# First time using mini-mill



## jhanko (Jan 19, 2009)

Hey guys, long time-no see. I recently made some titanium Nitecore D10's. They turned out great, but I'd like to make a couple of them really special. I ordered some 1.55mm x 5mm trit from Bart that I want to put in these. The area that I want to put them in has ~.080" wall, so I'm fine there. I got a mini-mill that mounts to my lathe. I wish I would have got a seperate machine instead. It seem to always be in the way when I'm working on the lathe. Oh well, too late now. I also ordered some .0625", 4 flute carbide end mills. I never used a mill before and was wondering the best way to cut these slots. Plunge to desired depth, then cut to length or make several small cuts? How can I get all the slots the same length? Any way to divide the slots with equal spacing without buying a rotary table or something like that? How do I chamfer the edges of the slots when I'm done? Sorry for so many questions, but I nervous about destroying any of these. I photoshop'd a picture of what I want to do. Thanks!


----------



## G1K (Jan 19, 2009)

To get the slots evenly spaced (3, 4, or 6 slots) you can get a collet block set. Usually they contain a square one and a hex one. If the part you have will fit inside a 5c collet your golden, 5c collets are cheap and so are the collet blocks.

Here's an example (no affiliation)
http://www.penntoolco.com/catalog/products/products.cfm?categoryID=836

I've seen these much cheaper on ebay, but not sure of the quality.

FWIW, you won't be able to get 90 degree inside corners like the rendition above, the slots will have the radius of the cutter in each corner, or 1/16".

With a 1/16 endmill, you want to take shallow cuts and you also want the cutter RPM fairly high. Make sure the feed direction for the rectangle is opposite the rotation of the cutter, you don't want to climb cut, it may deflect the small cutter and break it. Keep the cutter and slot free of chips and keep it cool. 

If it's a center cutting end mill you can plunge with it, otherwise drill a small pilot hole somewhere in the slot location as a starting point.

As for controlling lenght, use the handle scales or a DRO if so equipped. Maybe a picture or two of you lathe/mill?

R


----------



## jhanko (Jan 19, 2009)

G1K said:


> To get the slots evenly spaced (3, 4, or 6 slots) you can get a collet block set.


Those are neat. Never seen those before. Sounds like a cheap solution.



> FWIW, you won't be able to get 90 degree inside corners like the rendition above, the slots will have the radius of the cutter in each corner, or 1/16".



I was aware of that.



> With a 1/16 endmill, you want to take shallow cuts and you also want the cutter RPM fairly high. Make sure the feed direction for the rectangle is opposite the rotation of the cutter, you don't want to climb cut, it may deflect the small cutter and break it.



Well, I think I screwed up then. I ordered end mills that are .002" larger than the trit OD. I though I could cut both sides of the slot at the same time.



> If it's a center cutting end mill you can plunge with it, otherwise drill a small pilot hole somewhere in the slot location as a starting point.



That I can handle...



> As for controlling lenght, use the handle scales or a DRO if so equipped.



I don't have DRO's and my handles have enough backlash to cause considerable inconsistancies



> Maybe a picture or two of you lathe/mill?



I'll get one up in a few minutes.

Thanks for the info. I love learning!


----------



## G1K (Jan 19, 2009)

JHanko said:


> Well, I think I screwed up then. I ordered end mills that are .002" larger than the trit OD. I though I could cut both sides of the slot at the same time.



You can do both at the same time, just be careful of the end mill loading up and the tool deflection. Go slow with the feeds and keep it cool and well lubricated.

R


----------



## gadget_lover (Jan 19, 2009)

A few other thoughts...

1) You have the mill head mounted on the lathe? There's a good chance you can use the lathe spindle as an indexer by chucking the light in the lathe, then spin the chuck X number of teeth, mark the cut, go onto the next.


2) If the light is mounted on the table, then you can clamp stops to the ways to limit the travel. This will assure all are the same length. The exact length is not as important as the fact that they look the same length.

3) Add a stop the vise that will hold your light so that it goes back to the same relative position each time it is moved.

4) based on the size of the bit (1/16 inches = 1.5875 millimeters) and the width of the trit vials, (1.55mm), you will only have to move the light in one direction. This means you will have full engagement of the cutters so climb milling is not an issue.

5) Use a collet designed for small cutters. A drill chuck is likely to have a lot of runout (many thousandths of an inch) which may cause the carbide to shatter.

6) Check with one of the folks here about the right RPM for 1/16 inch carbide in titanium. You really need to get close to the right speed, probably above 2000 rpm.

