PDA

View Full Version : Engraving speed for stainless



Ian Rankin
02-22-2010, 7:50 PM
Hi all.
Are there any engravers experienced in engraving stainless steel. I have a job engraving 300mm high Arial typestyle characters in 316 s/s. I have a Jaeger spindle in this machine (up to 60000rpm) and using tungsten cutter with a tip dia of 4.5mm. Could someone suggest feed rates / spindle speeds best suited to this job.

Thanks in advance

Regards
Ian Rankin

Dave Johnson29
02-22-2010, 8:12 PM
Are there any engravers experienced in engraving stainless steel.

Hi Ian,

How many cutting edges?

For 316 SS, a single lip cutter and 0.002" per cut, carbide cutter 5500rpm and 11-inches per minute according to my milling cutter calculator.

You will need some cutting fluid, at least WD40 sprayed on frequently.

If that doesn't help, give me the number of flutes cutting, the desired amount per cut and I can calculate it for you.

Ian Rankin
02-22-2010, 8:40 PM
Dave,
Thanks for showing an interest. I am using a single edge D type cutter with a tip dia of 4.5mm. I am covering the surface with a cutting oil. From memory I am using a travel speed of .2 inches per sec spindle speed varying from 12000 - 20000 rpm. and a depth of cut .25mm. Sorry for the mixture of metric and inches. Is there a chart for all this info for various materials for different tip diameters etc.

Kind regards
Ian

Dave Johnson29
02-22-2010, 9:14 PM
Hi Ian,

There may be a chart but I use a calculator I wrote in some CNC software I developed. I used the Speeds and Feeds formulas from Machinery's Handbook edition 25. It is the Engineer's Bible.

In my software I enter the material, the cutter diameter, cutter material, cutter flutes and the depth of cut per rotation. I guessed at 0.002" cut per rotation. At 2.5mm deep (0.010") the depth is not an issue.

At 0.2"/sec that is 12"/min so probably a bit fast for the 5500rpm I quoted earlier.

If you can't go below 12K rpm then feed would be 24"/min or 0.4"/sec at 12K rpm.

If rpms are too high you will eat the cutter on the stainless. Also you stand a good chance of work hardening the material making it even harder to cut.

Mixing mm/Inch is no problem. Happy to help.

Rodne Gold
02-23-2010, 2:50 AM
Apart from feeds and speeds, cooling when cutting stainless is cruicial cos if you work harden the piece in the cutting path , you might as well throw it away as you can never get past that. Best to use a coolant feed when doing so.
By the way , TC cutters are not a great option for stainless , HSS cutters or the like are much better - the TC cutter is brittle and tends to chip on the cutting edge leading to a lot of heat generation and thus work hardening.
Apart from that , a good strategy is to have as little of the cutter protuding from the collet as possible , as the longer the cutter , the more it flexes and for stainless that's not good.
Google "speed and feed calculator" , lots of em online. like this one
http://www.daycounter.com/Calculators/GCode/Feed-Rate-Calculator.phtml

Dan Hintz
02-23-2010, 7:58 AM
Wow, I feel like I stepped off of the plane into another world... different language ;)

Keep talking, I'll learn it all eventually... :D

Dave Johnson29
02-23-2010, 10:54 AM
Ian,

If you go with HSS you will need to drop the speed and feed by at least 4 times, maybe 5 or 6.

I use only carbide cutters for SS but I do have a flood coolant that is running at about 6 gallons per minute.

Maybe try using two-flute a ball-nosed milling cutter instead of an engraving cutter.

As Rodney suggests, keep the exposed cutter short. I have even snapped them in half so I can get them deeper into the collet for minimal exposed length and max stiffness. Good point Rodney.

Dave Johnson29
02-23-2010, 10:55 AM
Wow, I feel like I stepped off of the plane into another world... different language


Welcome to my World Dan. :D:D

Rodne Gold
02-23-2010, 11:09 AM
Do you grind your own TC single flute cutters Dave? We have found that some TC stock is better than others and we grind a specific way when using em for SS. We don't exactly halve them , leaving them slightly over halved , we also start our relief/back clearance nearer the cutting edge and take quite a bit off , our included angles for V cutters are wider and we never use tip widths less than .5mm and only use the best grade TC
I am also very conservative with plunge rates , finding most cutters break when entering the material. Apart from that , I use undiluted Diatsol cutting fluid flooding the plate , its water soluable and easy to clean off , Its a mission for me to use a constant flow of coolant. I was however considering one of those venturi air cooling thingys , but have never got round to it or tested one.

