Those tiny bevelled letters

This forum is for general discussion regarding VCarve Pro

Those tiny bevelled letters

Postby James E » Wed Jan 10, 2007 2:49 pm

I would like to make some letters in 3mm acrylic, with a 10 degree sloping side, - they are to make moulds in sand for casting aluminium into. The tutorials and trial and error have got me quite a way.
I have seen some of these letters that have been made previously, and yes, the internal and external corners are sharp, ok no problem there, but on some of the small text - like a double-decker 'g' where the upper loop and the lower loop almost touch, the bevels nearly meet at the bottom, but there is such a tiny gap- less than 1mm-. This can't be a tapered end mill can it?
So I have been trying with a 20 degree included engraving bit with some success.
Is this a good way?
I can't get a very smooth finish as requred to allow the sand to release the letters,
Is this just spindle speed and feed rate, and if so what do you guys reccommend?
I'm not a total novice, but this job...I need help.

Thanks in advance

James
James E
Vectric Craftsman
 
Posts: 229
Joined: Wed Jan 10, 2007 2:26 pm
Location: Derbyshire UK

Will this help!

Postby Jonmilligan » Wed Jan 10, 2007 11:34 pm

:idea: Hi James, I used to make rubber stamps for a company,I used 3mm acrylic for the molds and then poured silicone into them. After much experimenting I ended up using an Antares Inc. rubber stamp engraving cutter, it worked really well. Antares is in the States, but they have agents in most countries, if not, they ship direct. They are a good price and very high quality cutters, I hope this helps
Regards
John Milligan
[url] http://www.antaresinc.net/2004EngCutSet.html
Jonmilligan
 
Posts: 38
Joined: Thu Sep 21, 2006 6:48 am
Location: Caniambo, Victoria, Australia

Thanks

Postby James E » Thu Jan 11, 2007 6:43 pm

Thanks for that John, its an interesting site, and there is a distributor in the UK, although I have found them a bit awkward to deal with. With that in mind, could you give me some idea of the feed and speed and depth of pass you used with these cutters? I'm more used to end mills myself.

Thanks again

James
James E
Vectric Craftsman
 
Posts: 229
Joined: Wed Jan 10, 2007 2:26 pm
Location: Derbyshire UK

Postby James E » Fri Jan 12, 2007 1:08 pm

Yes, just to follow up, I have ordered what the company expert purports to be the ideal tool, but when I asked for speed and feed and depth of pass he said he didn't know, it depends on the machine. I can't understand that.
Any info gratefully received.

James
James E
Vectric Craftsman
 
Posts: 229
Joined: Wed Jan 10, 2007 2:26 pm
Location: Derbyshire UK

Postby James E » Tue Jan 16, 2007 12:52 pm

Mmmm, well I tried the cutter, and it gives a marginally better finish, but it doesn't help with the problem of re-attached dust on the cut edge of the acrylic. Any ideas of cause or cure for this?

Thanks in advance
James
James E
Vectric Craftsman
 
Posts: 229
Joined: Wed Jan 10, 2007 2:26 pm
Location: Derbyshire UK

Postby Wemme » Tue Jan 16, 2007 8:00 pm

With cast arcylic i get dust weld on mainly when the cutter is getting too hot.
tooo low feed rate, too fast spindle speed and a blunt cutter add to this.
I find if i'm nearing a cut and dust is starting to weld on I blow compressed air at the tool.
clears the dust and cools the tool.

Regards
Bart

James E wrote:Mmmm, well I tried the cutter, and it gives a marginally better finish, but it doesn't help with the problem of re-attached dust on the cut edge of the acrylic. Any ideas of cause or cure for this?
Thanks in advance
James
User avatar
Wemme
Vectric Wizard
 
Posts: 506
Joined: Mon Jan 30, 2006 6:31 am
Location: Christchurch, New Zealand

Postby Peter Stenabaugh » Tue Jan 16, 2007 10:59 pm

Hey guys, recently I was playing around trying to cut some lexan on my mill. I was pocketing out some text that I had inserted from Vcarve, then converted the text to curves so I could pocket it out. The first attempt worked not too bad, but I had a lot of fuzzy burrs around all the edges, which was way too much to have to clean up, besides when cleaning lexan, any slips will badly scratch your material. I did a couple more of the same engraving, but this time I gave the project a periodic spray of WD-40. This solved all my problems. The finish cut was clean, almost no burrs at all, and any that I did have cleaned off with a finger nail. I was using Vcarve for the pocketing routine, and a nice new sharp 3/32 3 flute end mill for the pocketing. All I got was a bunch of really small chips and very little mess. The WD-40 cleans up easily with some soap and water.