7) If only two vials are visble at a time, then any deviation in the spacing is not apparent. I think you can do 5 vials and not notice if they are off.

8) make some test pieces to practice on. A groove 0.061 (1.55mm) deep in a .080 thick curved wall may give you a surprise, depending on the curve, how much deeper you want to go to protect the vial, etc. I'm no good with trigonometry, but I can envision the arc on the outside, the arc on the inside and the width of the cut. That image says that to get the vial below the surface of the curve you will be cutting deeper than .061, and that the thickness at the outsides of that 1/16 wide slot will be less than .080.

8) Use a good indicator, center finder, etc to make sure you are centered over the tube. You can use the 6 inch ruler trick for that.


Good luck

Daniel


----------



## jhanko (Jan 19, 2009)

Wow, great info here! Keep it coming!



gadget_lover said:


> 1) You have the mill head mounted on the lathe? There's a good chance you can use the lathe spindle as an indexer by chucking the light in the lathe.



When I bought the mill, I thought it mounted to the carriage and wanted to do that exact thing. When it arrived, I found it mounted to the bed.:shakehead




> If the light is mounted on the table, then you can clamp stops to the ways to limit the travel.



That's a good idea. I should be able to come up with some simple stops.




> Add a stop the vise that will hold your light so that it goes back to the same relative position each time it is moved.



Another good idea.



> Based on the size of the bit (1/16 inches = 1.5875 millimeters) and the width of the trit vials, (1.55mm), you will only have to move the light in one direction. This means you will have full engagement of the cutters so climb milling is not an issue.



That's great news!



> Use a collet designed for small cutters. A drill chuck is likely to have a lot of runout (many thousandths of an inch) which may cause the carbide to shatter.



Unfortunately, I'm stuck with the chuck. The good news is that I have checked the runout repeatedly at <.001".



> Check with one of the folks here about the right RPM for 1/16 inch carbide in titanium. You really need to get close to the right speed, probably above 2000 rpm.



My mill goes from 0-2500 rpm, so I'm good there...



> If only two vials are visble at a time, then any deviation in the spacing is not apparent. I think you can do 5 vials and not notice if they are off.



That's good news, but I think I'm too anal to accept the deviation. It would drive me crazy...



> Make some test pieces to practice on. A groove 0.061 (1.55mm) deep in a .080 thick curved wall may give you a surprise, depending on the curve, how much deeper you want to go to protect the vial, etc. I'm no good with trigonometry, but I can envision the arc on the outside, the arc on the inside and the width of the cut. That image says that to get the vial below the surface of the curve you will be cutting deeper than .061, and that the thickness at the outsides of that 1/16 wide slot will be less than .080.



Good info...



> Use a good indicator, center finder, etc to make sure you are centered over the tube. You can use the 6 inch ruler trick for that.



Dont mean to sound stupid, but what is the "6 inch ruler trick"?



> Good luck.



Thanks, I'm going to need it!

Here's a picture of my rig...


----------



## StrikerDown (Jan 19, 2009)

If the chuck it held in the spindle with a taper like a MT-2 you can get holders that have an MT-2 arbor. If that works it should be more secure and accurate for the small end mill.

Lower the spindle and see if there is a slot through the spindle. If there is your mill drill probably came with a drift (tapered wedge) that is used to remove the the tapered arbor from the spindle.


----------



## jhanko (Jan 19, 2009)

StrikerDown said:


> If the chuck it held in the spindle with a taper like a MT-2 you can get holders that have an MT-2 arbor. If that works it should be more secure and accurate for the small end mill.
> 
> Lower the spindle and see if there is a slot through the spindle. If there is your mill drill probably came with a drift (tapered wedge) that is used to remove the the tapered arbor from the spindle.



The mill does have an MT-2 taper with a drawbar to hold it in place. So, I should look for a 1/8" (the end mill shank size) holder with an MT-2 drawbar arbor? It doesn't sound easy to find or cheap...


----------



## gadget_lover (Jan 19, 2009)

The ruler trick is the same one you use to get the lathe tool's tip exactly on center.


Put a sharp tool in the mill chuck. Center it over the tube you are going to work on. Set a thin stiff piece of metal on the tube. I use a 6 inch metal ruler.

When you pinch the ruler between the sharp point and the circumference of the tube, it will tilt left or right unless the tip is right over the center.

The first picture shows the tip too far to the right. The second is fairly well centered.


