# Engraving tips for hobby Mill? V-Tip, Ball top, what have you used?



## countryguy (Jul 20, 2014)

Uggg.... About my 30th Question this month!  So much to learn!  Thanks for the review if you are reading this. You're all wonderful here. 

Engraving (pic below)  was done w .125 on a DXF i did today in Draftshight to DolphinCAM V12.  about 3500 RPM at 5ipm.  I do not have the time to go build and attach a HS router adapter to mount on the quill... But that will come in time.   So for now, Which bits have you used in your Mill. 

The process I have needs a little clean up and I need to get some better engraving tips for brass and steel work I think.  That said,  Do I just look and buy the usual HSS / Carbide 1/8 shank stuff that Dremel and off-brand's sell?  (link below).  

There are:   Ball End Mills, V-cutter engravers, Ball head engravers, and the diamond tipped , and finally the stone type tops.     Hmmmm    I have good results w/ the 1/8" so I am thinking get those again in 1/16 ball nose Mill" and try the V-cutter in HSS?          you favorites and/or Suggestions welcome. 


My first attempt  but is similar to my 2D plasma work, so no big deal really.  3.5" across.
. Need to play and experiment a bit.  Looking for your ideas and input. 

Note-  I have searched and read via the "Similar threads"  and did searches on this. Still reviewing. I do search often as well in the archives.  Great stuff in there if you take the time to search it.  ;-)   Not just asking w/o looking ;-) 
CG. 




http://www.amazon.com/Engraving-Cut...1405895093&sr=8-1&keywords=1/16+engraving+tip

- - - Updated - - -

Here is a seemingly OK priced starter kit in what I was thinking I need?  
http://www.2linc.com/engraving_tools_starter_kits.htm

Hey.... this is a cool site.  Even have Feeds and Speeds.   Now if someone sells a quick spindle/quill to router adapter , I think this may be easy after all.  Passing along what I find cool! 
CG


----------



## countryguy (Jul 21, 2014)

So I ended up ordering a coated and non-coated carbide ball mill .063 cutter w/ 1/8" shank via Amazon.  Vendor is Niagra cutter.   $12 for non-coated and $14 for the coated.    Should be here in just a few days.   

Will post up picks later if anyone is interested.  CG.


----------



## Robert LaLonde (Jul 21, 2014)

countryguy said:


> So I ended up ordering a coated and non-coated carbide ball mill .063 cutter w/ 1/8" shank via Amazon.  Vendor is Niagra cutter.   $12 for non-coated and $14 for the coated.    Should be here in just a few days.
> 
> Will post up picks later if anyone is interested.  CG.



Most of the aluminum nitride coatings are actually more likely to chip weld to aluminum.  TiN, AlTiN, TiAlN, etc.  For the most part flood coolant and bright carbide has worked the best for me.  I have heard good things about Diamond, DLC, and ZrN coatings for aluminum work with ZrN probably being the most often mentioned, but I just use uncoated.  I do a lot of high speed small cutter work in aluminum.  Down to 1/16 routinely, and occassionally down to 1/32.  It pretty hard to beat a water soluble lube/coolant like TRIM for aluminum work. Under about 3/32 I stick with 2 flute, and mostly use 3 flute for 1/8 and larger.  Chip clearance is an issue with aluminum milling.  Sometimes its hard to find the size you want in the smaller mills in 2 flute and you are forced to buy 4 flute.  If you do then take a lighter cut and blast those chips out of there with flood or atleast an air blast.  

There is no substitute for a light (not to light (usually about 0.003")) finish pass in aluminum with a sharp cutter for a good quality finish.  No matter what you do you are likely to get some edge tearing and burrs on the edges of slot cuts that might need to be polished off. I think 0.001 is too light as you are fighting the work hardened surface of the previous pass and will very quickly dull your cutter.  

~~ BASED ON SLOTTING (which is what you are doing) ~~

In your original post you do not say what your depth of cut is, but a quick check with FS Wizard gives the following with 6061-T6:

Cutter:  .125, 2 Flute, 1.25 stickout, Carbide, Standard Geometry,

RPM:  3500
WOC: Slotting
DOC:  0.004"
FEED: 7.09 IPM

That being said I have found from experience that FS Wizard assumes a very rigid machine and and produces a result more consistent with high speed machining, not high finish quality.  A slower feed will produce a better finish quality (usually) and a shorter tool life.  

Your 5-IPM feed is probably fine, but you may want to consider your depth of cut.  I found that the max I could reasonabley do with a .125 ball nose was about 0.005" before I learned about calculators like FS Wizard.  

When you drop down to .0625 ball mills you will find your feed rate and DOC really needs to drop with your limited speed spindle.  2.95 & .003 for a quick check with FS Wizard.  Maybe a little slower with your machine and/or a good finish quality.  

Making a quill clamp or other mount for an off side high speed spindle of some kind is a must for efficient material removal rates with tiny cutters. Depending on how often you plan to do this type of work their are a number of approaches.  

Rotary handpiece: 15K-18K RPM - Harbor Fright have less runout than the lower price Foredoms, but Foredom also makes a more expensive tighter tolerance one.  I have Foredom handpieces of low and high tolerance hanging from my Harbor Fright drive motors, but I no longer use them as CNC spindles.   

