cutting small letters in brass

[changrudy]

Hi Everyone,

I need some advice here since my dilemna involves two problems in one.

I have a client who wants to cut small....real small letters in brass. I did a sample cut with the smallest bit I can find (1/64") on poplar as you can see from the picture.

Now I need to do this in brass. I've never cut brass before but from what I read, the feed rates are very slow (.3ips, .1ips) and no cooling is necessary. For this size bit, are these speeds still valid?

Any suggestion for a good supplier for these bits? the one I have (harvey tool) broke on a second try on hard wood.

Thanks in advance,

Rudy

[michael_schwartz]

Interested in this subject as well since I am thinking of making a brass branding iron, for signing work.

[beacon14]

That's pushing the tolerances of the machine. I'm guessing you'll have to be prepared for a lot of bit breakage at that size in hard material. I did some 1/4" high letters to match something that had been laser-engraved using a .02 bit in walnut, one bit would cut 10 plaques then the next one would snap right away. Your 1/64" bit will be .015" - good luck and let us know how it turns out. I would definitely do some test cuts before agreeing to cut this job.

You might want to look for end mills from McMaster-Carr or another industrial supplier.

[shoeshine]

I work in brass quite a bit these days, and yes you will break bits on doing these. Those aren't bad S&F #'s to start but you might neeed to pull back even a bit more. The key even more than speed and feed, is --extremely-- shallow passes, ramp every and I mean every, cut and cutting lubricant. I am doing production work with 1/8" bits and I make passes of .02". For a .015 bit I would not go more than .008 per pass and most "bots" arent really dialed in to be able to get resolution at that level. This is really more in the micro-mill territory.

anyway I would definately run several tests before you commit to that job. try www.pecisebits.com (http://www.pecisebits.com) for cutters and get a good sticky cutting oil. CRC makes a tapping (thread cutting lubricant) oil for tapping on vertical surfaces in a rattle can that might work.

alternatively, I might think about re-working the design to use Vcarving to get the lettering, You can use much sturdier bits. the advice about ramping, shallow passes, and lubricant still applies.

good luck
Chris

[geometree]

You may want to consider chemical etching. Take a look at this method and results. http://www.instructables.com/id/Big-Brass-Ones/

[changrudy]

Thanks for the comments guys, it's a place to start and I will do some samples before committing to this job. For some of the bigger letters, I can use a 30 degree v-bit but for the smallest letters I don't think it's small enough. Anyone know where to get a 15 degree v-bit? Centurion only goes to 30 I believe.

Rudy




I work in brass quite a bit these days, and yes you will break bits on doing these. Those aren't bad S&F #'s to start but you might neeed to pull back even a bit more. The key even more than speed and feed, is --extremely-- shallow passes, ramp every and I mean every, cut and cutting lubricant. I am doing production work with 1/8" bits and I make passes of .02". For a .015 bit I would not go more than .008 per pass and most "bots" arent really dialed in to be able to get resolution at that level. This is really more in the micro-mill territory.

anyway I would definately run several tests before you commit to that job. try www.pecisebits.com (http://www.pecisebits.com) for cutters and get a good sticky cutting oil. CRC makes a tapping (thread cutting lubricant) oil for tapping on vertical surfaces in a rattle can that might work.

alternatively, I might think about re-working the design to use Vcarving to get the lettering, You can use much sturdier bits. the advice about ramping, shallow passes, and lubricant still applies.

good luck
Chris

[dubliner]

You might try one of Gary Beckwith's .0625 ball nose bits. They taper down from a .25 shank to .0625. They might give you a little extra rigidity and uss all the other advice as well. I hate turning down jobs, but sometimes they cost you more in time and bits than you can realistically charge.

[changrudy]

Just a little update. I've tried cutting the same letters in a hardwood using a 30 degree v-bit. The resolution is actually quite good on the bot. Just waiting for brass to come in to do a real test. I'll keep you guys posted.

One thing I did learn with partworks is that I have to trick it into using the v-bit to do the area clearance with the same v-bit.

For example, cutting a 12pt helvetica font,

Pocket#1 Using a 30 deg v-bit only, the preview shows a cut barely below the surface.

Pocket#2 Using a 30 deg v-bit and a 1/32" endmill for large area clearance tool gives the message shown in picture "message". Continue to calculate toolpath and it gives a proper v-carve with just the v-bit.

Anyone ever experience this? Must be a bug in my opinion... I was lucky to stumble on this. What this means is that I can now try to cut the brass with v-bits as opposed to 1/64 bits.