----------



## StrikerDown (Jan 19, 2009)

JHanko said:


> The mill does have an MT-2 taper with a drawbar to hold it in place. So, I should look for a 1/8" (the end mill shank size) holder with an MT-2 drawbar arbor? It doesn't sound easy to find or cheap...




I did a quick search on the Griz website But you should check around:
$16.
http://www.grizzly.com/catalog/2009/Main/616

Not the problem at hand, just an observation:
That is a large looking drill chuck in your tail stock! much bigger than the mill/drill Almost looks as big as the 3 jaw! Just wondering if it crowds you for space and if you can you use the chuck out of the Mill/drill to gain length between tail and head?


----------



## jhanko (Jan 19, 2009)

gadget_lover said:


> The ruler trick is the same one you use to get the lathe tool's tip exactly on center.
> 
> 
> Put a sharp tool in the mill chuck. Center it over the tube you are going to work on. Set a thin stiff piece of metal on the tube. I use a 6 inch metal ruler.
> ...



Awsome trick! Thank you...

One more thing, Is this what I should be looking for? I'd have to find them with metric drawbar threads though...
http://cgi.ebay.com/7-PC-Morse-Tape...ItemQQimsxZ20090117?IMSfp=TL090117114008r9374


----------



## gadget_lover (Jan 19, 2009)

Your mill looks a lot like the head from the micro-mill that I have. 






You can get 1/8 inch MT2 collets all over the place. LMS has them, so does Enco, etc. 

If you really have only .001 runout you will be OK, but beware of the endmill slipping. Check it between cuts to make sure its still the same height.


----------



## StrikerDown (Jan 19, 2009)

Gadget,

This is how I know if my cutting tool is above, on, or below center on the lathe.
Funny I never thought to use this trick on drilling round work. Thanks!:thumbsup:


----------



## gadget_lover (Jan 19, 2009)

JHanko said:


> Awsome trick! Thank you...
> 
> One more thing, Is this what I should be looking for? I'd have to find them with metric drawbar threads though...
> http://cgi.ebay.com/7-PC-Morse-Tape...ItemQQimsxZ20090117?IMSfp=TL090117114008r9374



Yes, that is what you want. The collet goes most of the way into the spindle, so you lose almost no room between the table and the cutting tool... other than the length of the tool.

Check your drawbar to see what thread you actually have. I have some collets that use a 3/8-16 thread and some that are metric, so I just bought a foot of all-thread and cut it to length.

Daniel


----------



## jhanko (Jan 19, 2009)

gadget_lover said:


> Your mill looks a lot like the head from the micro-mill that I have.



Yep, exact same mill. Mine just came with a cast L-bracket to mount it to the bed instead of a table. How do you like it? Haven't used mine yet...


----------



## jhanko (Jan 19, 2009)

gadget_lover said:


> I have some collets that use a 3/8-16 thread and some that are metric, so I just bought a foot of all-thread and cut it to length.
> 
> Daniel



Great idea! Never thought of that trick either... Too much information. My head is about to explode!


----------



## StrikerDown (Jan 19, 2009)

StrikerDown said:


> I did a quick search on the Griz website But you should check around:
> $16.
> http://www.grizzly.com/catalog/2009/Main/616
> 
> ...




OOps I just noticed the 1/8 shank size, do you already have the end mill?

Drill chucks really aren't designed for much side loading but that is a small end mill that would break before you applied much side load... Give it a try on a sample work piece and go for it if it works to your satisfaction. Make sure to check the run out on the tool shank.

PS: The collets look like a much better idea!


----------



## gadget_lover (Jan 19, 2009)

JHanko said:


> Yep, exact same mill. Mine just came with a cast L-bracket to mount it to the bed instead of a table. How do you like it? Haven't used mine yet...



It is remarkably usable. I've had one for 3 years now, and I've done all sorts of things with it. I used it just last night to make a few standoffs for the DRO I'm adding to my bigger mill. 

You need to stay within it's envelope. No big (> 3/4 inch) end mills, no 3 inch boring bars, no .250 deep cuts in a single pass. I've milled trit pockets in titanium with it. 

BTW, you can get the collets separately from LMS in metric or imperial thread.
http://littlemachineshop.com/products/product_view.php?ProductID=1745&category=

Daniel


----------



## jhanko (Jan 19, 2009)

Ok, looks like I got everything covered except how to hold the light. I've been looking at collet blocks and don't think they will work. I think I will need to hold the light in the section with the smaller diameter. Is there any way to get this to work? My other option is to cut the trit slots before I turn down that section, but I want to mill a couple of light that are already complete...


