissimilar materials with beveled edge - is a lesson in compromise. You need to experiment with tooling and technique and carefully select the best overall compromise in edge quality, time, expense and hold that up against what the customer wants & is willing to pay.

-B

Wow, thanks to everyone for the replies. I can't work on that machine today but will get back to it tomorrow. We are in an academic setting and the technician who set up and maintained our machine moved across the country a couple of months ago. We are trying to get a handle on maintenance and running this particular job at the same time.
Brady, thanks for the suggestion of feed and rotation with ramping. I've never run ramps before and will be looking at your article which seems quite helpful. I tried the speeds that I did based upon other recommendations and slowed it down as it became clear that we were not getting what we should.

From the bill of purchase and looking at the machine itself, we are running a PRS Standard shopbot with a 4x8 bed. The spindle says that it is HSD brand and 4 hp. As far as I can tell it maxes out at 18k rpm. I know someone who cuts acrylic with 24k at 100 inches per minute and gets excellent results, but that totally different setup with a mastercam etc.

Yes, the goal is to cut acrylic in the manner that the original post says. I had a few minutes at the end of the work week to test out this tapered bit so decided to cut out a couple of words - it seemed like a good test.
Does anyone know of a standard cut test?
The vendor of the acrylic mirror recommended the mounting to sintra to protect the mirror backing. Due to it's softer material makeup, the sintra has been fine to cut on the tablesaw ,but it appears this may be a drawback with the cnc. I can say that it appears to not be causing a problem. We may consider mounting to another plain sheet of acrylic to standardize moving forward.


It's unfortunate to find out that the ball nose is not a good tapered bit for this purpose. We've got another one coming at a 3deg angle from woodline that they custom made.
Is this the kind of endmill bit that you were thinking of:
http://preview.tinyurl.com/o2hthan

For tapered bits, Amana send us to Woodline and Onsrud recommended a similar ball nose.
Thanks,
Peter

Quote:

---

Originally Posted by Tim Lucas

would it help some to reverse (climb) the cuts, some of it looks like tearout

---

Thanks for the recommendation Tim. We are going to design a test pattern and will try climb cuts in multiple passes to get a better edge.

Quote:

---

Originally Posted by bradywatson

It looks to me like the first thing you need to do is power up the machine & shake down every axis with considerable force (don't overpower it) - and see if you can track down if the pinions are loose. Those cuts are horrible.

You should NOT be using a ball end tool unless you are doing 3D or decorative engraving. The tapered bit should be square. Your RPM is too low for plastic - you want to be in the 16-18k range, and slow that move speed down. Shoot for 1.2,0.7 for your XY, Z speeds and adjust as needed. No sense in running 2" per sec on a 2" tall letter, right? Do your cuts in multiple passes using a smooth ramped entry (in profile toolpath options in VCP/Aspire) - 1 pass may be too deep causing the motors to stall.

You may also want to adjust your VR settings to the numbers I lay out in the Ramping Article - but check for mechanical slop first.

Let us know how you make out. What model machine are you running...Assuming it is a Standard?

-B

---

It's good to hear that we should expect more from the machine. It is a standard shopbot with HSD 4 hp spindle. It appears that 18k is max rpm.
I was not involved in setup or construction of the machine, so this is quite helpful but also unfamiliar.
So, to check pinions I should turn it on and run the spindle warm up routine, zero it, then I push it physically - by hand? Is there a way to look for what area to tighten? On the gantry or the sides? I'll certainly give it a once over and tighten anything that seems loose, just trying to figure out what to look for.
The collet is new.
Thanks

If the only purpose of the Sintra is to protect the mirror, then I would just get a 12 or 24" roll of transfer tape, which is like masking tape, available through sign supply houses & cover it with that. It's cheaper in the long run. I don't know how you are attaching the Sintra to the mirror - ???

Sintra cuts beautifully on these machines with a single or double o-flute. So it isn't an issue with the right geometry. You can get by with an end mill, but the finish is not as nice.

FYI - ShopBot has techs in your area that can give you training and tune up the machine in your shop. Call them to inquire. 2 days of training would pay for itself in no time considering you'd be 'getting all the answers' to your questions right away.

Your 300Hz spindle is fine. It's nice to have a few extra RPM, but there is no impediment to you cutting what you want.

You don't want to use a BALL end mill - if for no other reason than you will be left with a cusp on the parts that looks like this---> л - which is probably NOT what you want. You could get around this by burying the bit into the table until it no longer imparts a cusp on the edge, but this is frowned upon for a number of reasons.

-B

Quote:

---

Originally Posted by bradywatson

If the only purpose of the Sintra is to protect the mirror, then I would just get a 12 or 24" roll of transfer tape, which is like masking tape, available through sign supply houses & cover it with that. It's cheaper in the long run. I don't know how you are attaching the Sintra to the mirror - ???

Sintra cuts beautifully on these machines with a single or double o-flute. So it isn't an issue with the right geometry. You can get by with an end mill, but the finish is not as nice.

FYI - ShopBot has techs in your area that can give you training and tune up the machine in your shop. Call them to inquire. 2 days of training would pay for itself in no time considering you'd be 'getting all the answers' to your questions right away.

