Need Help!- aluminium engaving yet again

[rusel]

Hi
Have been reading past thread on this and the feeds and speed vary from near nothing to hypersonic, Well I'am confused....
I keep getting a burr around the edge. The aluminium is 6061.
The attached was done with a 60 degree angle with a 0.2mm flat tip(10 x 60° Carbide PCB Engraving Bits CNC Router Tool #15 (eBay item 290527878007 end time 27-Feb-11 03:17:21 AEDST) : Industrial)
at 19800rpm, flood coolant, FR 30mm, two at 0.1mm per cut, one pass at 0.05mm total of 0.25mm
The centre logo had 3 passes at 0.084mm the one at 0.056mm total of 0.35mm same rpm and FR
Do I go fast FR or RPM or both?I feel I'm already going slow with FR
Deeper cut per pass?
What has worked for you.
Thanks for any help you can give.

Russell

[jeffrey001]

Look like there's run out on your spindle.

Measure run out with a dial indicator.

Find where the indicator move to the highest value.

Place the cutting edge of the tool toward this mark.

The cutting edge of the tool must always be where the run out is higher.

These tools are not the highest quality and very often are not centered.

Measure the diameter of the tool and also where the flat is, must be centered perfectly(half the diameter on the tool)

Just a though.

Jeff

[Superman]

Russ
The tool seems to not have a sharp enough cutting edge and is pushing the material out, not enough radial clearance in the point area ( common problem )

We do our engraving with similar tools, we call D bits ( single point vee cutters - you do have to have a knack to sharpen them accurately ), but are leaning to using off the shelf 1mm ball nose slotdrills

cutting data
@ S6000-8000 RPM
Z feed 100 mm/min
XY Feed 250 mm/min
DOC max 0.2mm ( depends on what finish you want )
coolant ON

I even use this data on steel
In a pinch, you could use a #2 HSS centre drill using the same data

[DMF_TomB]

......a sharp high rake cutter designed for aluminum does better on aluminum. dull or low rake cutters make bigger burrs.
......some use a ball endmill for engraving saying it helps lessen burrs.
......some take final cut at only 0.02mm to try to weaken burrs so they come off. this works better with ball endmills or conical tipped ones and does not help much with regular endmills. sometimes a blunt tip (shallow angle) and or larger ball endmill taking shallow cuts pushes burrs back down more than sideways and this helps somewhat with burrs.
......some try clear plastic tape over metal and engrave through it. sometimes chips and shavings can scratch a mirror finish and tape protects it. although peeling tape off is sometimes time consuming.
......a soft medium or fine surface conditioning abrasive disc at 10,000 rpm will take burrs off most things and smooth finish. surface conditioning discs are softer and leave less swirl marks and blend surface smoother than sandpaper discs. they are like a semi hard buffing wheel. they take little metal off but will blend or take off / blend stuff sticking up like burrs.
......some alloys make more burrs than others when engraving. basically if you turn it on a lathe and it likes to make long chips / ductile instead of chips breaking off short. try on a free machining Stainless. Some newer Stainless alloys are designed to machine as fast as low carbon steel and have short curly chips for easy lathe turning. look for an alloys that breaks off as shorter chips and is less ductile.

[rusel]

Hi
Thank for the replies. I'am going to work thought these and give you my results
jeffrey001
Did the measurement and the tool was out 180 degrees for cutting edge and run out so i rotated tool. It was better but still had a burr
Measured the tool dia was 3.17 and the flat was 1.62 according to you it should be 1.585
Tried one with a flat of 1.55mm finish cut of 0.05mm still have a burr

Superman
I do not have any way of reshaping tools
Will look at 1mm ball mill. Definitional like the DOC and Feed rates

DMF_TomB
A great amount of info thanks
I can not us a surface clean up as the surface is at a mill finish

Thank for the info but I will take more info

Russell

[Markwind]

I think the cutter has a lot to do with it, even the slight bit of runout with a v-type bit is trouble,

I came across this guy engraving aluminum, he uses a ball nose, which I believe is more forgiving for engraving detail, then V-type bits
Ruckus Frame Blocks



you can see his cnc router is made from wood, with probably tons of play, and I am sure the rotary tool has runout, yet he appears to get a good finish
with ball nose CNC Router

[jeffrey001]

Just some more information.

Harvey Tool > Carbide Miniature End Mills, Diamond End Mills, Carbide Long Flute End Mills, Carbide Long Reach End Mills

Engraving Fact Sheets

http://www.signsupply.com/PDF/Roland.../Tools_FAQ.pdf


I would try to buy a high quality engraving tool.

You will get only one for the same price but result will probably be much better.

Jeff

[rusel]

Hi
Many thanks for all the advice. I did lean much, main one is that cheap tools are expensive in the long run.
I end up using a ball mill see attached photo

Again many thanks

[Superman]

Use a smaller ballnose to get better definition of the characters, say half the size of what you used in the photo

HINT
We machine alum daily, sometimes we will rub a face, after machining, with "wet & dry" emery paper 200-400 grit, another item you cam use to finish off is a "scouring pad" or "scotch-brite" to get rid of the fine burrs that are often left behind, but is not good for heavier burrs

[w_bloemen]

We always engrave aluminium with V-type bits, its very important that the cutting edge is just over the middel of the diameter. It`s also important that the rest of the edge is free. It sometimes helps if you run the program again but than 0.01mm deeper.
What coolant do you use? Aluminium tends to stick, try to lubricate with alcohol

kind regards