----------



## G1K (Jan 19, 2009)

The light looks like it has a threaded connection between where you want to mill and the head? Make a threaded hole in something that you can grip in your 3 jaw chuck. Screw the light half into that, and your set. For support on the other end, use a live center, or even just some material between the light and the compound, since the light wont be spinning.


R


----------



## jhanko (Jan 19, 2009)

G1K said:


> The light looks like it has a threaded connection between where you want to mill and the head? Make a threaded hole in something that you can grip in your 3 jaw chuck. Screw the light half into that, and your set. For support on the other end, use a live center, or even just some material between the light and the compound, since the light wont be spinning.
> 
> 
> R



I was thinking of something like that, but was worried that vibration from the milling process would constantly try unscrewing the parts.


----------



## gadget_lover (Jan 19, 2009)

Workholding is the fun part of milling. There are a million different fixtures that you can buy to hold the part you are working on. I only have a few dozen of them.

Typically , you would hold a cylinder in a V-block. 

I see what appear to be to be T-slots on the compound slide. That would be your table. 

Typically a T-nut in the slot would hold a clamp that secures the piece to the table. There are many sizes of t-nuts. 

Keep in mind that you are using enough energy to slice through metal. If there is any movement at all it can knock your piece off center, cause it to bind and rip it from the clamps. Sound like fun? Like using the chuck on the lathe, the light needs to be secure enough that there is no chance of it coming lose, but not so tight that it deforms the piece.

Examples of clamping kits.... http://littlemachineshop.com/products/product_category.php?category=11

You can also use a small vice, like a 2 or 3 inch screw-less toolmaker's vise.
Example of vise: http://littlemachineshop.com/products/product_view.php?ProductID=1590&category=3

I can post a picture of a similar setup if you need it.

Daniel


----------



## jhanko (Jan 19, 2009)

gadget_lover said:


> I see what appear to be to be T-slots on the compound slide. That would be your table.



Actually, I'll remove the compound slide and use the cross slide as the table. Much larger and more rigid.



> You can also use a small vice, like a 2 or 3 inch screw-less toolmaker's vise.



Yeah, I definitely see a need for one of those.

I would love to get this, but can't afford it.
http://littlemachineshop.com/products/product_view.php?ProductID=1702&category=1034788869

I found another one for over $100 less. Looks like the same thing with different paint.
http://www.shars.com/products/view/419/4quot_Tilting_Index_Space


----------



## cmacclel (Jan 20, 2009)

There is many great ideas here but I would suggest if you really want these done and for them to look good I would see if a local shop would help you out. Milling titanium on that small of a machine with a 1/16th end mill may not be fun. If anything is loose you pretty much can kiss the endmill and possible the part goodbye.

Also your first journey into milling should not be with the most difficult material to machine 

Send TranquilityBase an E-Mail he does these all the time on his machine.

Mac


----------



## jhanko (Jan 20, 2009)

Well, something finally went right for me for once. It turns out that the store that had that index spacer was 1 hour from my house. I just got home from there. I ended up buying the spacer and 7 piece MT2 collet set. I am amazed at this spacer. Much heavier than I thought. The quality of this thing blows me away. Very well constructed with nice, laser engraved scales. Time to clean it up and learn to use it. I may paint it. It's very ugly! Now that I think about it, with this mounted on my cross slide table, I really don't need a mill at all. I could probably do what I want with the tools mounted in the lathe chuck....

Jeff


----------



## Fred S (Jan 20, 2009)

If you mount that indexing head on the cross-slide with the jaws of the indexing head facing toward you, you will be all set; IF you can get your end mill sticking out far enough from the lathe chuck jaws. watch for deflection of the light body if the jaws of the indexing head chuck are very far from the proposed cutting area. You can still mount the indexing head on the carraige and use the mill, and it may work better for spindle access


----------



## jhanko (Jan 20, 2009)

Fred S said:


> If you mount that indexing head on the cross-slide with the jaws of the indexing head facing toward you, you will be all set; IF you can get your end mill sticking out far enough from the lathe chuck jaws. watch for deflection of the light body if the jaws of the indexing head chuck are very far from the proposed cutting area. You can still mount the indexing head on the carraige and use the mill, and it may work better for spindle access



I mounted it to the cross slide with the jaws facing the lathe chuck. I have all the room I'll ever need. :twothumbs Man, I love this thing already! The piece in the picture is just some scrap I was practicing on...