Speeds and feeds were about 2400 rpm on the cutter and 20 ipm feed.
The 5 letters (AFIRS) cut out at .040 deep took about 15 minutes.

Give the WD-40 a try, it might work for you as well.

I really prefer not to have to engrave into lexan as it is so soft, that it scratches so easily. I would much rather use Corian.

If you guys are looking for sources of free Corian, check out any local cabinet / counter top fabricators that use Corian or similar products. If you offer to do a bit of engraving for them from time to time, they will most likely give you all their scrap sink cutouts etc. The sink cutouts make really good custom cutting boards, for their customers.

Corian is really nice to cut, almost any speed and feed seems to work. I have tried everything from about 5 ipm to 40 ipm and with speeds of 2400 and 15000. I get no problems, and the chips come off like thin feathers - easy cleanup and no melting of the material on the cutter - so far. I did find that at 2400 rpm on my mill, that I had to keep the feed below 30 ipm, or else I started to get rough sides on the cut, just due to too fast a feed rate for the rpm being used.

Pete
Peter Stenabaugh
Vectric Craftsman
 
Posts: 189
Joined: Wed Jun 07, 2006 7:26 pm
Location: Calgary, Alberta Canada

Postby Wemme » Wed Jan 17, 2007 2:01 am

Hi Pete.
Thanks for sharing, I will give it a go next time I am cutting.
It may make my tools last longer than they have in the past when cutting cast Acrylic.
Regards
Bart
User avatar
Wemme
Vectric Wizard
 
Posts: 506
Joined: Mon Jan 30, 2006 6:31 am
Location: Christchurch, New Zealand

Postby James E » Sun Jan 21, 2007 7:46 pm

Thanks Pete the WD40 has cleaned the edges up a lot. It's the half rund half flat engraving type cutter that I am using. I don't have any trouble with twin or triple edge tools.

I'll get some compressed air set up soon and try that as well.

Thanks again

Jim
James E
Vectric Craftsman
 
Posts: 229
Joined: Wed Jan 10, 2007 2:26 pm
Location: Derbyshire UK

Postby Peter Stenabaugh » Mon Jan 22, 2007 12:38 am

The only other thing to watch out for when machining any type of plastic is to make sure your cutter is really sharp. Plastic has a bad habit of dulling your tools really fast. The reason that happens is that you are not machining at the "sweet spot" with regards to feed and speed. It is a trial thing to figure out and can take many hours, which is why most people dont bother, unless you are doing it all the time and the cutter life is important.

There is a web site you can check out that explains this in more detail, but I dont have the link on this computer, but I will have it in a couple days if you want it. I did post it a few weeks back - somewhere, but I dont remember the thread.......

You could also try a google search on 'feeds and speeds" to see what you get .......

Pete
Peter Stenabaugh
Vectric Craftsman
 
Posts: 189
Joined: Wed Jun 07, 2006 7:26 pm
Location: Calgary, Alberta Canada

Postby James E » Mon Jan 22, 2007 11:16 am

Thanks Pete that's a great link
http://precisebits.com/tutorials/calibr ... speeds.htm

I found it in your previous posts

Jim
James E
Vectric Craftsman
 
Posts: 229
Joined: Wed Jan 10, 2007 2:26 pm
Location: Derbyshire UK

Postby Peter Stenabaugh » Mon Jan 22, 2007 6:34 pm

Yep, that's the one. I got a lot of useful information from there.

I did do a test like they talk about at the end where you make a continuous snaking path. I made mine 2" on the long side with a 1/2" crossover. I changed and increased the feed for each long pass. I went from 5" ipm to 45 ipm, for a test on my freshly converted cnc milling machine. I did a test in some Corian and some UHMW sign plastic. Both turned out great. With my cutter - a 1/4" spiral upcut - at 2400 rpm, it did not make any difference in either material, as to the feed rate. They both cut really cleanly with no burrs, except a couple of little curls in the plastic at the corners. I guess it would be even better to have an arc at the ends to reverse direction, then your cutter would not slow down so much, and it might be a truer representation of actual cutting conditions.

At any rate, in the Corian I found that even though it cut really well at the higher feed rates, I started to get a rough finish on the sides of the cut surface due to the fact that the feed rate was too high for the cutter rpm. So it appears as though the 'sweet' speed for corian, at 2400 rpm is about 25 - 30 ipm. The plastic did not appear to exhibit any roughness on the cut surface, although I did not test beyond that point. It would also be good to do the same test with a V bit, as this is where you would see the surface roughness to be more apparent.

Good luck.

Pete
Peter Stenabaugh
Vectric Craftsman
 
Posts: 189
Joined: Wed Jun 07, 2006 7:26 pm
Location: Calgary, Alberta Canada


Return to VCarve - General

Who is online

Users browsing this forum: BigC and 45 guests