Rudy

[changrudy]

Hey guys,

Another update if anyone is interested. Able to cut 0.135" high letters in brass using a diamond coated 1/64" bit. After breaking 3 bits, I went super slow (0.1 ips @ 0.005" pass) and cutting fluid to cut this one. Customer is happy, just not sure how to price this. It took 1.5 hrs to cut, no joke. I'm sure I can cut this down significantly by slowly raising the speed but at the risk of breaking an $$$ bit. Any suggestions?

Thanks for looking.

[blackhawk]

You may want to take a look at Brady's article on the Shopbot website about ramp and corner speeds. If you play around with these, you might help out your bit breakage.

I have engraved some letters on a metal working CNC mill. I have broken 1/8" bits when the cutter gets to a sharp corner in a letter.

[Brady Watson]

...After breaking 3 bits, I went super slow (0.1 ips @ 0.005" pass)

Any suggestions?


Rudy,
Type in VR to SB3. The 1st 2 values are going to be the most important for this type of work. These are the XY and Z Move Ramp Speed. If they are sitting at the default values (0.4 for Alpha, 0.2 for Standard), then you will NEVER go any slower than those values.

I would not go lower than .1 on either, although you may be able to do .05 if your individual computer and machine are OK with it. When you start getting down to these lower speeds, the clock that syncs the computer and control box can get a bit coarse - for lack of better term.

Shopbot has made provisions for slower cutting, and you can alter the Step Interval Divider on the VU screen in SB3. At the bottom, you will see "Slow Speed Generation for Unusual Requirements" - Below that the default value for "Step Interval Divider" is 1. Take care when messing with this & be sure to return it to 1 when you are done small cutting. Start with a value of 2 and see how that works.

Here's a quote from SB3->Help->ComRef.pdf:

Step Interval Divider (default = 1)

The standard movement speed or federate can be set as low as .05 (inches/sec; or 1.27 mm/sec) see [VS]. Occasionally, it may be necessary for a specialized application to move your tool at even slower speeds. Slower speeds can be achieved by dividing the timing interval between steps so that stepping is even slower. The step interval can be increased by whole numbers so that it is 2 times longer, 3 times longer, etc up to 100 times longer. This means the speed will be ½ slower, 1/3 slower, etc ... up to 1/100 the displayed speed. Only use the step interval divider when a very slow speed is needed.

So...If you set a MS,2.0,1.0 in your SBP file, AND you set the Step Interval Divider to 2, THEN your real life move speed will be MS,1.0,0.5

Don't forget to switch it back when you are done. You can also SAVE YOUR CURRENT config by means of the US command. Give it a meaningful name, like RudyBigCutting. Then, make your changes for small cutting and type in US and give it a meaningful name, like RudySmallCutting. Then, when you want to call up either, just type in UR, say yes to all the prompts, and point to the config you want to run.

Be sure to hog out with a larger tool(s), like 1/8", 1/16" and never plunge straight down. Always ramp into the cuts.

-B

[changrudy]

Thanks for the suggestions.

Brady-I don't have any intention to slow down the feedrates anymore since it's long enough as it is for this one item. I plan on doing alot of them. I do use a smaller bit to hog out the excess material.

A question though. I've tried entering many different ramp distances in partworks (1/4, 1/8, 0.05) but each preview I look at does not seem to indicate any ramping motion. Is it because it's too small to even notice?

Thanks,

Rudy

[waynelocke]

I have no real idea on price but could you make a master and have them cast in brass?

[Brady Watson]

A question though. I've tried entering many different ramp distances in partworks (1/4, 1/8, 0.05) but each preview I look at does not seem to indicate any ramping motion. Is it because it's too small to even notice?


Since you are using such small tools & moves, just select a 'Smooth' & 'Angle' ramp of 10 to 20 degrees. Then it will do it's own math for each letter and scale the ramp accordingly, rather than trying to find the right ramp length.

If you zoom in too close on the 3D toolpath preview, then portions of the toolpath will disappear. Zoom out a little & you should see the ramps. It may help to reduce your model XY size so that it is close to the artwork size in order to 'tighten' up the pixels at that level of zoom.

Compressed air coolant will help reduce tool breakage...DIY Air Coolant (http://www.talkshopbot.com/forum/showthread.php?t=4677&highlight=football+inflator&page=2)

-B

[changrudy]

Brady-that ramp angle option, is that in aspire? I use partworks and don't seem to have that option (v 2.505). Thanks for the cooling DIY, something worth looking into.

Wayne-I receive blank castings that needs a sequential number carved in it. So each one is custom cause each casting is unique in it's own way since I can't zero accurately enough with a jig to be able to do mass cut them.

Rudy

[Brady Watson]

I forgot you were doing a pocket...That option is only available on a profile cut in PWorks and Aspire. Sorry.

-B