----------



## TranquillityBase (Jan 20, 2009)

You shouldn't have any problems milling trit slots with that machine...

Ask away, I'll answer, and with photos if you need them 

I'll edit this post, and let you know what cutter I used...Gotta go to the shop BRB...

*EDIT: 1/16" HSS END MILL 2 FLUTE STUB DBL BALL*

*BTW, sweet little rotary head you have :twothumbs*


----------



## jhanko (Jan 20, 2009)

TranquillityBase said:


> You shouldn't have any problems milling trit slots with that machine...
> 
> Ask away, I'll answer and with photos if you need them



I only have 2 questions left, I think... First, what RPM do you recommend for a 1/16" end mill on titanium? Second, what's the best way to clean up the sharp edge when finished? I was thinking a slight chamfer with a carbide countersink.. Thanks!


----------



## TranquillityBase (Jan 20, 2009)

I use 850 RPM, and just some cutting oil...Usually just one big drop of cutting oil.

If the cutter is sharp there won't be any burr...


----------



## gadget_lover (Jan 20, 2009)

I have no doubt that it can be done with Jeff's equipment. How do I know???

https://www.candlepowerforums.com/posts/2670315&postcount=19




Daniel


----------



## jhanko (Jan 21, 2009)

TranquillityBase said:


> I use 850 RPM, and just some cutting oil...Usually just one big drop of cutting oil.
> 
> If the cutter is sharp there won't be any burr...



OK, thanks!



gadget_lover said:


> I have no doubt that it can be done with Jeff's equipment. How do I know???
> 
> https://www.candlepowerforums.com/posts/2670315&postcount=19
> 
> ...



Nice! Did you get those small end mills on Ebay? I see them there all the time real cheap, but didn't get them because I was concerned they would be weak with that long flute length. Do you break alot of them? These are the ones I ordered. Item # 16106250. I just wish they would get here...


----------



## StrikerDown (Jan 21, 2009)

Hey Gadget, 

Besides keeping wine in the bottle, what is the wine cork for?


----------



## gadget_lover (Jan 21, 2009)

YOu WOULD notice that!


The owner of the bezel sent the tritium vial taped to a little pocket in the end of the cork. Sort of like natural bubble wrap.

I used very light pressure and hiked the speed all the way up. I don't recall where I got the bits. I tend to find things and say to myself "Hey, I might need that some day!" I might have bought them at Harbor Freight, a local ham radio club swap meet or at a rock-hound / jewelry festival. I can't quite recall.

Daniel


----------



## StrikerDown (Jan 22, 2009)

gadget_lover said:


> YOu WOULD notice that!
> 
> 
> The owner of the bezel sent the tritium vial taped to a little pocket in the end of the cork. Sort of like natural bubble wrap.
> Daniel


 
Good... I was about to call Mothers Against Drunk Drilling on you.


----------



## Oznog (Jan 22, 2009)

JHanko said:


> OK, thanks!
> 
> Nice! Did you get those small end mills on Ebay? I see them there all the time real cheap, but didn't get them because I was concerned they would be weak with that long flute length. Do you break alot of them? These are the ones I ordered. Item # 16106250. I just wish they would get here...



Those in the case on the milling table in his pic look like the ones from Harbor Freight. They're drills or reamers, and at $9 for 20 random and possibly mislabeled sizes, are a great deal on drills! But they're NOT cutters.

It's hard to make out what he's got on the mill, but it looks like a carbide diamond burr or something similar intended for cutting fiberglass FR4 PC boards and plastics. 

Carbide Plus is a REALLY excellent eBay vendor drillman1:
http://stores.ebay.com/CARBIDE-PLUS
was gonna buy a bunch then realized he's in Georgetown, Tx like 10 miles from here. I just drove up and bought a big array of milling bits for a VERY reasonable sum. Plus he's just a super cool knowledgeable guy.

I'd really expect the 2-flute endmill to be best:
http://cgi.ebay.com/1-8-stub-length...25260QQcmdZViewItemQQ_trksidZp1742.m153.l1262
I've done a bit of CNC milling work with these and a bunch of his other stuff already and have been really impressed.


----------



## modamag (Jan 22, 2009)

Just another bit of info from my limited experience.

I use 3/32" or 2mm endmill and single pass.

I recommend your cut to be the following for you MiniMill.
Cut depth - 0.010" and SLOW feed rate 
Final Depth - 0.080" - 0.090"
Final Length of Cut - 0.205" (5.2 mm)

Use ALOT of coolant.