Wood router:  8K-34K RPM - A trim router or a mid size router will work for occassional work, but if you run them continuously for hours you will burn them up quicker than you might think.  A full size continuous duty 3+ HP router may last longer, but I would still consider them occassional duty.  Also flood coolant could cause a shock hazard.  I do occassional "nearly dry" (hand applied cutting oil and air blast) aluminum machining on my CNC gantry router with a trim router.  Mostly it gets used for wood though.  

3 Phase Spindle and VFD:  8K-24K RPM - Air cooled or water cooled.  The water cooled ones from more reputable vendors work fairly well. I have never used an air cooled one because I planned all along to use flood coolant for aluminum milling with them at high speed.  I have a 0.8Kw 110V unit on my Taig as its main permanent spindle, and I have 2.2Kw 220V unit on one of my larger mills as its main permanent spindle. 

Dremel and Rotozip are no options in my opinion.  Both their main spindle and their hand peices have horrible runout and slop in my opinion.  They are sloppy to make them hold up longer, and work fine as hand held tools, but are not suitable for use as a precision mounted tool.  

Making a mount is not a huge deal.  I bet you can do it in half a day or less.  Ok, maybe a day the first time you tackle and plan a project like that.


----------



## DMS (Jul 21, 2014)

Updates are welcome. I didn't post a response initially because I really haven't done any engraving except for one PC board I made. I build an auxiliary spindle out of a pencil grinder. The cutter was a single edge conical type cutter (I believe it was an Onsrud). Worked pretty well at 50k rpm. That is one thing I have heard about engraving; you want as much speed as you can throw at it. The clamp for the pencil grinder was more or less a 1 day project.


----------



## Robert LaLonde (Jul 21, 2014)

DMS said:


> Updates are welcome. I didn't post a response initially because I really haven't done any engraving except for one PC board I made. I build an auxiliary spindle out of a pencil grinder. The cutter was a single edge conical type cutter (I believe it was an Onsrud). Worked pretty well at 50k rpm. That is one thing I have heard about engraving; you want as much speed as you can throw at it. The clamp for the pencil grinder was more or less a 1 day project.



Very good point about the pencil grinder.  I assume air?  I have not used one, and the only reason I didn't mention them is because most of them that I have seen are not rated for continuous duty.  At the very least if I was to use one I would add a water separator, desiccant filter, and an air tool oiler to feed it directly.  I have heard of people getting very good results with them for short jobs.  

There are also high speed, high precision, purpose built air spindles, but the price is pretty steep for a hobby machinist.


----------



## DMS (Jul 21, 2014)

The unit I had came with an inline oiler. It was a cheap ($19) unit from Horrible Fright. It was a small board, and I didn't do any area clearing, so it only took about 10 or 20 mins. Yes, air powered. The nice thing about engraving spindles is they don't need much torque, just a bunch of speed. I have seen people use Dremel type tools as well, but I have lost most of my respect for the brand in recent years. The HF pencil grinders are cheap enough for an experiment, and bearings seem OK.


----------



## JimDawson (Jul 21, 2014)

My pencil grinder from HF works good also, and it's cheap.  The bearings seem OK.  Here is what I did with it. http://www.hobby-machinist.com/showthread.php?t=23186&p=205311&viewfull=1#post205311


----------



## Bishop (Jul 21, 2014)

I added a pencil grinder to my little X2 with good results so far.


----------



## countryguy (Jul 21, 2014)

Bob, thank you for the very detailed reply!  CG. 




Bob La Londe said:


> Most of the aluminum nitride coatings are actually more likely to chip weld to aluminum.  TiN, AlTiN, TiAlN, etc.  For the most part flood coolant and bright carbide has worked the best for me.  I have heard good things about Diamond, DLC, and ZrN coatings for aluminum work with ZrN probably being the most often mentioned, but I just use uncoated.  I do a lot of high speed small cutter work in aluminum.  Down to 1/16 routinely, and occassionally down to 1/32.  It pretty hard to beat a water soluble lube/coolant like TRIM for aluminum work. Under about 3/32 I stick with 2 flute, and mostly use 3 flute for 1/8 and larger.  Chip clearance is an issue with aluminum milling.  Sometimes its hard to find the size you want in the smaller mills in 2 flute and you are forced to buy 4 flute.  If you do then take a lighter cut and blast those chips out of there with flood or atleast an air blast.
> 
> There is no substitute for a light (not to light (usually about 0.003")) finish pass in aluminum with a sharp cutter for a good quality finish.  No matter what you do you are likely to get some edge tearing and burrs on the edges of slot cuts that might need to be polished off. I think 0.001 is too light as you are fighting the work hardened surface of the previous pass and will very quickly dull your cutter.
> 
> ...



- - - Updated - - -

Here are about a dozen or so from non HF Vendors.  My hf is a hike for me.   I am addicted to amazon Prime.  Everything in two days and no driving 

http://www.amazon.com/s/ref=nb_sb_noss_1?url=search-alias%3Daps&field-keywords=Pencil+air+grinder


----------