Your 300Hz spindle is fine. It's nice to have a few extra RPM, but there is no impediment to you cutting what you want.

You don't want to use a BALL end mill - if for no other reason than you will be left with a cusp on the parts that looks like this---> л - which is probably NOT what you want. You could get around this by burying the bit into the table until it no longer imparts a cusp on the edge, but this is frowned upon for a number of reasons.

-B

---

We have applied 3m pre-mask to the front surface of the mirror prior to cutting. The sintra is applied to the back surface to protect the mylar mirror part during cutting but also when these individual pieces get glued to the final support - wood columns. So there has to be some kind of backing for gluing and sintra was recommended due to its ease of cutting and porousness - the recommended adhesive is silicone for flexibility. The mounting material is also silicone based for flexibility between the acrylic mirror and the sintra. It is a pressure sensitive film called opti-clear.

Also, I realize now that one of the tests that I posted pictures of (the 2ips letters, the most wobbly ones) were solid sintra, not this laminated acrylic sintra thing.
These tests were cut .05" into the sacrificial LDF board to avoid the ball part. The tabs that I used definitely show the curvature and it is not great for the part. But since I have now two ball nose tapered bits in shallow angles, can you elaborate more on what the drawbacks of cutting into the LDF are?

I am now planning on several approaches for testing.
1.2 pass profiling : rough cut with Oflute unbeveled, followed by tapered end mill.
2.Ball nose bits we have purchased, in two passes first to clear the sintra, adhesive and mylar then 2nd pass to cut the acrylic itself.

I will be tugging and pushing on the head tomorrow and tightening anything that I can find. That said, I am certainly going to push for us to have a shopbot person come by to check out our setup and give direct suggestions.
I'm assuming that I ought to contact Shopbot directly for this, correct? You don't know anyone in the general Southern California area do you?
Thanks

Quote:

---

Originally Posted by bobmoore

When I look at the witness marks in your spoil board on that last picture I see uneven vectors. You may need to do some serious node editing. Bob

---

Thanks for the heads up. I'm going to make another test file and be sure the vectors are right on with that one. This was text made in sketchup and imported, then cut with an "on" vector path. This may have led to the characteristic you describe.

Quote:

---

Originally Posted by FSICM

here is a pic of acrylic and foam I did

---

Frank, those look like excellent multi-material cuts. I'm going to see what I can do with the machine and then may very well send you a message with a question once I get everything in order.
Thanks for the offer!

Yes - contact SB directly for services.

You don't want to eat into your LDF because it now becomes a channel for vacuum to escape...and it fuzzes up the board and causes other problems that need attention. If you are only running 1 sheet - not a huge deal...but if you are running several, it will give you problems.

-B

I, for one, can't imagine the machine being that whacked up. It looks like substrate movement.

I just can't imagine the machine could be that loose. If this was my machine, I'd "SCREW" some masonite down on the bed, set some good type and carve away. Lets say you try some 2" script and Helvetica as a first test. Use Screws, not vacuum.

Joe

Brady, You still helping people to set up machines and solve specific production issues, or has that fallen by the wayside in the last year? You're not cheap, but I've seen posts saying you are worth every dollar and it was the best money they ever spent.:)

Scott,
Yes - Still doing that sort of thing, although I did take a hiatus for a few months this Summer. In the past year we had a number of family members that were sick or passed away - including my boy Grover (who you see sitting on the SB in my VR article) - and that had to take priority over all else. Things have simmered down, although there will be a few more moving on in the next few months. Such is life - and I felt no need to share sad news, because we ALL have our own 'stuff' to deal with on a daily basis. Just being thankful and showing gratitude puts all into perspective.

We now return to your regularly scheduled thread...

-B

Brady, Good to know, Sorry to hear.
Still can't believe I couldn't "Sell" you on the idea of visiting the "Tourist Mecca" of Kennebunkport and helping me set up "Gratis" :) I must be slipping, But probably learned more by doing it myself:)

Hi All,
I wanted to pick up this thread that had so much helpful information. Sorry for my slow response. In short, school started, everything got super busy, time on the shopbot was slashed, and we got it to work much better quickly.
Joe, you were right! Sure enough we had some real piece movement on some of our cuts with the original text cuts. The thing was that we screwed it down just to be sure after cutting about half of what we had done. The vacuum was just not strong enough with the small pieces. We had a newly leveled bed, but it couldn't do it. Now we are doing both vacuum and screw down. I have to say I don't like the screw down - and I don't like cutting through to a sacrificial board, but with tabs it makes it work and 1 sheet of mdf for every 10-20 cutting sessions is workable.
Also, we are now using the pre-mask on the surface of the mirror, thanks for this suggestion as well.
And thanks as well to those who suggested the two pass system. We are running the oflute 1/8" first over each of the toolpaths and then chasing it with the tapered end mill (no more ball nose). It is producing a cleaner cut now. Both o-flute and end mill are going at 14k and .5ips now. IT's accurate, it seems to still wobble a bit if we speed up much beyond this, but we don't really need to. Still makes me think we may have something a bit loose in the Shopbot, but it certainly was not the cause of the big wobbles that originated this thread.
Thanks to all for the help and suggestions. Sorry for the delay in response.
Peter