Get a 1/8" MT2 collet because from 1/8" standard shank will expose you to all different size of cutters.

Shove the bit up as high as you can in the collet.

And lastly, PRACTICE on a scrap piece of Ti 6/4 or SS316 first.
Although, I think your nightcore is CP grade, but it's best to practice on the harder stuff to be sure. Worst case scenario you'll bust couple endmills @ < $10/each. It's still better than ruining your $$$ light.


----------



## jhanko (Feb 2, 2009)

I just wanted to say thanks to all that took the time to help and offer advice. The end mills finally arrived today. I practiced on some aluminum first, which got old in about 5 minutes. I chucked up some 6AL-4V and cut a test slot. It went alot easier than I expected. All I need to do is make up a couple carriage stops, as you can see I made the slot too long. Did I mention these mills are SHARP! I just barely touched it...


----------



## TranquillityBase (Feb 2, 2009)

Nice! :thumbsup:

 Be careful


----------



## precisionworks (Feb 2, 2009)

Very nice, Jeff:twothumbs



> Didi I mention these mills are SHARP!


My worst cuts always happen when trying to extract an end mill or twist drill from a collet. The flutes on a new (or newly sharpened) tool are like razors. Then you end up bleeding all over the table, vise & work for half an hour:mecry:


----------



## gadget_lover (Feb 3, 2009)

Nice work Jeff.

If you are going to repeat cuts, a stop for the vice (so the work goes back in the same place) and stops for the table (so it goes the same distance each time) are great time savers.

Sorry about the cut. I did not think to warn you. The glancing touch as you reach beyond the spindle is what catches me. I take a medication that makes my blood 'slicker' so every scratch bleeds like that. 

I put blood, sweat or tears into every project. The blood is pretty much guaranteed. The sweat and tears depend on the luck of the day.

Daniel


----------



## jhanko (Feb 3, 2009)

Thanks! These things are razor sharp for sure. The mill wasn't running when it happened. I reached in to adjust the work and pulled out with a bloody hand. I honestly didn't even feel it. One more thing: I cut down to a depth of .072". With a straight edge across slots length, I have ~.010" clearance to the vial. Across the width, ~.005". Is this safe enough or should I bury it more?


----------



## gadget_lover (Feb 3, 2009)

JHanko said:


> Thanks! These things are razor sharp for sure. The mill wasn't running when it happened. I reached in to adjust the work and pulled out with a bloody hand. I honestly didn't even feel it. One more thing: I cut down to a depth of .072". With a straight edge across slots length, I have ~.010" clearance to the vial. Across the width, ~.005". Is this safe enough or should I bury it more?



I can't say for sure, but .010 seems like enough if you will be filling it with epoxy. The light will not normally deform that far unless that exact point is the only one hitting something.

But one of the more experienced tritters should chime in.

Daniel


----------



## TranquillityBase (Feb 3, 2009)

That's about the same depth I cut slots for trit. .070" ~ .075"


----------



## TranquillityBase (Feb 3, 2009)

> Oznog said:
> 
> 
> > Those in the case on the milling table in his pic look like the ones from Harbor Freight. They're drills or reamers, and at $9 for 20 random and possibly mislabeled sizes, are a great deal on drills! But they're NOT cutters.
> ...


----------



## griff (Feb 3, 2009)

It looks like my little light need a TRIT:devil:




TranquillityBase said:


> You shouldn't have any problems milling trit slots with that machine...
> 
> Ask away, I'll answer, and with photos if you need them
> 
> ...


----------



## Oznog (Feb 3, 2009)

TranquillityBase said:


> > Carbide drills for drilling curcuit boards. Harbor Freight is correct...Excellent deal for a grab bag of tiny carbide drills :twothumbs
> 
> 
> But do heed my warning- I have some with clearly mislabeled collars. Measure first.


----------



## mdocod (Feb 4, 2009)

I'm probably a little late on this:

http://www.lathemaster.com/ROUNDBARCENTERFINDER.htm

but that may be handy


----------



## precisionworks (Feb 4, 2009)

> that may be handy


Those are meant for finding the approximate center of a part, where you don't need to be really close. To find center +/- .001 or .002, an edge finder is the easiest, fastest & least expensive method.


*Starrett 827B*









*Starrett 827A*






Either of those is about $20 & will last most of a lifetime.

If you're working a large OD part, where the edge finder won't fit, a wiggler is the ticket.


*Starrett S828






*With both an edge finder & a wiggler set, it's easy to find center of almost any part.


----------