We have a great source for VERY high grade TC , and that is the PCB industry , they use 1/8" and 6mm shanked drill bits and when they break the much smaller/thinner drill section , they normally toss em. We offer em 50c for their broken bits , mostly SOLID tc and every 3 months we collect a coupla hundred and pay the guys "beer money"
We use HSS and coated end mill type cutters cos they are a lot cheaper than TC and unfortunately our cutter grinder can't make em.
In general , I avoid actually engraving SS , what we do is coat the SS with polyester vinyl , stick it in the laser and ablate the vinyl , sand blast it to clear any glue residue and etch in Ferric Chloride.
The only real issue we have is removing the polyester vinyl after as it sticks like crazy.

Dan Hintz
02-23-2010, 11:46 AM
The only real issue we have is removing the polyester vinyl after as it sticks like crazy.
I assume you just scrape with a razor blade to remove it rather than futz with trying to peel?

Rodne Gold
02-23-2010, 12:10 PM
We have tried everything barring burning it off - currently use a flat blade paint scraper - I think we need to find a better resist thats laser friendly. Heating it or soaking in solvent doesnt seem to make a difference.
I have tried various paints as resists , but the etchant is spayed at 40 deg c and tends to lift off lesser resists especially in the middle of small letters like A's or B's
The major issue is that there has to be NO residue at all on the etched portions (the lasered ones ) , even a fingerprint is a no no , so we have to sandblast to get to bare virgin metal or in the case of paint , we used to use a mild abraisive household cream rubbed with out fingertips to clear the aftermath of lasering.
There are other types of resist like photosensitive ones and screened ones , but both require printed artwork and exposure units , we also just use plain vinyl thats cut with our vinyl cutter , but that wont do any detailed work at all or small lettering.

Dave Johnson29
02-23-2010, 1:24 PM
Do you grind your own TC single flute cutters Dave?

Nope, I buy them as needed. They are usually for an old Swift engraver and about 2" long. I use a diamond wheel to score around the cutter about an inch from the tip then break them off so I can get them into the collet with only about 1/8" sticking out. Sounds a bit like your PCB drills.

I had not thought of using them, but then I don't do enough hard metal engraving. I do a fair amount in aluminum though but the Carbide D-cutters work fine for that.

I have a high-speed spindle that attaches to the quill of one the CNC mills and just use one of the standard fixture offsets for it. I can then use the flood coolant. The CNC mill is not a dedicated engraver so it is slower but there is virtually no limit to the materials I can engrave. Because the machine is extremely rigid plunging etc is no issue.

An old machinist's axiom, "I can make anything and if I don't have a machine to make something, I can first, make the machine. :D

Ian Rankin
02-27-2010, 9:02 AM
Hi All,
Thanks for all your help, I have been busy all week trying to plod through this stainless job. I finally have a finish I am happy with. I have moved down to a tip of 2.5mm The spindle speed is 30000rpm and a movement speed of 2"ips. I have changed the fill pattern to the S sweep for 2 passes of .2mm cut depth changing cutter after each pass. I then do a final reverse spiral pass of .1mm to finish. The reverse spiral pass seemed burn the cutter it went into the corners when it was doing a .2mm cut. Now for the problem of paint filling these 300mm high letters. I am pouring the paint in one letter at a time and scraping of with card but it is tricky. Any better suggestions.

Thanks again for help.

Ian Rankin

Rodne Gold
02-27-2010, 12:43 PM
Well , the flood fill and scrape clean method is the best , you can do the whole plate in one go , but large letters are tricky as you scoop the insides when cleaning.
The best is to let it all dry quite well , spread newspaper on a flat surface , moisten with methlated spirits , turn the plate upside down with painted surface on top of the meths moistend newspaper and with circular movements rub it around.
The reason to use methylated spirits is that it generally doesnt mar the glossy finish of the painted letters.
You have to balance out paint thickness and drying time , the paint has to be thick enough to cover the milling marks , often requires a few coats. We use undiluted auto duco to fill our stuff as its very durable , especially in harsher climatic conditions.

Ian Rankin
02-27-2010, 3:44 PM
Rodney,
I am using a thick cellulose car paint is that the same as Duco? The guys in the paint shop gave me a brushing additive which slows the drying and seems to help with the flow. I have cleaned of carefully and then rub with a coarse rubbing compound which tends to blend the machine marks and the dust that seems always appear from nowhere. I usually fill perhaps 2/3 times. These plates are 2100 x 600mm x 3mm stainless so the handling has been a problem. I have 3 out of the four complete and I keep looking that them and noticing small flaws. They are going in the middle of a large roundabout so when they are in position I'm sure no one will notice a speck of dust. If a 40 footer gets his braking wrong they will probably end up in the scrapheap anyway.
That shouldn't be the attitude but after the hassles I have had I will be glad to see them go out the door.

Regards
Ian Rankin